March 2006 

NASA/CR-2006-214281 

STAGS Example Problems Manual 

Norman F. Knight, Jr. 

General Dynamics – Advanced Information Systems, Inc., Chantilly, Virginia 

Charles C. Rankin 

Rhombus Consultants Group, Inc., Palo Alto, California

https://ntrs.nasa.gov/search.jsp?R=20060008654 2018-05-17T09:03:07+00:00Z
The NASA STI Program Office . . . in Profile

Since its founding, NASA has been dedicated to the 

advancement of aeronautics and space science. The 

NASA Scientific and Technical Information (STI) 

Program Office plays a key part in helping NASA 

maintain this important role. 

The NASA STI Program Office is operated by 

Langley Research Center, the lead center for NASA’s 

scientific and technical information. The NASA STI 

Program Office provides access to the NASA STI 

Database, the largest collection of aeronautical and 

space science STI in the world. The Program Office is 

also NASA’s institutional mechanism for 

disseminating the results of its research and 

development activities. These results are published by 

NASA in the NASA STI Report Series, which 

includes the following report types: 

• TECHNICAL PUBLICATION. Reports of 

completed research or a major significant phase 

of research that present the results of NASA 

programs and include extensive data or 

theoretical analysis. Includes compilations of 

significant scientific and technical data and 

information deemed to be of continuing 

reference value. NASA counterpart of peerreviewed formal professional papers, but having 

less stringent limitations on manuscript length 

and extent of graphic presentations. 

• TECHNICAL MEMORANDUM. Scientific 

and technical findings that are preliminary or of 

specialized interest, e.g., quick release reports, 

working papers, and bibliographies that contain 

minimal annotation. Does not contain extensive 

analysis. 

• CONTRACTOR REPORT. Scientific and 

technical findings by NASA-sponsored 

contractors and grantees. 

• CONFERENCE PUBLICATION. Collected 

papers from scientific and technical 

conferences, symposia, seminars, or other 

meetings sponsored or co-sponsored by NASA. 

• SPECIAL PUBLICATION. Scientific, 

technical, or historical information from NASA 

programs, projects, and missions, often 

concerned with subjects having substantial 

public interest. 

• TECHNICAL TRANSLATION. Englishlanguage translations of foreign scientific and 

technical material pertinent to NASA’s mission. 

Specialized services that complement the STI 

Program Office’s diverse offerings include creating 

custom thesauri, building customized databases, 

organizing and publishing research results ... even 

providing videos. 

For more information about the NASA STI Program 

Office, see the following: 

• Access the NASA STI Program Home Page at 

http://www.sti.nasa.gov

• E-mail your question via the Internet to 

help@sti.nasa.gov 

• Fax your question to the NASA STI Help Desk 

at (301) 621-0134 

• Phone the NASA STI Help Desk at 

(301) 621-0390 

• Write to: 

 NASA STI Help Desk 

 NASA Center for AeroSpace Information 

 7121 Standard Drive 

 Hanover, MD 21076-1320
National Aeronautics and 

Space Administration 

Langley Research Center Prepared for Langley Research Center 

Hampton, Virginia 23681-2199 under NASA Task Order NNL05AC09T 

 

March 2006 

NASA/CR-2006-214281 

STAGS Example Problems Manual 

Norman F. Knight, Jr. 

General Dynamics – Advanced Information Systems, Inc., Chantilly, Virginia 

Charles C. Rankin 

Rhombus Consultants Group, Inc., Palo Alto, California
Available from: 

NASA Center for AeroSpace Information (CASI) National Technical Information Service (NTIS) 

7121 Standard Drive 5285 Port Royal Road 

Hanover, MD 21076-1320 Springfield, VA 22161-2171 

(301) 621-0390 (703) 605-6000 
In

troduction............................................................................................................................................4

Historical Setting................................................................................................................................4

Pre-STAGS Days............................................................................................................................4

EarlySTAGS Years.......................................................................................................................5

InitialNASALangleyEfforts........................................................................................................5

Finite ElementYears......................................................................................................................6

Nonlinear Solution Procedures......................................................................................................6

Global FunctionEffort...................................................................................................................7

STAGSRestructuringEffort.........................................................................................................7

STAGSC-1Era...............................................................................................................................8

QSTAGStothe Present.................................................................................................................8

STAGSVersion5.0...........................................................................................................................9

STAGS Functional Modules.............................................................................................................9

Usage...................................................................................................................................................9

DemonstrationExample Problems.....................................................................................................10

Cook Membrane Problem................................................................................................................11

Background...................................................................................................................................11

Modeling andAnalysis Process...................................................................................................11

NumericalResults andDiscussion..............................................................................................13

STAGS Input Files.......................................................................................................................16

ProblemReferences......................................................................................................................18

Euler-Column Buckling Problem....................................................................................................19

Background...................................................................................................................................19

Modeling andAnalysis Process...................................................................................................20

NumericalResults andDiscussion..............................................................................................22

STAGS Input Files.......................................................................................................................23

ProblemReferences......................................................................................................................28

FreeVibrationof Straight Beam.....................................................................................................29

Background...................................................................................................................................29

Modeling andAnalysis Process...................................................................................................30

NumericalResults andDiscussion..............................................................................................31

STAGS Input Files.......................................................................................................................34

ProblemReferences......................................................................................................................39

FreeVibrationof Circular Ring......................................................................................................40

Background...................................................................................................................................40

Modeling andAnalysis Process...................................................................................................41

NumericalResults andDiscussion..............................................................................................42

STAGS Input Files.......................................................................................................................44

ProblemReferences......................................................................................................................51

Bucklingof Blade-Stiffened Flat Panels........................................................................................52

Background...................................................................................................................................52

Modeling andAnalysis Process...................................................................................................53

NumericalResults andDiscussion..............................................................................................57

STAGS Input Files.......................................................................................................................66

ProblemReferences......................................................................................................................79

Raasch CurvedHook Problem........................................................................................................80

Background...................................................................................................................................80

Modeling andAnalysisProcess...................................................................................................80

NumericalResults andDiscussion..............................................................................................83
2

STAGS Input Files.......................................................................................................................83

Problem References......................................................................................................................87

Buckling and Collapse of Circular Cylinder with Square Cutouts...............................................88

Background...................................................................................................................................88

Modeling and Analysis Process...................................................................................................88

Numerical Results and Discussion..............................................................................................92

STAGS Input Files.................................................................................................................... 100

Problem References................................................................................................................... 108

Scordelis-Lo Barrel Roof Problem .............................................................................................. 109

Background................................................................................................................................ 109

Modeling and Analysis Process................................................................................................ 109

Numerical Results and Discussion........................................................................................... 112

STAGS Input Files.................................................................................................................... 114

Problem References................................................................................................................... 118

Transient Response of Truncated Conical Shell ......................................................................... 119

Background................................................................................................................................ 119

Modeling and Analysis Process................................................................................................ 119

Numerical Results and Discussion........................................................................................... 122

STAGS Input Files.................................................................................................................... 126

Problem References................................................................................................................... 129

Snap-Through of Hinged Shallow Cylindrical Shell .................................................................. 130

Background................................................................................................................................ 130

Modeling and Analysis Process................................................................................................ 130

Numerical Results and Discussion........................................................................................... 132

STAGS Input Files.................................................................................................................... 141

Problem References................................................................................................................... 147

Advanced-Features Example Problems........................................................................................... 148

Buckling of Sandwich Panels....................................................................................................... 149

Background................................................................................................................................ 149

Modeling and Analysis Process................................................................................................ 150

Numerical Results and Discussion........................................................................................... 154

STAGS Input Files.................................................................................................................... 157

Problem References................................................................................................................... 173

Crack Growth Simulation for Middle-Crack Tension Panel...................................................... 174

Background................................................................................................................................ 174

Modeling and Analysis Process................................................................................................ 175

Numerical Results and Discussion........................................................................................... 179

STAGS Input Files.................................................................................................................... 191

Problem References................................................................................................................... 210

Hybrid Quasi-Static/Transient Solution Procedures Application .............................................. 211

Background................................................................................................................................ 211

Modeling and Analysis Process................................................................................................ 213

Numerical Results and Discussion........................................................................................... 214

STAGS Input Files.................................................................................................................... 218

Problem References................................................................................................................... 224

Progressive Failure Analysis of Postbuckled Shear Panel ......................................................... 226

Background................................................................................................................................ 226

Modeling and Analysis Process................................................................................................ 227

Numerical Results and Discussion........................................................................................... 228

STAGS Input Files.................................................................................................................... 233

Problem References................................................................................................................... 242
3

Membrane Wrinkling Problems................................................................................................... 243

Background................................................................................................................................ 243

Modeling and Analysis Process................................................................................................ 246

Numerical Results and Discussion........................................................................................... 249

STAGS Input Files.................................................................................................................... 257

Problem References................................................................................................................... 269

Actuator Problems......................................................................................................................... 273

Background................................................................................................................................ 273

Modeling and Analysis Process................................................................................................ 273

Numerical Results and Discussion........................................................................................... 273

STAGS Input Files.................................................................................................................... 277

Problem References................................................................................................................... 279

Summary............................................................................................................................................ 280

References ......................................................................................................................................... 280
4

Introduction

NASA Langley has been involved with shell analysis research and development for many

decades. Much of the early shell analysis research enabled space flight through the thorough

understanding of shell theory and development of computerized shell design tools. This

development occurred during an epoch when several technological advancements were taking

place; in particular, the development of electronic computations and associated numerical

methods such as finite difference and finite element methods. STAGS had its beginnings as an

Lockheed Missiles & Space Company research code and evolved into a powerful shell analysis

code offering unique capabilities such as advanced nonlinear solution procedures, load relaxation

for re-establishing equilibrium, sandwich elements, fastener elements, generalized imperfection

modeling, constraint definitions, and constitutive modeling utilities.

STAGS is an acronym for STructural Analysis of General Shells. Development of STAGS’ 

technology and analysis tools began in 1963, nearly forty years ago, at the Lockheed Palo Alto

Research Laboratory (Applied Mechanics Group) of the Lockheed Missiles & Space Company

(LMSC) in Palo Alto, CA.

* Initially casted as a finite difference code (finite elements were just

appearing and computer systems were quite limited in capability), STAGS evolved to a finite 

element code in the late 1970’s. It is based on a small-strain, large-deformation, large-rotation

energy formulation including nonlinear material behavior. Historically STAGS has been a shell

analysis tool; however, three-dimensional nonlinear analysis capabilities have been incorporated

in recent years. STAGS continues to serve as both a structural mechanics research tool for shell

analysis and nonlinear mechanics as well as an advanced structural analysis tool for aerospace

structures.

Historical Setting

A brief historical summary of the development of the STAGS shell analysis code is given here.

This summary is not intended to review all shell analysis work but rather those aspect

contributing to computerized shell analysis and the STAGS code. The summary covers the early

LMSC effort through the current effort resulting in STAGS Version 5.0. Reference citations to

STAGS documents are given when they can be identified.

Pre-STAGS Days

Computer analysis of shell structure was well under way in the early 1960’s at LMSC. NASA

Marshall Space Flight Center sponsored some of the early shell analysis formulations and

implementations from 1963 to 1968 [1-3]. Much of the work focused on developing equilibrium 

equations for cylinders, cones and spheres and then applying finite difference approximations to

arrive at a set of algebraic equations to solve using matrix algebra. However, the system of

equations was unsymmetric. Another aspect of the work investigated the use of an energy

formulation to pose the buckling problem wherein finite difference approximations are used for 

derivative terms. Stationary conditions on the energy functional then gave rise to a symmetric set

of nonlinear algebraic equations. This approach, led by Bo O. Almroth, was a significant

advancement and provided the basis for future shell analysis tools developed at LMSC and

elsewhere.

 * This organization is now the Lockheed Martin Advanced Technology Center of Lockheed Martin

Missiles & Space (LMMS).
5

Following the NASA Marshall Space Flight Center contract, LMSC continued their shell analysis

research and development work under internal research and deveopment funding. During this

time, methods research computer codes were developed, extended and sometimes abandoned.

Most likely, an internal LMSC research code called STAGS came into being while not formally

released - like many of our own special-purpose research codes. However, this work was not

done in a vacuum either. Government agencies, in particular the military, were also involved in

shell analysis research.

In should be noted that other shell analysis research was also underway during this time including

others at LMSC, NASA, AFFDL, NSRDC, and many universities. However, much of this work

was directed towards shells of revolution and not general shell structures. Shell analysis codes

such as BOSOR, FASOR, SRA, GIRLS, SALORS and others were developed during this period.

Early STAGS Years

STAGS initial development was an outgrowth of LMSC work sponsored by NASA Marshall

Space Flight Center in 1963. NSRDC sponsored work at LMSC that resulted in an analysis

capability for stiffened shells with cutouts [4, 5]. Then the Air Force (SAMSO and AFFDL)

sponsored additional work including bifurcation buckling, thermal effects, plasticity, and general

coordinate systems [6]. The work on arbitrary non-orthogonal coordinates led by Marlowe was

based on his PhD work with Flugge at Stanford University [7]. The geometrically nonlinear 

equations were discretized using a half-station finite difference approach where was defined at

the nodes and u and v were defined at half-station points. The resulting code called STAGSA

(some use STAGS-A) was released in 1972 to the structural analysis community. Formal users

documentation was released through AFFDL in 1973 [8, 9].

During this period, competition between research groups was very keen. Selected shell analysis

problems were defined and tossed down as challenges and provide, even today, a gauntlet of 

difficult nonlinear shell analysis problems. References 11-13 are cited as key references from

this period.

Initial NASA Langley Efforts

NASA Langley funding of STAGS-related efforts appears to have begun in the early 1970’s -

although this date is somewhat uncertain because of NASA Langley’s involvement with the

BOSOR development at LMSC. Dr. Paul Cooper was the first NASA LaRC contract monitor for

shell analysis work at LMSC, followed by Dr. James Starnes, Dr. Wendell Stephens, Dr. Jerrold

Housner, Dr. Gaylen Thurston, Dr. James Starnes, and finally Dr. Richard Young.

To resolve some issues present in STAGSA, a new version, STAGSB, was developed based on a 

modified finite difference approach with all displacement unknowns at grid points (whole-station

finite difference approach). STAGSB was released in 1974 [14]. STAGSB also permitted the

use of segmented or branched shells.

Then because finite element technology was maturing, a comparative study between the finite 

difference and finite element approaches for nonlinear shell collapse problems was needed. This

study was enabled, in part, by STAGSC [15, 16], an analysis code with the whole-station finite 

difference approach having different areas of integration for bending and membrane energy

contributions and also the first implementation of shell finite elements. Other LMSC shell finite 

element analysis work (e.g., REXBAT) began to be implemented with the STAGS code. The 4-

node QUAF (quadrilateral flat) element originated by Almroth and Brogan from a combination of 
6

the Melosh QB12 bending element [17] with the Willam membrane element [18]. Tuning this

element (410 element) has occurred over the years, and it remains the workhorse shell element of 

STAGS [19]. The Ahmad thick shell elements [20] were added for isotropic shells. Basic

plotting capabilities such as finite element geometry, deformed shapes, and contour plots were 

developed and called STAPL by leveraging on NASA LaRC work [21].

Finite Element Years

STAGSC-1 represented the first complete finite-element-only version of STAGS [22]. In 1981,

Almroth and Brogan evaluated the STAGS finite element capabilitiues and compiuational

efficiencies [23]. Early in the STAGSC-1 development, an evaluation of STAGSC-1 was

performed by Thomas and Sobel in 1981 [24]. Their report discussed many test cases and

documented some of the internal programming aspects of STAGS, which had never been

documented before. Woytowitz [25] also released a sample problems manual providing some 

illustrative examples of STAGS usage.

Unfortunately, Bo Almroth’s death in February 1983 left a major void in the STAGS

development team. After some time, Dr. Charles Rankin emerged as the LMSC contact for 

STAGS and structural mechanics research and development continued. This time period also saw

a shift towards more focused program support and less basic research. Ref. 26 is a collection of

papers honoring Bo Almroth.

Several releases of STAGSC-1 occurred during the 1980’s without any name change or version

number except the release date printed in the output. For the most part, NASA Langley was the

primary sponsor of the mechanics technology implemented in STAGS including arc-length

control [27-30], corotation formulation [31-34], nonlinear springs [33], contact [34], and the

Thurston bifurcation processor based on the equivalence transformation [35-37].

During this same time period, NSRDC funded the development of STAGS-2000 which was to be

a modern version of STAGS based on a database manager developed by Peter Stehlin. It was to

be completely modular and consistent with software standards for extendibility and

maintainability. This version was never installed at NASA Langley.

Nonlinear Solution Procedures

Nonlinear solution procedures are cornerstone concepts of the STAGS shell analysis code. From

STAGS’ initial beginnings, nonlinear solution procedures have been played a significant role in

advancing shell analysis technology. Shell collapse using nonlinear methods was considered first

followed by bifurcation buckling methods as an alternative approach to collapse analyses.

The nonlinear analysis procedures implemented within STAGS are based on an incremental

iterative procedure using the Newton-Raphson approach. STAGS takes great care to formulate 

and evaluate consistent first and second variations of the energy functional. Both full and

modified Newton-Raphson implementations are available. Because of the speed of the sparse 

matrix equation solver, the use of a full Newton-Raphson approach for even very large problems

(>100,000 degrees of freedom) has become routine. Each solution step requires an initial “guess” 

or starting solution. STAGS uses the previous step’s converged solution as the initial guess until

three converged solutions are obtained. Then quadratic extrapolation can be used to form the 

initial guess for the next step. Solution control sensors include error norms based on the iterative 

change in the solution and on the residual or imbalance forces. During the iterative process for 

each step, these error indicators, total elastic energy, determinant of the stiffness matrix,

maximum component in the residual vector are printed. These values can be monitored and

provide some added insight into the overall behavior of the structure.
7

STAGS offers three different solution control procedures: load control, displacement control, and

arc-length control. STAGS has offered the arc-length-control procedure developed by Riks since

the early 1980’s. The direct involvement of Dr. Riks with LMMS staff over the years has led to

very robust, accurate, and stable nonlinear solution procedures. The arc-length constraint

equation implemented within STAGS is based on the normal-plane constraint equation which has

been very reliable for a wide range of nonlinear problems. The implementation does not solve 

the constraint equation (which is quadratic) directly as Crisfield does because of the questions

surrounding which root of the quadratic equation to use. STAGS solves the constraint equation in

a manner analogous to the approach used to solve the nonlinear equilibrium equations - expand in

a Taylor series. This approach provides a very robust method for selecting the appropriate path

rather than heuristics for root selection. STAGS is capable of solving nonlinear problems

including those exhibiting snap-through and snap-back behavior.

Global Function Effort

In attempt to reduce the computational cost associated with nonlinear shell analysis, Almroth et

al. [38, 39] proposed the use of global functions as a Rayleigh-Ritz procedure on the discretized

global system of equations. In this approach, the vector of nodal degrees of freedom is

transformed to a “reduced system” through the use of transformation matrix. The columns of the

transformation matrix are essentially previous nonlinear solutions for the “full system” or global

functions. RRSYS implemented the global function approach as a predictor using the reduced

system and STAGSC-1 as the corrector for a reduced system formulation using the full system

for nonlinear static problems.

This formulation provides an effective solution procedure for problems that do not exhibit any

path dependence due to material nonlinearities or mode jumping. If the solution throughout the 

range of loading exhibits a self-similar behavior, then reduction methods are attractive. However

as a solution procedure for general structural analysis problems, the limitations restricted its

further development to academic issues.

STAGS Restructuring Effort

Early STAGS development (pre-STAGS through STAGSC; early 1960’s through mid 1970’s)

evolved from an LMSC internal research computer code to a computer code distributed outside 

LMSC. STAGS had a demonstrated capability for solving practical aerospace shell structures

problems. Mechanics research was driven by space applications and military funding. Research

directions were generally set by the sponsor in concert with Lockheed; however, LMSC had

considerable flexibility in their STAGS methods research thrusts.

The early STAGS development team was a small core group (4-6 people) from Lockheed with

technical interaction from their government sponsors. Few researchers outside of Lockheed

waded into the actual STAGS source code. Sponsoring agencies tended to be more focused on

extending features, adding new capabilities, and developing advanced methods rather than on the

more mundane, albeit necessary, tasks associated with software maintenance, documentation, and

migration to newer computer systems. This tendency resulted in limited theoretical and system

documentation. In addition and perhaps more critical is the fact that during this period, most

methods developers (not just STAGS developers) were more focused on the methods work rather 

than software maintainability and longevity of their computer code. As a result, computer codes

evolved into very difficult programming environments to maintain (i.e., the era of “spaghetti” 

codes).
8

The early period of STAGS development was also the early period of computing systems

development. As a result, programming techniques and standards were just developing and

attention focused on computer memory management and computational efficiency. STAGS

development work proceeded from a UNIVAC computer system to a DEC VAX VMS computer

system. During this same period, commercial finite element codes were also under development

focusing on general-purpose structural analysis needs.

STAGSC-1 Era

Later STAGS development (STAGSC-1 era extends from the mid 1970’s through the early

1990’s) continued along the same path with the primary sponsor being the NASA Langley

Research Center. Structural mechanics research was driven by aerospace applications. Research

directions were still generally set by the sponsor in concert with LMSC; however, LMSC still had

considerable flexibility in their methods research thrusts.

The STAGS development environment did not change significantly. Lockheed had 3-4 people 

working on STAGS with about that many more working on related projects (e.g., modeling and

analysis tasks, coupling STAGS to the underwater shock analysis code USA to form USASTAGS). Sponsoring agencies continued to be more focused on extending features, adding new

capabilities, and developing advanced methods rather than on software infrastructure tasks

although an awareness of its importance had emerged.

Computing systems had evolved some during this period. Lockheed was using a VAX VMS 

computer system as their main development environment while NASA LaRC had access only to

CDC Cyber-class computers. Computer-word-length issues (i.e., 32-bit versus 60-bit words;

single versus double precision) related to data and memory management needed to be addressed

relative to the impact on accuracy, computational speed, and overall solution efficiency.

Software changes to STAGS were delivered to NASA LaRC periodically in UPDATE-format

with either bug fixes or new features or both. The NASA LaRC contact person then installed the 

updates on NASA computers (or arranged for installation) and notified STAGS users of the new

version.

QSTAGS to the Present

In 1984, NASA Langley initiated a new activity called the Computational Structural Mechanics

or CSM. Its aim was to define the next generation of structural analysis tools and provide a 

framework for structural mechanics research. LMSC served as the prime contractor for this

activity for a 5-year period from 1987 to 1992. The STAGS work at LMSC continued under

independent funding from NASA Langley. As a result, a new restructured STAGS emerged

called QSTAGS or quick STAGS that in essence was STAGS Version 1.0 in the current naming

convention. QSTAGS then served as the main research version of STAGS at LMSC for a few

years as new capabilities and old restrictions (e.g., limit on the number of shell units) were

removed.

In the mid 1980’s, LMSC worked to transform the STAGS internal architecture from a file-based

system (i.e., TAPE21 and TAPE22 or the MOD and SOD files, respectively) to a database

system. This conversion enabled the technology transfer from STAGS to the CSM Testbed. In

1988, NSRDC sponsored the development of a STAGS-to-Testbed interface in order to provide 

them a mechanism to transfer their STAGS finite element models to the CSM Testbed.

In 1994, STAGS Version 2.0 was released. This version represented a major software 

enhancement with significant portions of the code being re-written. In addition, the STAGS users
9

documentation was overhauled. Additional versions were released nearly every year until

Version 2.4 was released in 1997.

Some of the major new features in this version included the Generic Constitutive Processor or 

GCP for constitutive research, the 9-node ANS element, mesh refinement transition elements

(E510 and E710) for the E410 shell element, new STAGS database access routines, crack growth

analysis tools, load relaxation and hybrid static/transient analysis option and various postprocessing features for results displays, xy-plotting, and access to PATRAN or I-DEAS.

MSC.Software, Inc. was also contracted to provide a STAGS-preference with PATRAN for 

developing STAGS finite element models and results post-processing.

The current STAGS development strategy (QSTAGS through current version; mid 1990’s to

present) has not changed significantly over the past decade. Historically, the STAGS 

development team has always been a small core group from Lockheed with technical interaction

from their government sponsors. However, many of the STAGS key developers are now retired

and work as consultants.

STAGS Version 5.0

STAGS Version 5.0 is the current release of STAGS. This version has been available for

approximately two years and represents a complete integration of various developments by the 

STAGS key developers as well as others. New capabilities include user-defined materials, userdefined elements, user-defined fabrications, progressive failure methodologies, actuator elements,

Stein-Hedgpeth membrane wrinkling model, and Hahn nonlinear elastic material model. New

documentation has been generated as well. STAGS is available on several UNIX systems (SUN,

SGI, and HP), on the Apple OS X, and on both 32-bit and 64-bit Linux systems. Documentation

supporting STAGS Version 5.0 is given in References 65-74.

STAGS Functional Modules

STAGS is actually a small set of executable computer programs (S1, S2, and STAPL). Users

typically execute the S1 processor to read basic finite element modeling data and build essential

geometry and material tables. The S2 processor performs the element stiffness evaluations,

global assembly of vectors and matrices, application of boundary conditions, matrix

decompositions, solution procedures (linear or nonlinear, static, transient, or eigenvalue), and

recovery of secondary fields. The STAPL processor is a stand-alone, static graphical tool for

undeformed and deformed geometry plots as well as contour plots. The XYTRANS processor 

creates xy-plotting data from the STAGS databases directly. The PITRANS processor creates

ASCII files from the STAGS databases for post-processing by PATRANS or I-DEAS. User

documentation includes four manuals - two are preliminary forms. Much of the formulation and

development for the newer features are documented directly in the users manual. Some basic 

training materials were developed about 10 years ago.

Usage

STAGS usage is essentially the same as any other finite element analysis code. The user prepares

the input, submits the input file to STAGS propcessors for execution, and once execution is

completed, post-processes the numerical results. Three input files are typically defined. The 

STAGS S1 processor reads an input file with an extension *.inp (e.g., my_problem.inp).

The S1 processor evaluates the geometry data, boundary conditions, loading definitions,

constraints, and other finite element data. Successful execution of the S1 processor results in the 

generation of a PDF file of the problem finite element model in the file my_problem_m.pdf.
10

Next, the STAGS S2 processor reads an input file with an extension *.bin (e.g.,

my_problem.bin). The S2 processor is the computational processor and performs the finite 

element solution based on the parameters contained in the *.bin file. Postprocessing can be 

accomplished using the STAGS STAPL processor for batch graphical files generation. The 

STAPL processor can be executed as an interactive command and the user provides answers to

STAPL queuries, which generates an input file with the extension *.pin (e.g.,

my_problem.pin). This is a simple way to generate a new STAPL input file that may be used

to generate many plots by copying the input generated by the interactive approach and editting

the lines for additional plots. Batch execution usually follows and a PDF file results that can be 

viewed.

Demonstration Example Problems

A series of commonly used demonstration problems are described, modeled, analyzed, and results

presented. STAGS capabilities to solve these demonstration problems are illustrated through

results comparison withavailable reference solutions and/or finite element mesh refinement

studies. Each demonstration problem is first described and background information provided.

The modeling and analysis process using STAGS is then described. Numerical results are

presented and compared to reference solutions. Listings of selected STAGS input files are given

for completeness and easy reference for the reader. References specific to each demonstration

problem are provided to close each section.
11

Cook Membrane Problem

Background

The membrane problem posed by Cook (1987) involves a trapezoidal-shaped membrane fixed

along one edge and loaded by in-plane shear loading along the opposite edge. The geometry of 

the membrane has the appearance of a swept-wing plan-form as shown in Figure 1. The

dimensions, material properties and loading are defined in Figure 1 using U. S. customary units.

Figure 1. Cook membrane problem: geometry, material properties, and loading.

The membrane has a unit thickness and a unit in-plane shear load along the vertical edge at x=48

inches. The four corners of the membrane (starting at the origin and moving in a clockwise 

manner) have (x,y) coordinate values in inches of (0, 0), (0, 44), (48, 60), and (48, 44) – all

coordinates are given in inches. This problem provides a good measure of the robustness of the 

elements since the fixed-end of the panel and its shape cause a stress gradient throughout the 

membrane, and it is frequently used to assess membrane elements (e.g., see Davis, 1995). The 

reference solutions obtained by Ibrahimbegovic, Taylor and Wilson (1990) for stresses and Cook

(1993) for deflections are used for comparison.

Modeling and Analysis Process

The STAGS model is generated using a single shell unit with the quadrilateral plate surface

geometry (ISHELL=3). Material properties and membrane construction are defined using both

the historical STAGS approach and the current GCP approach. Mesh discretization studies

include different levels of mesh refinement and different element types. Mesh refinement is

readily performed by changing the number of nodes N in each direction on the F-1 record (i.e.,

the mesh is defined as N×N mesh of nodes). Element type is selected using the N-1 record

(KELT). Representative finite element meshes using 3-node, 4-node and 9-node shell elements

are shown in Figure 2.

x, u

y, v

P

48 in.

16 in.

44 in.

P = 1 lb.

E = 1 psi

ν = 1/3

h = 1 in.

Boundary Conditions

u(0,y)=0

v(0,y)=0

A

B C
12

4-node E410 quadrilateral shell element.

9-node E480 (9ANS) quadrilateral shell element.

3-node E330 (MIN3) triangular shell element.

Figure 2. Representative finite element discretizations for N=11
13

Material modeling for an elastic isotropic material using the historical STAGS approach requires

data on the I-1 and I-2 records to define the material properties and the K-1 and K-2 records to

define the construction or fabrication data. Material modeling using the current GCP approach

requires data on the I-5a and I-6a records to define the material properties and the I-5a, I-21a, I21b, I-21c, I-21d, and I-21e records to define the fabrication.

Loading is specified as a uniformly distributed shear load across the right end of the membrane.

It is specified as a line load (Nxy = 1/16 lb/in.) using the Q-1, Q-2, and Q-3 records. As a check

on the loading, the summation of the equilibrium forces across the loaded edge in the direction of 

applied loading should equal unity (i.e., total force equal to edge length times line load).

Boundary condition on the displacements are specified using the P-1 and P-2 records. All out-ofplane degrees of freedom are suppressed since only a membrane response is needed. The drilling

degrees of freedom are suppressed for the E330 and E480 elements but they are retained for the

E410 element. These freedoms are constrained using the Q-3 records with the exterior looping

feature (see sample S1 input file).

Numerical Results and Discussion

Results are presented for the tip deflection at point C (48, 52) in the y-direction denoted by vc and

the reference solution of Cook (1993) is 23.91 inches. Results are presented for the maximum 

principal stress at point A (24, 22) denoted by σA and the reference solution by Ibrahimbegovic et

al. (1990) is 0.237 psi. Results are also presented for the minimum principal stress at point B (24,

52) denoted by σB, and the reference solution by Ibrahimbegovic et al. (1990) is –0.202 psi. The

principal stresses at a point for a plane stress problem are computed using:

( )

2

2

1,2 max max 2 and 2 xy

x y x y !

" "

! !

" "

" + #

#

$

%

&

&

'

( )

± =

+

=

These computations have been incorporated into the stress output subroutines for the E410

element in the STAGS S2 processor.

Tip displacement results shown in Table 1 indicate that models using the E480 9ANS shell

element converge quickly to the reference solution, while models using the E330 and E410 shell

elements converge at a slower rate. For the E480 element, the membrane response is

approximated in a biquadratic manner. For the E410 element, the membrane response is nearly

bilinear except for the contribution of the drilling degrees of freedom. Since every element in the

finite element mesh is a trapezoid, element sensitive to mesh distortion is clearly evident. Effort

should be expended by the analyst to minimize element distortion when using the E410 element

in a membrane dominant problem. Contour plot of the v-displacement component is shown in

Figure 3.
14

Table 1. Mesh refinement study for three shell elements in STAGS – reference solution is 23.91 inches

(Cook, 1993).

Number of Nodes Tip Deflection at Point C, vc (inches)

per Edge, N E330 Element E410 Element E480 Element

3 9.897 11.101 22.735

5 16.297 17.697 23.618

7 19.493 20.562 23.813

9 21.105 21.836 23.886

11 22.001 22.512 23.911

13 22.537 22.910 23.925

15 22.885 23.163 23.932

17 23.118 23.334 23.937

19 23.285 23.454 23.940

21 23.405 23.542 23.942

Figure 3. Contour plot of the v-displacement component from the linear solution for N=11 and

the E410 element.

23.1

0

x, u

y, v

(inches)
15

Figure 4. Contour plot of the maximum principal stress component from the linear solution for 

N=11 and the E410 element.

Figure 5. Contour plot of the minimum principal stress component from the linear solution for 

N=11 and the E410 element.

0

-0.248

(psi)

0.224

-0.05 (psi)
16

Principal stress values near Points A and B for the N=11 mesh using the E410 element are

consistent with the reference values. The principal stress distributions are shown in Figures 4 and

5 for the N=11 mesh of E410 elements. Values taken at element integration points from either 

size of these reference locations (see Figure 2a) are:

Near Point A: Element 41 = 0.222; Element 51 = 0.223 (Point A Ref. Value = 0.237)

Near Point B: Element 50 =-0.184; Element 60 =-0.186 (Point B Ref. Value =-0.202)

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Cook

Typical 2D Shell Model Input Files

The following text files give the input for the plane stress membrane model using the E410 4-

node shell element in STAGS with eleven nodes per edge (N=11).

cook2D.inp (for S1 processor)

COOK TRAPEZOIDAL MEMBRANE PROBLEM $A-1

C

C TRAPEZOIDAL MEMBRANE WITH INPLANE SHEAR TIP LOAD

C

C REF.: COOK, "AN ELEMENT ERROR INDICATOR AND A RELATED

C STRESS-IMPROVEMENT PROCEDURE," COMM. IN NUMERICAL

C METHODS IN ENGINEERING, VOL. 9, 1993, PP. 207-217.

C

C MODEL INPUT CONTROLS

0 0 1 0 0 0 0 $B-1

1 10*0 $B-2

1 0 1 0 0 1 $B-3 INCLUDE GCP INPUT

11 11 $F-1 DISCRETIZATION: NROWS, NCOLS OF NODES

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

1.0 0.33 0.0 0.10 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

1.0, $I-6A YOUNG'S MODULUS, PSI

0.33, $I-6A POISSON'S RATIO

2.588E-4, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

1.0 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 1.0 0.0 0 $K-2 LAYERED WALL

C

C SHELL UNIT 1 MODEL DEFINITION

C
17

3 0 4*0 $M-1 QUADRILATERAL PLATE GEOMETRY

0.0 0.0, $M-2 (X1, Y1)

0.0 44.0, $M-2 (X2, Y2)

48.0 60.0, $M-2 (X3, Y3)

48.0 44.0 $M-2 (X4, Y4)

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 DISCRETIZATION RECORD, ELEMENT SELECTION

2 0 0 0 $P-1 EDGE 1 IS CLAMPED

110 000 $P-2 EDGE 2 IS FREE INPLANE, OTHERWISE FIXED

110 000 $P-2 EDGE 3 IS FREE INPLANE, OTHERWISE FIXED

110 000 $P-2 EDGE 4 IS FREE INPLANE, OTHERWISE FIXED

1 0 0 0 $Q-1 LOADING SUMMARY

1 2 0 $Q-2 LOAD SET SUMMARY

-0.0625 2 2 11 0 0 $Q-3 NXY=1/16 LB/IN ACROSS RIGHT END

0.0 -1 3 0 0 0 3 1 0 0 $Q-3 EXTERIOR LOOPING TO SET

C OUT-OF-PLANE DOF TO ZERO

1 1 0 1 $R-1 OUTPUT CONTROL FOR SHELL UNIT 1

cook2D.bin (for S2 processor)

COOK TRAPEZOIDAL MEMBRANE PROBLEM $A-1

0 1 5*0 -1 $B-1 ANALYSIS CONTROL

1.0 $C-1 LOAD MULTIPLIERS

cook2D.pin (for STAPL processor)

Cook Membrane problem $A-1

6 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C plot undeformed geometry with global node numbers

0 0 6 0 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0 $PL-6 rotations

C plot undeformed geometry with global element numbers

0 0 1 0 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0 $PL-6 rotations

C plot deformed and undeformed geometry

1 0 1 0 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0 $PL-6 rotations

C plot v-displ contours on deformed geometry

2 0 1 0 0 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0 $PL-6 rotations

C plot S1P principal stress on the deformed geometry

2 0 7 0 0 0 0 7 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0 $PL-6 rotations

C plot S2P principal stress on the deformed geometry

2 0 7 0 0 0 0 8 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0 $PL-6 rotations
18

Problem References

Cook, R. D., “A Plane Hybrid Element with Rotational D. O. F. and Adjustable Stiffness,”

International Journal for Numerical Methods in Engineering, Vol. 24, 1987, pp. 1499-1508.

Cook, R. D., “An Element Error Indicator and a Related Stress-Improvement Procedure,” 

Communications in Numerical Methods in Engineering, Vol. 9, 1993, pp. 207-217.

Ibrahimbegovic, A., Taylor, R. L., and Wilson, E. L., “A Robust Quadrilateral Membrane Finite 

Element with Drilling Degrees of Freedom,” International Journal for Numerical Methods in

Engineering, Vol. 30, 1990, pp. 445-457.

Davis, Timothy S., Assessment of High-Order Serendipity and Lagrangian Quadrilateral

Membrane Elements, Master’s Thesis, Department of Aerospace Engineering, Old Dominion

University, Norfolk, VA, December 1995.
19

Euler-Column Buckling Problem

Background

Stiffened panels are a common configuration in the aerospace industry. Modeling the stiffeners

affects the buckling predictions. For stiffened panels exhibiting overall buckling behavior, the 

stiffeners participate with the panel skin in the buckling mode. As a result, the stiffener models

need to be capable of modeling an in-plane buckling behavior (i.e., in the x-y plane). For beam 

models, this represents an Euler column-buckling problem about a specific axis of the beam

cross-section. For plate models, the finite elements need to be capable of exhibiting in-plane 

buckling behavior. The geometry, material properties, and loading of the column are defined in

Figure 6 using U. S. customary units.

Figure 6. Euler column buckling problem: geometry, material properties, and loading.

h

t

L

x

y

E = 10.0 Msi

ν = 0.0

L = 30.0 in.

h = 1.0 in.

t = 0.05 in.

Nx0 = -1000 lb/in.

A = ht

J t h

I

I th

I t h

yz

zz

yy

3

3

3

3

1

0

12

1

12

1

=

=

=

=
20

The analytical solution for linear bifurcation buckling of a long slender column simply supported

at its ends is given by Brush and Almroth (1975):

2 0

2

Euler x

cr Euler

x N

hL

EI

h

P

N ! "= = =

where E is Young’s elastic modulus (10 Msi), Izz is the moment of inertia equal to

/ 12 3 th

(.0041666 in.

4

), L is the column length (30 in.), t is the column thickness (0.05 in.), h is the

column width (1.0 in.), and

Nx0

is the uniform compressive longitudinal pre-stress value (-1000

lb/in.). Using these values, the critical buckling factor 

! Euler

evaluates to:

0.456926

108

5 2

= =

! " Euler

The buckling mode shape corresponds to a single half wave along the column length (n=1). The 

higher eigenvalues and corresponding mode shapes are in proportion to the factor n

2

; that is,

2

2

2

L

EI P n n!

=

Hence the first four eigenvalues will be a multiple of 

! Euler

by factors of 1, 4, 9, and 16,

respectively.

Modeling and Analysis Process

Three separate STAGS finite element models are considered in this test case problem: 1D beam 

model, 2D plate model, and 3D solid model. Each model has 31 equally spaced nodes along the 

column length. These finite element models are shown in Figure 7. A summary of each model

includes:

1. Beam model – Model the column using discrete beam elements in an element unit. This model

will predict general buckling mode shapes – no cross-sectional deformation of the column.

2. Plate model – Model the column with plate elements in a single shell unit.

3. Solid model – Model the column with solid elements in a single shell unit

Material properties and laminate construction are defined using both the historical STAGS

approach (i.e., STAGS versions prior to GCP) and the current GCP approach. Material modeling

for an elastic isotropic material using the historical STAGS approach requires data on the I-1 and

I-2 records to define the material properties and the K-1 and K-2 records to define shell

fabrication data. Material modeling using the current GCP approach requires data on the I-5a and

I-6a records to define the material properties and the I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e 

records to define the fabrication. Note that a zero Poisson ratio is used in the 2D and 3D analyses

in order to correlate with the 1D beam-column solution – no biaxial stress. Also the current GCP

implementation does not support beam elements. Hence beam cross-sectional properties (A, Iyy,

Izz, J) are defined using the J-1 and J-2 records.
21

Figure 7. Finite element models studied for the Euler column buckling problem.

(a) Beam model. (b) Plate model. (c) Solid model.
22

Loading is specified as an applied end shortening at the x=0 end of the column using the Q-1, Q2, and Q-3 records. Boundary condition on the displacements are specified using the P-1 and P-2

records for the plate model. For the beam model, the boundary conditions are specified on the 

user point record (S-1 record). The boundary conditions are such that buckling about the “strong”

axis occurs as the lowest buckling mode. For the plate and solid models, two sets of boundary

conditions are needed: one to generate the pre-stress state and another to simulate in-plane 

simple-support boundary conditions. All degrees of freedom associated with out-of-plane

displacements and bending rotations are suppressed.

Numerical Results and Discussion

The pre-buckling stress distributions is specified rather than computed. For a pre-stress in-plane 

longitudinal stress resultant loading of Nx0=1000 lb/in. In order to apply the loading in the same 

manner for the three idealizations considered (1D, 2D, and 3D), an applied end shortening δ at

one end of the column is specified. For the uniform pre-stress state, the corresponding end

shortening is:

0.06 in. 0= =

Et

Nx L !

The eigenvalue analysis has a convergence tolerance of 10-4and the number of eigenpairs

requested is four. No shift is used in the eigen solution.

Results of the STAGS analyses are summarized in Table 2 where the eigenvalues are normalized

by the first analytical eigenvalue ! Euler . The first eigenvalue agrees very well with the analytical

solution. Contour plots of the eigenvectors or mode shapes for the 2D plate model are shown in

Figure 8. The displacement component v in the y direction are shown in the figure.

Table 2. Normalized Eigenvalue Solutions for Euler Column Buckling Problem.

Normalized Eigenvalues, ! ! Euler

n Analytical

Solution

1D Beam Model

– E210

2D Plate Model

– E410

3D Solid Model

– E885

1 1 1.0000 0.9953 0.9970

2 4 4.0000 3.9555 3.9520

3 9 9.0001 8.8057 8.7633

4 16 16.0011 15.4280 15.2780
23

Figure 8. Contour plots of the in-plane displacement component v

of the mode shapes from the 2D plate model.

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Euler-column

1D Beam Model Input Files

euler1d.inp (for S1 processor)

Euler column-buckling problem - 1-D model $A-1

C

C Thin strip, Euler column buckling from uniform axial compression

C

C REF.: Brush and Almroth, "Buckling of Bars, Plates

C and Shells," 1975.

C

C MODEL INPUT CONTROLS

0 0 1 0 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 -90.0 $B-1b model rotations

0 1 0 $B-2

1 1 1 0 0 1 $B-3 USE GCP INPUT

C

C Define Element Unit data

C

32 0 30 0 0 0 $h-1 No. of points and No. of beam elements

C

Mode 1

with one

half wave

Mode 2

with two

half waves

Mode 3

with three

half waves

Mode 4

with four

half waves

+1.0

-1.0
24

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1(HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.10 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

2.588E-4, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

0.05 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C Beam cross-sectional properties

C

1 1 1 0 4.1666E-5 0.0 0.0 0 0 0 $j-1

0.05 1.041666E-5 4.1666E-3 0.0 $j-2

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 0.05 0.0 0 $K-2 LAYERED WALL

C

C ELEMENT UNIT 1 MODEL DEFINITION

C

1 0 0 0 0.0 0.0 0.0 100 001 $s-1 end point at x=0

2 0 0 0 1.0 0.0 0.0 110 001 0 29 0 $s-1

1 0 0 0 1.0 0.0 0.0 $s-1a incrementation

31 0 0 0 30.0 0.0 0.0 000 001 0 $s-1 end point at x=L

32 0 0 0 15.0 1.0 0.0 111 111 $s-1 reference node

C

C Generate beam elements

C

1 2 32 210 1 0.0 0.0 0.0 0 0 30 $T-2

1 1 0 $T-2a generate 30 elements

C

C generate loads - applied end shortening

C

1 0 $u-1 Loads summary

1 1 0 $u-2 Load set summary

6.0e-2 -1 1 1 $u-3 end shortening at x=0 end

1 0 0 $v-1 output control

euler1d.bin (for S2 processor)

Euler column-buckling PROBLEM $A-1

C

C Thin strip, Euler column buckling from uniform axial compression

C

C REF.: Brush and Almroth, "Buckling of Bars, Plates

C and Shells," 1975.

C

1 1 0 0 0 0 0 -1 $b-1 buckling analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control
25

4 $d-3 cluster definition

2D Plate Model Input Files

euler2d.inp (for S1 processor)

Euler column-buckling problem - 2D model $A-1

C

C Thin strip, Euler column buckling from uniform axial compression

C

C REF.: Brush and Almroth, "Buckling of Bars, Plates

C and Shells," 1975.

C

C MODEL INPUT CONTROLS

0 0 1 0 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 -90.0 $B-1b model rotations

1 10*0 $B-2

1 0 1 0 0 1 $B-3 INCLUDE GCP INPUT

31 5 $F-1 DISCRETIZATION: NROWS, NCOLS OF NODES

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.10 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

2.588E-4, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

0.05 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 0.05 0.0 0 $K-2 LAYERED WALL

C

C SHELL UNIT 1 MODEL DEFINITION

C

2 0 4*0 $M-1 Rectangular PLATE GEOMETRY

0.0 30.0 0.0 1.0 $M-2 L=30 in.; h=1.0 in.

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 DISCRETIZATION RECORD, ELEMENT SELECTION

0 0 0 0 1 $P-1 EDGEs 1 & 3 simple support; Edges 2 & 4 free

100 001

110 001

000 001

110 001

0 0 0 0 $P-1 EDGEs 1 & 3 simple support; Edges 2 & 4 free

100 001

110 001

100 001

110 001

1 0 0 0 $Q-1 LOADING SUMMARY - force inplane buckling

1 4 $q-2
26

6.0e-2 -1 1 1 0 0 $q-3 u=constant at x=0

0.0 -1 3 0 0 0 $q-3 w=0 everywhere

0.0 -1 4 0 0 0 $q-3 ru=0 everywhere

0.0 -1 5 0 0 0 $q-3 rv=0 everywhere

1 1 0 0 $R-1 OUTPUT CONTROL FOR SHELL UNIT 1

euler2d.bin (for S2 processor)

Euler column-buckling PROBLEM $A-1

C

C Thin strip, Euler column buckling from uniform axial compression

C

C REF.: Brush and Almroth, "Buckling of Bars, Plates

C and Shells," 1975.

C

1 1 0 0 0 0 0 -1 $b-1 buckling analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control

4 $d-3 cluster definition

euler2d.pin (for STAPL processor)

Euler column-buckling problem - uniform compression

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0

2 0 4 0 2 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0

2 0 4 0 3 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0

2 0 4 0 4 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0

3D Solid Model Input Files

euler3d.inp (for S1 processor)

Euler column-buckling problem - 3D solid model $A-1

C

C Thin strip, Euler column buckling from uniform axial compression

C

C REF.: Brush and Almroth, "Buckling of Bars, Plates

C and Shells," 1975.

C

C MODEL INPUT CONTROLS

0 0 1 1 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 -90.0 $B-1b model rotations

1 10*0 $B-2

1 0 1 0 0 1 $B-3 INCLUDE GCP INPUT

31 5 $F-1 DISCRETIZATION: NROWS, NCOLS OF NODES

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.10 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION
27

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

2.588E-4, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SOLID_FABRICATION 1 1 0 $I-5A GCP Solid Fabrication Record

0.05 $I-22a element thickness

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

0.05 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 0.05 0.0 0 $K-2 LAYERED WALL

C

C UNIT 1 MODEL DEFINITION (one solid element thickness thickness)

C

2 0 0 0 1 1 $M-1 Rectangular PLATE GEOMETRY

0.0 30.0 0.0 1.0 $M-2 L=30 in.; h=1.0 in.

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

885 0 0 $N-1 DISCRETIZATION RECORD, ELEMENT SELECTION

3 3 3 3 $p-1 free - BC given on q-records

2 $q-1 basic and incremental BCs (homogeneous constraints)

1 12 0 $q-2 load set summary

6.0e-2 -1 1 1 0 0 0 0 0 0 1 $q-3 u=u0 at x=0; layer 1

6.0e-2 -1 1 1 0 0 0 0 0 0 2 $q-3 u=u0 at x=0; layer 2

6.0e-2 -1 1 1 0 0 0 0 0 0 3 $q-3 u=u0 at x=0; layer 3

0.0 -1 2 1 0 0 0 0 0 0 1 $q-3 v=0 at x=0; layer 1

0.0 -1 2 1 0 0 0 0 0 0 2 $q-3 v=0 at x=0; layer 2

0.0 -1 2 1 0 0 0 0 0 0 3 $q-3 v=0 at x=0; layer 3

0.0 -1 1 31 0 0 2 1 0 0 1 $q-3 u=v=0 at x=L layer 1

0.0 -1 1 31 0 0 2 1 0 0 2 $q-3 u=v=0 at x=L layer 2

0.0 -1 1 31 0 0 2 1 0 0 3 $q-3 u=v=0 at x=L layer 3

0.0 -1 3 0 0 0 0 0 0 0 1 $q-3 w=0 everywhere; layer 1

0.0 -1 3 0 0 0 0 0 0 0 2 $q-3 w=0 everywhere; layer 2

0.0 -1 3 0 0 0 0 0 0 0 3 $q-3 w=0 everywhere; layer 3

C Incremental BC's for buckling (be sure to set INCBC=1 on B-1 record)

2 9 0

0.0 -1 2 1 0 0 0 0 0 0 1 $q-3 v=0 at x=0; layer 1

0.0 -1 2 1 0 0 0 0 0 0 2 $q-3 v=0 at x=0; layer 2

0.0 -1 2 1 0 0 0 0 0 0 3 $q-3 v=0 at x=0; layer 3

0.0 -1 2 31 0 0 0 0 0 0 1 $q-3 v=0 at x=L; layer 1

0.0 -1 2 31 0 0 0 0 0 0 2 $q-3 v=0 at x=L; layer 2

0.0 -1 2 31 0 0 0 0 0 0 3 $q-3 v=0 at x=L; layer 3

0.0 -1 3 0 0 0 0 0 0 0 1 $q-3 w=0 everywhere; layer 1

0.0 -1 3 0 0 0 0 0 0 0 2 $q-3 w=0 everywhere; layer 2

0.0 -1 3 0 0 0 0 0 0 0 3 $q-3 w=0 everywhere; layer 3

1 1 0 0 $R-1 OUTPUT CONTROL FOR SHELL UNIT 1

euler3d.bin (for S2 processor)

Euler column-buckling PROBLEM $A-1

C

C Thin strip, Euler column buckling from uniform axial compression

C

C REF.: Brush and Almroth, "Buckling of Bars, Plates
28

C and Shells," 1975.

C

1 1 0 0 0 0 0 -1 $b-1 buckling analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control

4 $d-3 cluster definition

Problem References

Brush D. O. and Almroth, B. O., Buckling of Bars, Plates and Shells, McGraw-Hill Book

Company, New York, 1975.
29

Free Vibration of Straight Beam

Background

Free vibration of a straight cantilevered beam modeled using both one- and two-dimensional

elements is studied. Two vibration cases are considered: in-plane vibration and lateral vibration.

The geometry and material properties of the beam are defined in Figure 9 using U. S. customary

units.

Figure 9. Straight cantilevered beam problem: geometry and material properties.

The analytical solutions for linear free vibration of a straight cantilevered beam are given by

Timoshenko, Young and Weaver (1974). The frequencies for longitudinal axial vibration are 

given by Timoshenko et al. (1974, p. 369) as:

" m = (2m #1)$

2L

E

%

where E is Young’s elastic modulus (10 Msi), ρ is the mass density, L is the column length (10

in.), and m is the number of halfwaves along the beam, and ωm is the circular frequency (radians

per second) for the m-th vibration mode. The value used for the acceleration due to gravity is

386.4 in./s

2

and is specified on the B-4 record of the S1 input file. In terms of cycles per second

or hertz, the frequency for the m-th mode is given by:

!

"

2

m

mf =

The frequencies for in-plane (x-z plane) flexural vibration are given by Timoshenko et al. (1974,

p. 426) as:

A

EI

k yy

m m

!

" 2=

where Iyy is the moment of inertia about the y-axis, A is the cross-sectional area, t is the beam

thickness (0.1 in.), h is the beam width (1.0 in.),and km is a constant obtained from the roots of the

following equation:

cos(km L) cosh(km L) + 1 = 0

E = 10 Msi

ν = 0.0

L = 10.0 in.

h = 1.0 in.

t = 0.1 in.

ρ g= 5/6 lb/in.

3

A th

I t h

I th

zz

yy

=

=

=

3

3

12

1

12

1

L

x

z

h

t

y

z
30

The consecutive roots of this equation are given by Timoshenko et al. (1974, p. 426) as:

m kmL

1 1.875

2 4.694

3 7.855

4 10.996

5 14.137

6 17.279

For higher values of m, the roots are approximated by the expression:

kmL = (2m "1)#

2

The frequencies for lateral (x-y plane) flexural vibration are given by Timoshenko et al. (1974, p.

426) as:

A

EI k zz

m m

!

" 2=

where Izz is the moment of inertia about the z-axis. Using this formula, the frequencies for the 

different vibration modes are computed and given in Table 3.

Table 3. Analytical vibration frequencies for cantilevered straight beam.

m Type of Mode

2 ! m

fm

1 Flexural-xy 4.776×103 10.999

2 Flexural-xy 187.590×103 68.933

1 Flexural-xz 4.776×105 109.990

3 Flexural-xy 1471.031×103 193.033

4 Flexural-xy 5649.057×103 378.275

2 Flexural-xz 187.590×105 689.326

1 Extensional 1144.085×105 1702.351

3 Flexural-xz 1471.031×105 1930.328

4 Flexural-xz 5649.057×105 3782.754

2 Extensional 10296.761×105 5107.054

Modeling and Analysis Process

Three separate STAGS finite element models are considered in this sample test case problem:

beam model, shell model, and solid model. In each case, the number of nodes along the beam

length is either 21 or 41; however, for the 3-D 20-node solid element model, the number of 
31

elements along the beam length is half that of the beam and shell models. A summary of each

model includes:

1. 1-D beam model – Model the beam using 2-node beam elements in an element unit.

2. 2-D shell model – Model the beam with 4-node shell elements (x-z plane) in a single shell unit.

3. 3-D solid model – Model beam with 20-node solid elements in a single shell unit.

Material properties and laminate construction are defined using both the historical STAGS

approach (i.e., STAGS versions prior to GCP) and the current GCP approach. Material modeling

for an elastic orthotropic material using the historical STAGS approach requires data on the I-1

and I-2 records to define the material properties and the K-1 and K-2 records to define the 

laminate fabrication data. Section properties for the beam elements can only be accomplished

using the historical STAGS approach using the J series of records. Material modeling using the 

current GCP approach requires data on the I-5a and I-6a records to define the material properties

and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the fabrication.

Boundary condition on the displacements are specified using the P-1 and P-2 records. The 

boundary condition on the left end is clamped with all degrees of freedom restrained at that edge 

(x=0). All other nodes are free. For the 1-D beam model the nodal degrees of freedom are

specified on the node point definition records (S-1 records). For the 2-D shell model, the degrees

of freedom on the boundary edges are specified on the P-1 record. For the 3-D solid model, the 

nodal degrees of freedom for each nodal layer through the thickness are specified using applied

displacement loading conditions on the Q-records. The E885 20-node solid element is used so

that even though the number of nodes along the beam length is the same in the different models,

only half the number of elements is required.

Numerical Results and Discussion

Free vibration of the beam is analyzed for three types of vibration modes: axial, in-plane (xz) 

flexural, and lateral (xy) flexural. There is no external load on the beam – vibration about an

unstressed state. The eigenvalue analysis has a convergence tolerance of 10-4and the number of 

eigenpairs (eigenvalue and corresponding eigenmode) requested is sixteen. No shift is used in the 

eigenvalue solution.

The results for 21 and 41 nodes along the beam length are given in Tables 4, 5 and 6 for the

beam, shell, and solid element models, respectively. Representative vibration mode shapes for

flexural modes in the xy-plane are shown in Figure 10 for the 1-D beam model.
32

Table 4. Vibration analysis results for 1-D beam model.

Frequency, Hertz

Mode Mode Type Analytical E210 Beam Model

20 elements 40 elements

1 Flexural-xy 10.999 10.987 10.997

2 Flexural-xy 68.933 68.662 68.867

3 Flexural-xz 109.990 109.873 109.968

4 Flexural-xy 193.033 191.766 192.706

5 Flexural-xy 378.275 374.796 377.378

6 Flexural-xy 625.249 617.911 623.423

7 Flexural-xz 689.326 686.619 688.667

8 Flexural-xy 934.062 920.507 930.667

9 Flexural-xy 1304.563 1281.933 1298.983

10 Extensional 1702.351 1701.337 1702.245

Table 5. Vibration analysis results for 2-D shell model.

Frequency, Hertz

Mode Mode Type Analytical E410 Shell Model

20 elements 40 elements

1 Flexural-xy 10.999 10.939 10.802

2 Flexural-xy 68.933 68.517 67.660

3 Flexural-xz 109.990 109.831 109.925

4 Flexural-xy 193.033 192.085 189.376

5 Flexural-xy 378.275 377.546 370.992

6 Flexural-xy 625.249 627.193 613.166

7 Flexural-xz 689.326 686.353 688.400

8 Flexural-xy 934.062 943.564 915.905

9 Flexural-xy 1304.563 1330.481 1279.306

10 Extensional 1702.351 1701.242 1701.564

Table 6. Vibration analysis results for 3-D solid model.

Frequency, Hertz

Mode Mode Type Analytical E885 Solid Model

10 elements 20 elements

1 Flexural-xy 10.999 10.970 10.992

2 Flexural-xy 68.933 68.312 68.734

3 Flexural-xz 109.990 108.824 109.044

4 Twisting --- 163.963 153.970

5 Flexural-xy 193.033 190.197 191.966

6 Flexural-xy 378.275 370.477 374.784

7 Twisting --- 493.116 493.611

8 Flexural-xy 625.249 608.260 616.127

9 Flexural-xz 689.326 647.861 652.075

10 Flexural-xy 934.062 --- ---
33

(a) Mode 1, flexural mode in xy-plane, 10.997 hertz.

Mode 2, flexural mode in xy-plane, 68.867 hertz.

Mode 4, flexural mode in xy-plane, 192.706 hertz.

Mode 5, flexural mode in xy-plane, 377.378 hertz.

Figure 10. Representative flexural vibration mode shapes from the 1-D beam model.
34

STAGS Input Files

These STAGS input files are located under the following directory:

$STAGSHOME/Sample-Testcases/Beam-Vibration

Model using 1-D Beam Elements

The following text file provides the input for a beam finite element model using forty 2-node

E210 beam elements along the beam length.

beam1d.inp (for S1 processor)

Straight beam free vibration problem - 1-D model $A-1

C

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

C MODEL INPUT CONTROLS

1 0 1 0 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 -90.0 $B-1b model rotations

0 1 0 $B-2

1 1 1 0 0 1 $B-3 INCLUDE GCP INPUT

386.4 $B-4 acceleration due to gravity, g (in/s/s)

C

C Define Element Unit data

C

42 0 40 0 0 0 $h-1 No. of points and No. of beam elements

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.83333 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

2.1583354E-3, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

0.10 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C Beam cross-sectional properties

C

1 1 1 0 8.3333E-5 0.0 0.0 0 0 0 $j-1

0.1 8.3333E-3 8.3333E-5 0.0 $j-2

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 0.10 0.0 0 $K-2 LAYERED WALL

C

C ELEMENT UNIT 1 MODEL DEFINITION

C

1 0 0 0 0.0 0.0 0.0 000 000 $s-1 end point at x=0
35

2 0 0 0 0.25 0.0 0.0 111 111 0 40 0 $s-1 BC's for x-z inplane

vibration

1 0 0 0 0.25 0.0 0.0 $s-1a user point

incrementation

42 0 0 0 5.0 1.0 0.0 111 111 $s-1 reference node

C

C Generate beam elements

C

1 2 42 210 1 0.0 0.0 0.0 0 0 40 $T-2

1 1 0 $T-2a generate 20 elements

C

C generate loads - applied end shortening

C

0 0 $u-1 Loads summary

1 0 0 $v-1 output control

beam1d.bin (for S2 processor)

Straight beam free vibration problem - 1-D model $A-1

C

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

2 1 0 0 0 0 0 -1 $b-1 free vibration analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control

20 $d-3 cluster definition

beam1d.pin (for STAPL processor)

Straight cantilevered beam - free vibration problem

16 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

1 0 4 0 1 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 2 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 3 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 4 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 5 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 6 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 7 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 8 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 9 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 10 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 11 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 12 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 13 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 14 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP
36

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 15 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 4 0 16 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

Model using 2-D Shell Elements

The following text file provides the input for a beam finite element model using forty 4-node

E410 shell elements along the beam length and one element across the beam width.

beam2d.inp (for S1 processor)

Straight beam free vibration problem - 2-D model $A-1

C

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

C MODEL INPUT CONTROLS

1 0 1 0 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 -90.0 $B-1b model rotations

1 10*0 $B-2

1 0 1 0 0 1 $B-3 INCLUDE GCP INPUT

386.4 $b-4 acceleration due to gravity g (in/s/s)

41 2 $F-1 DISCRETIZATION: NROWS, NCOLS OF NODES

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.83333 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

2.1583354E-3, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

1.0 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 1.0 0.0 0 $K-2 LAYERED WALL

C

C SHELL UNIT 1 MODEL DEFINITION

C

2 0 4*0 $M-1 Rectangular PLATE GEOMETRY

0.0 10.0 0.0 0.1 $M-2 L=10 in.; t=0.1 in.

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 DISCRETIZATION RECORD, ELEMENT SELECTION

2 3 3 3 $P-1 Cantilevered beam simulation

0 0 0 0 $Q-1 No applied load - free vibration

1 0 0 0 $R-1 OUTPUT CONTROL FOR SHELL UNIT 1
37

beam2d.bin (for S2 processor)

Straight beam free vibration problem - 1-D model $A-1

C

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

2 1 0 0 0 0 0 -1 $b-1 free vibration analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control

16 $d-3 cluster definition

beam2d.pin (for STAPL processor)

Straight cantilevered beam - free vibration problem

16 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 2 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 3 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 4 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 5 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 6 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 7 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 8 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 9 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 10 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 11 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 12 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 13 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 14 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 15 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 16 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

Model using 3-D Solid Elements

The following text file provides the input for a beam finite element model using twenty 20-node 

E885 solid elements along the beam length and one element across the beam width and across the 

beam depth.

beam3d.inp (for S1 processor)

Straight beam free vibration problem - 3-D model $A-1

C
38

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

C MODEL INPUT CONTROLS

1 0 1 1 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 -90.0 $B-1b rotations for model plot

1 10*0 $B-2

1 0 1 0 0 1 $B-3 INCLUDE GCP INPUT

386.4 $b-4 acceleration due to gravity, g (in./s/s)

41 3 $F-1 DISCRETIZATION: NROWS, NCOLS OF NODES

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.83333 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

CC2.1583354E-3, $I-6A MASS DENSITY

2.1566598E-3, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SOLID_FABRICATION 1 1 0 $I-5A GCP Solid Fabrication Record

1.0 $I-22a element thickness

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

1.0 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 1.0 0.0 0 $K-2 LAYERED WALL

C

C UNIT 1 MODEL DEFINITION (one solid element thickness thickness)

C

2 0 0 0 1 1 $M-1 Rectangular PLATE GEOMETRY

0.0 10.0 0.0 0.1 $M-2 L=30 in.; t=1.0 in.

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

885 0 0 $N-1 DISCRETIZATION RECORD, ELEMENT SELECTION

3 3 3 3 $P-1 BC imposed on q-records

1 $q-1 homogeneous BC's imposed on q-records for 3D elements

1 3 0 $q-2 (E881 has 2 nodal layers; E883, E885 has three)

0.0 -1 1 1 0 0 3 1 0 0 1 $q-3 u=v=w=0 at clamped end for layer 1

0.0 -1 1 1 0 0 3 1 0 0 2 $q-3 u=v=w=0 at clamped end for layer 2

0.0 -1 1 1 0 0 3 1 0 0 3 $q-3 u=v=w=0 at clamped end for layer 3

1 0 0 0 $R-1 OUTPUT CONTROL FOR SHELL UNIT 1

beam3d.bin (for S2 processor)

Straight beam free vibration problem - 1-D model $A-1

C

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems
39

C in Engineering," 1974.

C

2 1 0 0 0 0 0 -1 $b-1 free vibration analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control

16 $d-3 cluster definition

beam3d.pin (for STAPL processor)

Straight cantilevered beam - free vibration problem

16 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 2 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 3 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 4 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 5 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 6 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 7 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 8 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 9 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 10 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 11 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 12 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 13 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 14 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 15 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 16 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

Problem References

Timoshenko, S., Young, D. H., and Weaver, W., Jr., Vibration Problems in Engineering, Fourth

Edition, John Wiley & Sons, Inc., New York, 1974.
40

Free Vibration of Circular Ring

Background

Free vibration of a circular ring modeled using both one- and two-dimensional elements is

studied. Two vibration cases are considered: extensional vibration and in-plane flexural

vibration. The geometry and material properties of the circular ring with a square cross sectional

area are defined in Figure 11 using U. S. customary units.

Figure 11. Circular ring problem: geometry and material properties.

The analytical solutions for linear free vibration of a circular ring are given by Timoshenko,

Young and Weaver (1974). The frequencies for extensional vibration are given by Timoshenko

et al. (1974, pp. 476-477) as:

2

2 (1 )

R

E m

m

!

"

+

=

where E is Young’s elastic modulus (10 Msi), ρ is the mass density, R is the radius of the

centerline of the ring (20/π in.), and m is the number of full waves (m=0 is the pure radial

vibration case), and ωm is the circular frequency (radians per second) for the m-th vibration mode.

In terms of cycles per second or hertz, the frequency for the m-th mode is given by:

!

"

2

m

mf =

E = 10 Msi

ν = 0.0

R = 20.0/π in.=6.3662 in.

h = 0.1 in.

t = 0.1 in.

g=386.4 in./s

2

ρ g= 5/6 lb/in.

3

A th

I t h

I th

zz

yy

=

=

=

3

3

12

1

12

1

R

x

y

t

x

z

h
41

Using these formula, the frequencies for the in-plane (x-z plane) extensional vibration modes are 

computed as follows:

m Type of Mode

2 ! m

fm

0 Pure radial 1.1441×108 1702.351

1 Extension 2.2882×108 2407.488

2 Extension 5.7204×108 3806.573

3 Extension 11.4408×108 5383.308

The frequencies for in-plane (x-y plane) flexural vibration of the circular ring are given by

Timoshenko et al. (1974, pp. 479-481) as:

(1 )

(1 )

4 2

2 2 2

AR m

EI

zzm m

m

+

!

=

"

#

where Izz is the moment of inertia about the z-axis, A is the cross-sectional area, t is the ring

thickness (0.1 in.), h is the ring width (1.0 in.), and ωm is the circular frequency (radians per

second) for the m-th vibration mode. For m=1, the frequency is zero indicating that the ring

moves as a rigid body.

Using this formula, the frequencies for the in-plane flexural vibration modes are computed as

follows:

m Type of Mode 2 ! mfm

1 Rigid Body 0 0

2 Flexural 16937.49 20.713

3 Flexural 135499.94 58.585

4 Flexural 498161.55 112.332

5 Flexural 1302884.10 181.666

6 Flexural 2803841.71 266.500

7 Flexural 5311597.88 366.803

8 Flexural 9193150.18 482.561

Modeling and Analysis Process

Three separate STAGS finite element models are considered in this test case problem: beam 

elements, shell elements, and solid elements. A summary of each model includes:

1. 1-D beam model – Model the beam using discrete beam elements using an element unit where 

node records (S records) are generated using an external FORTRAN code to compute nodal

coordinates and output each record.

2. 2-D plate model – Model the beam with plate elements (x-y plane) in a single shell unit using

the annular plate shell geometry.

For each model, a full 360-degree model of the ring is used (i.e., a 360° segment) with boundary

conditions applied to constrain the motion to the xy plane. The annular plate shell geometry does

not include extensions for 3-D elements – presumably because of the possible pole at the center.

Therefore a 3-D solid model is not consider; however, a 3-D model could be developed as an

element unit using MSC.Patran or other external finite element modeling approach.
42

Material properties and fabrication construction are defined using both the historical STAGS 

approach (i.e., STAGS versions prior to GCP) and the current GCP approach. Material modeling

for an elastic material using the historical STAGS approach requires data on the I-1 and I-2

records to define the material properties and the K-1 and K-2 records to define the fabrication

data. Section properties for the beam elements can only be accomplished using the historical

STAGS approach using the J records. Material modeling using the current GCP approach

requires data on the I-5a and I-6a records to define the material properties and records I-5a, I-21a,

I-21b, I-21c, I-21d, and I-21e to define the fabrication.

Boundary condition on the displacements are specified using the P-1 and P-2 records. The inplane edges of the 2-D shell model are free. The out-of-plane degrees of freedom are constrained

using the Q records to specify homogeneous conditions. The drilling freedom is retained as an

active degree of freedom for the E410 shell element since in contributes to the membrane

response of the element.

Numerical Results and Discussion

Free vibration of the circular ring is analyzed for two types of vibration modes: in-plane

extensional and in-plane flexural. There is no external load on the ring – vibration about an

unstressed state. The eigenvalue analysis has a convergence tolerance of 10-4and the number of 

eigenpairs (eigenvalue and corresponding eigenmode) requested is six. No shift is used in the 

eigenvalue solution. In both the 1-D and 2-D models, three rigid body modes are extracted first

(zero frequencies) and then the various modes (in pairs) are computed. The flexural modes occur

in pairs because of the periodicity of the solutions with one mode rotated relative to the other by

an angle corresponding to a half cycle. These mode shapes are shown in Figure 12 for the 1-D

beam model. Comparison of vibration frequencies for the models analyzed is given in Table 7.

The ring cross-sectional area is square. In the 1-D model no deformations occur in the crosssectional plane; however, in the 2-D model, in-plane deformations of the cross section may occur.

This added flexibility results in slightly lower vibration frequencies for the 2-D model.

Table 7. Vibration analysis results for circular ring.

Frequency, Hertz

Number of Finite Element Model

Full Waves, m

Mode Type Analytical

1-D Model 2-D Model

2 Flexural 20.713 20.717 19.095

3 Flexural 58.585 58.597 53.957

4 Flexural 112.332 112.36 103.40

5 Flexural 181.666 181.70 167.15

6 Flexural 266.500 266.56 245.09

7 Flexural 366.803 366.88 337.17

8 Flexural 482.561 482.66 443.33
43

(a) Mode 4, m=2

(b) Mode 6, m=3

(c) Mode 8, m=4

(d) Mode 10, m=5

(e) Mode 12, m=6

(f) Mode 14, m=7

Figure 12. Representative in-plane free vibration mode shapes.
44

STAGS Input Files

These STAGS input files are located under the following directory:

$STAGSHOME/Sample-Testcases/Ring-Vibration

Model using 1-D Beam Elements

The following text file provides the input for a beam finite element model using forty 2-node E210 beam

elements along the ring circumference.

ring1d.inp (for S1 processor)

Circular ring free vibration problem - 1-D model $A-1

C

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

C MODEL INPUT CONTROLS

1 0 1 0 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 -90.0 $B-1b model rotations

0 1 0 $B-2

1 1 1 0 0 1 $B-3 INCLUDE GCP INPUT

386.4 $B-4 acceleration due to gravity, g (in/s/s)

C

C Define Element Unit data

C

181 0 180 0 0 0 $h-1 No. of points and No. of beam elements

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.83333 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

2.15666E-3, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

0.10 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C Beam cross-sectional properties

C

1 1 1 0 0.3333E-4 0.0 0.0 0 0 0 $j-1

0.01 0.083333E-4 0.083333E-4 0.0 $j-2

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 0.10 0.0 0 $K-2 LAYERED WALL

C

C ELEMENT UNIT 1 MODEL DEFINITION
4

5

C

10006.3661980.0000000.01100010$s-1

20006.3623200.2221770.01100010$s-1

30006.3506900.4440840.01100010$s-1

40006.3313230.6654490.01100010$s-1

50006.3042420.8860030.01100010$s-1

60006.2694811.1054790.01100010$s-1

70006.2270811.3236070.01100010$s-1

80006.1770941.5401230.01100010$s-1

90006.1195821.7547620.01100010$s-1

100006.0546141.9672630.01100010$s-1

110005.9822692.1773680.01100010$s-1

120005.9026362.3848200.01100010$s-1

130005.8158112.5893660.01100010$s-1

140005.7219012.7907570.01100010$s-1

150005.6210192.9887490.01100010$s-1

160005.5132893.1830990.01100010$s-1

170005.3988423.3735710.01100010$s-1

180005.2778173.5599330.01100010$s-1

190005.1503623.7419570.01100010$s-1

200005.0166323.9194230.01100010$s-1

210004.8767904.0921130.01100010$s-1

220004.7310074.2598180.01100010$s-1

230004.5794594.4223330.01100010$s-1

240004.4223334.5794590.01100010$s-1

250004.2598184.7310070.01100010$s-1

260004.0921134.8767900.01100010$s-1

270003.9194235.0166320.01100010$s-1

280003.7419575.1503620.01100010$s-1

290003.5599335.2778170.01100010$s-1

300003.3735715.3988420.01100010$s-1

310003.1830995.5132890.01100010$s-1

320002.9887495.6210190.01100010$s-1

330002.7907575.7219010.01100010$s-1

340002.5893665.8158110.01100010$s-1

350002.3848205.9026360.01100010$s-1

360002.1773685.9822690.01100010$s-1

370001.9672636.0546140.01100010$s-1

380001.7547626.1195820.01100010$s-1

390001.5401236.1770940.01100010$s-1

400001.3236076.2270810.01100010$s-1

410001.1054796.2694810.01100010$s-1

420000.8860036.3042420.01100010$s-1

430000.6654496.3313230.01100010$s-1

440000.4440846.3506900.01100010$s-1

450000.2221776.3623200.01100010$s-1

460000.0000006.3661980.01100010$s-1

47000-0.2221776.3623200.01100010$s-1

48000-0.4440846.3506900.01100010$s-1

49000-0.6654496.3313230.01100010$s-1

50000-0.8860036.3042420.01100010$s-1

51000-1.1054796.2694810.01100010$s-1

52000-1.3236076.2270810.01100010$s-1

53000-1.5401236.1770940.01100010$s-1

54000-1.7547626.1195820.01100010$s-1

55000-1.9672636.0546140.01100010$s-1

56000-2.1773685.9822690.01100010$s-1

57000-2.3848205.9026360.01100010$s-1

58000-2.5893665.8158110.01100010$s-1

59000-2.7907575.7219010.01100010$s-1

60000-2.9887495.6210190.01100010$s-1

61000-3.1830995.5132890.01100010$s-1

62000-3.3735715.3988420.01100010$s-1
4

6

63000-3.5599335.2778170.01100010$s-1

64000-3.7419575.1503620.01100010$s-1

65000-3.9194235.0166320.01100010$s-1

66000-4.0921134.8767900.01100010$s-1

67000-4.2598184.7310070.01100010$s-1

68000-4.4223334.5794590.01100010$s-1

69000-4.5794594.4223330.01100010$s-1

70000-4.7310074.2598180.01100010$s-1

71000-4.8767904.0921130.01100010$s-1

72000-5.0166323.9194230.01100010$s-1

73000-5.1503623.7419570.01100010$s-1

74000-5.2778173.5599330.01100010$s-1

75000-5.3988423.3735710.01100010$s-1

76000-5.5132893.1830990.01100010$s-1

77000-5.6210192.9887490.01100010$s-1

78000-5.7219012.7907570.01100010$s-1

79000-5.8158112.5893660.01100010$s-1

80000-5.9026362.3848200.01100010$s-1

81000-5.9822692.1773680.01100010$s-1

82000-6.0546141.9672630.01100010$s-1

83000-6.1195821.7547620.01100010$s-1

84000-6.1770941.5401230.01100010$s-1

85000-6.2270811.3236070.01100010$s-1

86000-6.2694811.1054790.01100010$s-1

87000-6.3042420.8860030.01100010$s-1

88000-6.3313230.6654490.01100010$s-1

89000-6.3506900.4440840.01100010$s-1

90000-6.3623200.2221770.01100010$s-1

91000-6.3661980.0000000.01100010$s-1

92000-6.362320-0.2221770.01100010$s-1

93000-6.350690-0.4440840.01100010$s-1

94000-6.331323-0.6654490.01100010$s-1

95000-6.304242-0.8860030.01100010$s-1

96000-6.269481-1.1054790.01100010$s-1

97000-6.227081-1.3236070.01100010$s-1

98000-6.177094-1.5401230.01100010$s-1

99000-6.119582-1.7547620.01100010$s-1

100000-6.054614-1.9672630.01100010$s-1

101000-5.982269-2.1773680.01100010$s-1

102000-5.902636-2.3848200.01100010$s-1

103000-5.815811-2.5893660.01100010$s-1

104000-5.721901-2.7907570.01100010$s-1

105000-5.621019-2.9887490.01100010$s-1

106000-5.513289-3.1830990.01100010$s-1

107000-5.398842-3.3735710.01100010$s-1

108000-5.277817-3.5599330.01100010$s-1

109000-5.150362-3.7419570.01100010$s-1

110000-5.016632-3.9194230.01100010$s-1

111000-4.876790-4.0921130.01100010$s-1

112000-4.731007-4.2598180.01100010$s-1

113000-4.579459-4.4223330.01100010$s-1

114000-4.422333-4.5794590.01100010$s-1

115000-4.259818-4.7310070.01100010$s-1

116000-4.092113-4.8767900.01100010$s-1

117000-3.919423-5.0166320.01100010$s-1

118000-3.741957-5.1503620.01100010$s-1

119000-3.559933-5.2778170.01100010$s-1

120000-3.373571-5.3988420.01100010$s-1

121000-3.183099-5.5132890.01100010$s-1

122000-2.988749-5.6210190.01100010$s-1

123000-2.790757-5.7219010.01100010$s-1

124000-2.589366-5.8158110.01100010$s-1

125000-2.384820-5.9026360.01100010$s-1
47

126 0 0 0 -2.177368 -5.982269 0.0 110 001 0 $s-1

127 0 0 0 -1.967263 -6.054614 0.0 110 001 0 $s-1

128 0 0 0 -1.754762 -6.119582 0.0 110 001 0 $s-1

129 0 0 0 -1.540123 -6.177094 0.0 110 001 0 $s-1

130 0 0 0 -1.323607 -6.227081 0.0 110 001 0 $s-1

131 0 0 0 -1.105479 -6.269481 0.0 110 001 0 $s-1

132 0 0 0 -0.886003 -6.304242 0.0 110 001 0 $s-1

133 0 0 0 -0.665449 -6.331323 0.0 110 001 0 $s-1

134 0 0 0 -0.444084 -6.350690 0.0 110 001 0 $s-1

135 0 0 0 -0.222177 -6.362320 0.0 110 001 0 $s-1

136 0 0 0 0.000000 -6.366198 0.0 110 001 0 $s-1

137 0 0 0 0.222177 -6.362320 0.0 110 001 0 $s-1

138 0 0 0 0.444084 -6.350690 0.0 110 001 0 $s-1

139 0 0 0 0.665449 -6.331323 0.0 110 001 0 $s-1

140 0 0 0 0.886003 -6.304242 0.0 110 001 0 $s-1

141 0 0 0 1.105479 -6.269481 0.0 110 001 0 $s-1

142 0 0 0 1.323607 -6.227081 0.0 110 001 0 $s-1

143 0 0 0 1.540123 -6.177094 0.0 110 001 0 $s-1

144 0 0 0 1.754762 -6.119582 0.0 110 001 0 $s-1

145 0 0 0 1.967263 -6.054614 0.0 110 001 0 $s-1

146 0 0 0 2.177368 -5.982269 0.0 110 001 0 $s-1

147 0 0 0 2.384820 -5.902636 0.0 110 001 0 $s-1

148 0 0 0 2.589366 -5.815811 0.0 110 001 0 $s-1

149 0 0 0 2.790757 -5.721901 0.0 110 001 0 $s-1

150 0 0 0 2.988749 -5.621019 0.0 110 001 0 $s-1

151 0 0 0 3.183099 -5.513289 0.0 110 001 0 $s-1

152 0 0 0 3.373571 -5.398842 0.0 110 001 0 $s-1

153 0 0 0 3.559933 -5.277817 0.0 110 001 0 $s-1

154 0 0 0 3.741957 -5.150362 0.0 110 001 0 $s-1

155 0 0 0 3.919423 -5.016632 0.0 110 001 0 $s-1

156 0 0 0 4.092113 -4.876790 0.0 110 001 0 $s-1

157 0 0 0 4.259818 -4.731007 0.0 110 001 0 $s-1

158 0 0 0 4.422333 -4.579459 0.0 110 001 0 $s-1

159 0 0 0 4.579459 -4.422333 0.0 110 001 0 $s-1

160 0 0 0 4.731007 -4.259818 0.0 110 001 0 $s-1

161 0 0 0 4.876790 -4.092113 0.0 110 001 0 $s-1

162 0 0 0 5.016632 -3.919423 0.0 110 001 0 $s-1

163 0 0 0 5.150362 -3.741957 0.0 110 001 0 $s-1

164 0 0 0 5.277817 -3.559933 0.0 110 001 0 $s-1

165 0 0 0 5.398842 -3.373571 0.0 110 001 0 $s-1

166 0 0 0 5.513289 -3.183099 0.0 110 001 0 $s-1

167 0 0 0 5.621019 -2.988749 0.0 110 001 0 $s-1

168 0 0 0 5.721901 -2.790757 0.0 110 001 0 $s-1

169 0 0 0 5.815811 -2.589366 0.0 110 001 0 $s-1

170 0 0 0 5.902636 -2.384820 0.0 110 001 0 $s-1

171 0 0 0 5.982269 -2.177368 0.0 110 001 0 $s-1

172 0 0 0 6.054614 -1.967263 0.0 110 001 0 $s-1

173 0 0 0 6.119582 -1.754762 0.0 110 001 0 $s-1

174 0 0 0 6.177094 -1.540123 0.0 110 001 0 $s-1

175 0 0 0 6.227081 -1.323607 0.0 110 001 0 $s-1

176 0 0 0 6.269481 -1.105479 0.0 110 001 0 $s-1

177 0 0 0 6.304242 -0.886003 0.0 110 001 0 $s-1

178 0 0 0 6.331323 -0.665449 0.0 110 001 0 $s-1

179 0 0 0 6.350690 -0.444084 0.0 110 001 0 $s-1

180 0 0 0 6.362320 -0.222177 0.0 110 001 0 $s-1

181 0 0 0 0.000000 0.000000 0.0 110 000 0 $s-1

C

C Generate beam elements

C

1 2 181 210 1 0.0 0.0 0.0 0 0 179 $T-2

1 1 0 $T-2a generate 20 elements

180 1 181 210 1 0.0 0.0 0.0 0 0 0 $T-2

C
48

C generate loads - applied end shortening

C

0 0 $u-1 Loads summary

1 0 0 $v-1 output control

ring1d.bin (for S2 processor)

Straight beam free vibration problem - 1-D model $A-1

C

C Thin straight strip, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

2 1 0 0 0 0 0 -1 $b-1 free vibration analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control

20 -1.0 $d-3 cluster definition

ring1d.pin (for STAPL processor)

Straight cantilevered beam - free vibration problem

16 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

1 0 4 0 1 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 2 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 3 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 4 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 5 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 6 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 7 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 8 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 9 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 10 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 11 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 12 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 13 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX
49

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 14 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 15 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

1 0 4 0 16 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

Model using 2-D Shell Elements

The following text file provides the input for a finite element model using 360 4-node E410 shell

elements along the ring circumference.

ring2d.inp (fpr S1 processor)

Circular ring free vibration problem - 2-D model $A-1

C

C Thin 90-degreesegment of circular ring, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

C MODEL INPUT CONTROLS

1 0 1 0 0 0 0 $B-1

CCX1 0.0/ 2 90.0 / 3 0.0

1 0 0 1 $B-2

1 0 1 0 0 1 $B-3 INCLUDE GCP INPUT

386.4 $b-4 acceleration due to gravity g (in/s/s)

2 361 $F-1 DISCRETIZATION: NROWS, NCOLS OF NODES

1 2 1 4 $g-1 complete ring, full 360-degrees

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

10.0e+6 0.0 0.0 0.83333 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

10.0E+6, $I-6A YOUNG'S MODULUS, PSI

0.0 , $I-6A POISSON'S RATIO

2.15666E-3, $I-6A MASS DENSITY

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

SHELL_FABRICATION 1 1 0 0 0 $I-5A GCP SHELL FABRICATION RECORD

1 $I-21A GCP LAYER MATERIAL ID

0.1 $I-21C GCP LAYER THICKNESS, INCHES

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 0.1 0.0 0 $K-2 LAYERED WALL

C

C SHELL UNIT 1 MODEL DEFINITION

C

4 0 4*0 $M-1 Annular PLATE GEOMETRY

CC5.8662 6.8662 0.0 360.0 $M-2 Ra, Rb, theta-a, theta-b

6.3162 6.4162 0.0 360.0 $M-2 Ra, Rb, theta-a, theta-b
50

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 DISCRETIZATION RECORD, ELEMENT SELECTION

3 6 3 6 $P-1 symmetric quarter of a ring simulation

1 0 0 0 $Q-1 No applied load - free vibration

1 3

0.0 -1 3 0 0

0.0 -1 4 0 0

0.0 -1 5 0 0

CC0.0 -1 6 0 0

1 0 0 0 $R-1 OUTPUT CONTROL FOR SHELL UNIT 1

ring2d.bin (for S2 processor)

Circular ring free vibration problem - 1-D model $A-1

C

C Thin 90-deg segment of circular ring, free vibration problem

C

C REF.: Timoshenko, Young, and Weaver, "Vibration Problems

C in Engineering," 1974.

C

2 1 0 0 0 0 0 -1 $b-1 free vibration analysis

1.0 1.0 1.0 $c-1 load factors

100 1.0e-4 0 $d-2 eigenvalue control

16 -1.0 $d-3 cluster definition

ring2d.pin (for STAPL processor)

Straight cantilevered beam - free vibration problem

16 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

1 0 4 0 1 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 2 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 3 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 4 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 5 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 6 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 7 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 8 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 9 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 10 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 11 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX
51

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 12 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 13 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 14 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 15 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

1 0 4 0 16 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 90.0 / 3 0.0

Problem References

Timoshenko, S., Young, D. H., and Weaver, W., Jr., Vibration Problems in Engineering, Fourth Edition,

John Wiley & Sons, Inc., New York, 1974.
52

Buckling of Blade-Stiffened Flat Panels

Background

Stiffened panels are a common configuration in the aerospace industry. Stiffened panels may be modeled

in at least three ways. One way is to smear the stiffener stiffness over the panel skin – smeared-stiffener 

model. Another way is to model the stiffeners as discrete beams located along discrete lines in the model

and without cross-sectional deformations – discrete-stiffener model. The third way is to model the

stiffeners using shell elements – branched-plate model. Stroud, Greene, and Anderson (1984) studied

several stiffened-panel configurations subjected to in-plane compression and shear loads. Their results

are often cited as reference solutions for comparative purposes. The basic geometry of the panel and the 

repeating blade-stiffener segment considered in this study are defined in Figure 13 using U. S. customary

units.

Figure 13. Blade-stiffened panel problem: geometry and repeating element – all dimensions are given in

inches.

30 in.

30 in.

y

x

1.352 in.

5.0

in.

2.5

in.
53

These demonstration test cases involve a flat, square panel with six blade stiffeners (six repeating

elements). The panel has a length L equal to 30 inches and an overall panel width W of 30 inches (six

repeating elements of width 5.0 inches). No offsets are assumed for attaching the blade stiffeners to the

panel skin in the branched-plate model approach (i.e., there is a small amount of overlapping of material

at their connection point). The reference surface of the panel skin is defined as the middle surface of the 

skin. Three panel configurations are considered.

Panel 1 corresponds to Example 1 in NASA TP-2215 – a composite blade-stiffened panel. The panel skin

and blade stiffeners are laminated composite structures. The material definitions for the panel skin and

stiffener have the same linear elastic mechanical properties for an orthotropic material: E1=19.0 Msi,

E2=1.89 Msi, G12=0.93 Msi, ν12=0.38, and ν21=0.0378. The fabrication of the panel skin is a laminated

composite with a stacking sequence defined as

s [ 45 / 45 / 0 / 90 ] ± m 9 – a 28-ply laminate, and the

stacking sequence of the blade stiffeners is defined as

s [ 45 / 45 / 0 ] ± m 2 – a 12-ply laminate. The 

average ply thickness is 0.0055 inches. Two loading cases are considered here. The pure compression

case (Nx=1000 lb/in.) results in a load distribution of 811.35 lb/in. in each skin segment and 697.67 lb/in.

in each blade stiffener according to NASA TP-2215. The buckling load factor is 1.0030 with an overall

Euler buckling mode shape obtained from the EAL finite element code. The pure shear case (Nxy=1000

lb/in.) results in all the load going into the skin segments and nothing in the blade stiffeners. The 

buckling load factor is 1.5525 with a skewed mode shape having one halfwave in the stiffener direction

and two halfwaves across the panel.

Panel 2 corresponds to Example 2 in NASA TP-2215 – a metal blade-stiffened panel with a thick skin.

The panel skin is 0.084-inches thick, and the blade stiffeners are 0.058-inches thick. The material

definitions for the panel skin, and blade stiffeners are the same linear elastic mechanical properties for an

isotropic material: E=10.5 Msi and ν=0.32. The pure compression case (Nx=1000 lb/in.) results in a load

distribution of 842.67 lb/in. in each skin segment and 581.84 lb/in. in each blade stiffener according to

NASA TP-2215. The buckling load factor is 0.9759 with an overall Euler buckling mode shape obtained

from the EAL finite element code. The pure shear case (Nxy=1000 lb/in.) results in all the load going into

the skin segments and nothing in the blade stiffeners. The buckling load factor is 0.8138 with a skewed

mode shape having one halfwave in the stiffener direction and three halfwaves across the panel.

Panel 3 corresponds to Example 4 in NASA TP-2215 – a metal blade-stiffened panel with a thin skin.

The panel skin is 0.050-inches thick, and the blade stiffeners are 0.058-inches thick. The material

definitions from Panel 2 are used here as well. The pure compression case (Nx=1000 lb/in.) results in a 

load distribution of 761.23 lb/in. in each skin segment and 883.03 lb/in. in each blade stiffener according

to NASA TP-2215. The buckling load factor is 0.2965 with an stiffened panel buckling mode shape 

having six halfwaves between each stiffener obtained from the EAL finite element code (Whetstone,

1986). The pure shear case (Nxy=1000 lb/in.) results in all the load going into the panel skin segments and

nothing in the blade stiffeners. The buckling load factor is 0.2767 with a skewed mode shape having one

halfwave in the stiffener direction and four halfwaves across the panel.

The reference solutions obtained by Stroud, Greene, and Anderson (1984) for linear bifurcation buckling

loads and buckling mode shapes are used for comparison.

Modeling and Analysis Process

Three separate STAGS finite element models are considered in these demonstration test case problems:

smeared-stiffener model, discrete-stiffener model, and branched-plate model. The basic finite element

discretization for the panel skin is the same in each modeling approach – 36 elements across the panel

length and width. A summary of each model includes:
54

Smeared-stiffener model – Model the stiffened panel with a single shell unit for the panel skin and

STAGS automatically “smears” the stiffness of the blade stiffeners across the panel skin. Each stiffener

is defined in STAGS in the same manner as would be required for the discrete-stiffener model. A

rectangular subelement is defined using the J-1 and J-3b records for the metal stiffeners and STAGS

internally computes and outputs the beam stiffnesses. For the composite panel, the general stiffness

option for defining beam stiffnesses (EA, EIyy, EIzz, EIyz, GJ) using the J-1 and J-2b records. These

properties are defined relative to the stiffener cross-sectional centroid. The stiffener spacing and

eccentricity relative to the shell reference surface are defined using the K-6 record as part of the panel

skin fabrication data. This model will predict general buckling behavior but no skin-stiffener buckling

modes – essentially orthotropic panel buckling mode shapes. This model is shown in Figure 14.

Discrete-stiffener model – Model the stiffened panel with a single shell unit for the panel skin and model

the blade stiffeners as discrete beams located along discrete lines on the panel skin (lines of constant

values of y). The blade stiffeners are defined using the J records as in the smeared-stiffener model. These

discrete-beam stiffeners are located on the shell reference surface using the O-2a and O-2b records. This

discrete-stiffener model will predict general and skin-stiffener buckling mode shapes – essentially

stiffened-panel buckling mode shapes but no cross-sectional deformation of the stiffeners is permitted and

skin-stiffener interaction is limited to the nodal line attaching each stiffener. This model is shown in

Figure 15 with the discrete-beam stiffeners shown as darker lines.

Branched-plate model – Model the stiffened panel with multiple shell units – for both panel skin and

stiffeners. Two approaches could be used. First, each segment could be individually modeled (e.g., skin,

blade, skin, blade, etc.). This would result in seven shell units for the various panel skin segments and six

shell units for the stiffeners (one for each blade stiffener) – total of 13 shell units. The other approach

would be model the skin as a single shell unit with the six stiffener shell units attached within the skin

shell unit. The model using 13 shell units (each shell unit is indicated by a different color or shade) used

in these studies is shown in Figure 16. There are two 4-node shell elements (three columns of nodes) 

across the blade-stiffener height in the branched-plate model. The same finite element model is used for 

the composite and metal panels with changes in the shell fabrication number and the membrane loads for 

the panel skin and blade stiffeners.

In the analysis of this structure using either the discrete-stiffener or smeared-stiffener modeling approach,

the stiffness terms of the blade stiffener need to be provided to STAGS. For the metal panel case, the

rectangular geometry of the blade stiffener can be defined to STAGS and STAGS will compute the 

necessary terms. The x-direction is along the stiffener axis, the z-direction is perpendicular to the panel

skin, and the y-direction is perpendicular to the x-z plane of the stiffener. The quantities needed include: 3 0 12 12 

3 3 3 bt I J bt I b t A bt I =

yy

=

zz

=

yz

= =

where b is the blade width or height (1.352 in.) and t is the blade thickness (0.058 in.). The centroid of

the blade cross-sectional area is b/2 (0.676 inches) above the panel skin reference surface.

For the composite panel case, the blade stiffeners are also laminated structures. Currently there is no

automatic feature in STAGS to treat laminated beams. The approach used herein is define the laminate of

the blade and perform a laminate analysis using STAGS in order to obtain the coefficients of the so-called

ABD matrices. A dummy material is defined with all moduli defined as a million and the Poisson’s ratio

set to zero (see the I-records). Then the stiffness terms for the composite blades are computed as

followed:
55

( )

!

"

# $

%

& = +

= = =

!

"

# $

%

&

= '

66

12

11

2

22

2

12

11

2

4

 0

12

1

D

D GJ b

EI EAb EI D b EI

A

A EA b A

yy zz yz

Taking the computed values from these evaluations and dividing by a million gives the values used on the 

J-records since the dummy material terms are defined as a million. The centroid of the blade crosssectional area is b/2 (0.676 inches) above the panel skin reference surface.
56

Figure 14. Model of blade-stiffened panel using smeared-stiffener-modeling approach.

Figure 15. Model of blade-stiffened panel using discrete-stiffener-modeling approach.

Figure 16. Model of blade-stiffened panel using branched-plate-modeling approach.
57

Material properties and laminate construction are defined using both the historical STAGS approach (i.e.,

STAGS versions prior to GCP) and the current GCP approach. Material modeling for an elastic 

orthotropic material using the historical STAGS approach requires data on the I-1 and I-2 records to

define the material properties and the K-1 and K-2 records to define the laminate fabrication data.

Material modeling using the current GCP approach requires data on the I-5a and I-6a records to define the 

material properties and the I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e records to define the fabrication.

The blade stiffeners have a rectangular cross-sectional area. For the metal panels, the stiffeners have a

thickness of 0.58 inches and a height of 1.352 inches. Using the J-1 and J-3b records, the corners of the 

rectangular subelement are defined with the origin of the stiffener cross-sectional coordinate systems

located at the subelement’s center. Input on the K-6 record identifies the offset of the stiffener center

from the shell reference surface.

Loading is specified as a uniform membrane pre-buckling load in the panel skin and blade stiffeners. It is

specified using the Q-1 and Q-5 records. Boundary condition on the displacements are specified using

the P-1 and P-2 records. The buckling boundary conditions along the four edges of the panel skin are 

simply supported and defined by:

At x=0, L; v=w=θx=0

At y=0, W; u=w=θy=0

Numerical Results and Discussion

The uniform pre-buckling membrane stress distributions in the panel skin and blade stiffeners are taken

from Stroud, Greene, and Anderson (1984). For a pre-stress in-plane longitudinal stress resultant loading

of Nx=1000 lb/in., the load distribution between the panel skin and the blade stiffeners has been given

earlier and depends on the fabrication of the skin and stiffeners. For a pre-stress in-plane shear stress

resultant loading of Nxy=1000 lb/in., the entire in-plane shear load is carried by the panel skin and no

shear load is carried by the blade stiffeners. The eigenvalue analysis has a convergence tolerance of 10-4

and the number of eigenpairs requested is four. No shift is used in the eigen solution.

A summary of the buckling analysis results is given in Table 8. These results are consistent with the

finite element reported by Stroud, Greene and Anderson (1984) using the EAL finite element code.

Buckling mode shapes for compression and shear loadings are shown in Figures 17 and 18 for the 

smeared-stiffener model, in Figures 19 and 20 for the discrete-stiffener model, and in Figures 21 and 22

for the branched-plate model. The smeared-stiffener model essentially gives an orthotropic plate solution

that in some cases is sufficient. The discrete-stiffener model does permit stiffened-panel-buckling modes

to be predicted (modes with local skin buckling between stiffeners). The branched-plate model permits

stiffened-panel-buckling modes to be predicted as well as cross-sectional deformations within the planestress formulation used to model the cross-sectional elements of the stiffeners.
58

Table 8. Summary of buckling factors for compression and shear loads for three different panel

configurations using different finite element modeling approaches.

Applied Load, lb/in. Buckling Factor

NASA TP-2215 STAGS

Panel

No.

Nx Nxy Smeared EAL Smeared Discrete Branched

1 1000 0 0.9970 1.0030 1.0268 0.8499 1.0189

1 0 1000 1.4683 1.5525 1.6924 1.6279 1.5805

2 1000 0 0.9969 0.9759 1.0094 0.8269 0.9807

2 0 1000 0.9823 0.8138 1.0690 0.8651 0.8309

3 1000 0 0.9097 0.2965 0.9270 0.3008 0.3121

3 0 1000 0.6062 0.2767 0.6825 0.3208 0.2906

Buckling analyses were performed for different panels under different loading conditions and using

different finite element modeling approaches. The results are summarized in Table 8 and are shown to be

consistent with results from NASA TP-2215. Contour plots of the out-of-plane component of the

buckling mode shapes corresponding to both compression and shear load cases are shown in Figures 17

through 23. Under compression load, the smeared-stiffener models predict a overall buckling mode

shape with one half wave in each direction (see Figures 17a and 18a). Under shear loading, the smearedstiffener models predict one longitudinal half wave and several half waves across the panel perpendicular

to the stiffener direction (see Figures 17b and 18b). As the fidelity of the finite element model is

increased to a discrete-stiffener model, Panels 3 and 2 still exhibit long wavelength shear buckles as

shown in Figures 19b and 20b, respectively. However, Panel 3 (metal panel with a thin skin) exhibits a 

stiffened panel buckling model with eight half waves along the panel length and one half wave between

stiffeners (see Figure 19a). The thick skin panel (Panel 2) exhibits an overall buckling mode (see Figure 

20a). Increasing the modeling fidelity further to a branched-plate model allows cross-sectional

deformations of the blade stiffeners to be simulated. The buckling modes are shown in Figures 21

through 23 for Panels 3, 2, and 1, respectively. The compression-loaded Panels 2 and 1 exhibit Euler 

buckling mode shapes and demonstrate the need to plate elements to be capable of buckling in their own

plane.
59

(a) Pure membrane compression prebuckling stress state, Nx=1000 lb/in.

(b) Pure membrane shear prebuckling stress state, Nxy=1000 lb/in.

Figure 17. Buckling mode shapes for the metal blade-stiffened panel with a thin skin (Panel 3) obtained

using the smeared-stiffener modeling approach.

-1.0

+1.0
60

(a) Pure membrane compression prebuckling stress state, Nx=1000 lb/in.

(b) Pure membrane shear prebuckling stress state, Nxy=1000 lb/in.

Figure 18. Buckling mode shapes for the metal blade-stiffened panel with a thick skin (Panel 2) obtained

using the smeared-stiffener modeling approach.

-1.0

+1.0
61

(a) Pure membrane compression prebuckling stress state, Nx=1000 lb/in.

(b) Pure membrane shear prebuckling stress state, Nxy=1000 lb/in.

Figure 19. Buckling mode shapes for the metal blade-stiffened panel with a thin skin (Panel 3) obtained

using the discrete-stiffener modeling approach.

-1.0

+1.0
62

(a) Pure membrane compression prebuckling stress state, Nx=1000 lb/in.

(b) Pure membrane shear prebuckling stress state, Nxy=1000 lb/in.

Figure 20. Buckling mode shapes for the metal blade-stiffened panel with a thick skin (Panel 2) obtained

using the discrete-stiffener modeling approach.

-1.0

+1.0
63

(a) Pure membrane compression prebuckling stress state, Nx=1000 lb/in.

(b) Pure membrane shear prebuckling stress state, Nxy=1000 lb/in.

Figure 21. Buckling mode shapes for the metal blade-stiffened panel with a thin skin (Panel 3) obtained

using the branched-plate modeling approach.

-1.0

+1.0
64

(a) Pure membrane compression prebuckling stress state, Nx=1000 lb/in.

(b) Pure membrane shear prebuckling stress state, Nxy=1000 lb/in.

Figure 22. Buckling mode shapes for the metal blade-stiffened panel with a thick skin (Panel 2) obtained

using the branched-plate modeling approach.

-1.0

+1.0
65

(a) Pure membrane compression prebuckling stress state, Nx=1000 lb/in.

(b) Pure membrane shear prebuckling stress state, Nxy=1000 lb/in.

Figure 23. Buckling mode shapes for the composite blade-stiffened panel (Panel 1) obtained using the 

branched-plate modeling approach.

-1.0

+1.0
66

STAGS Input Files

The STAGS input files are provided in several subdirectories based on the panel configuration (Panel 1,

Panel 2, or Panel 3), pre-buckling membrane stress state (compression or shear), and modeling approach

(branched plate approach, discrete-stiffener approach, or smeared-stiffener approach). These 

subdirectories are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Stiffened-panel

Subdirectories for this test case are organized by specific panel number (Panel-1, Panel-2, or Panel-3).

Under each panel number subdirectory the two load cases (Compression and Shear) are defined as

subdirectories. Then under each load case, an additional subdirectory structure is defined for the different

structural modeling approaches (Branched-plate, Discrete-stiffener, and Smeared-stiffener).

Representative input file listings are provided to illustrate the various modeling approaches and required

STAGS input records.

Branched Model of Panel 1 (composite)

Panel 1 is a composite blade-stiffened panel with a laminated panel skin and laminated blade stiffeners.

This configuration corresponds to Example 1 in NASA TP-2215. The input file included here is for the

uniform compression case with an overall Nx membrane loading of –1000 lb/in. This compression load is

carried partly by the skin and partly by the stiffeners as indicated by the load magnitudes specified on the

Q-5 records. The load distributions were taken from NASA TP-2215. These input files are given in:

../Stiffened-panel/Panel-1/Compression/Branched-plate

cbranched.inp (for S1 processor)

Blade stiffened panel with laminated skin - TP 2215 Example 1 $a-1

0 0 0 0 0 3 $b-1

1 -240.0 / 2 0.0 / 3 -30.0 $b-1b model rotations

13 0 0 12 0 $b-2

3 2 5 0 0 1 $b-3

37 3 37 3 37 5 37 3 37 5 37 3 37 5 ,

37 3 37 5 37 3 37 5 37 3 37 3 $f-1

1 2 2 4 $g-1 connections

1 2 3 4

3 2 4 4

3 2 5 4

5 2 6 4

5 2 7 4

7 2 8 4

7 2 9 4

9 2 10 4

9 2 11 4

11 2 12 4

11 2 13 4 $ g-1 connections

C

C Material definition for Example 2 and 4

C

1 $i-1 material data

10.5e6 .32 $i-2 aluminium

C

C Material definition for Example 1

C

2 $i-1 G/E material data
67

19.0E+6 0.0378 0.93E+6 0.1 0.0 1.89E+6 $i-2

C

C Dummy material data tas multipliers for composite stringer

C stiffness terms (EA, EIyy, EIzz, GJ)

C

3 $i-1 dummy material multipliers

1.0E6 0.0 1.0E6 0.1 0.0 1.0E6 $i-2

C

C ---- GCP Input -----

C

C Material for Examples 2 and 4

C

ISOELASTIC 1 1 1 $I-5

10.5E+6 0.32 2.0E-5 4*0.0 $i-6a E, Nu, rho

C

C Material for Example 1

C

ORTHOELAST 2 1 1 $I-5

19.0E6 1.89E6 1.89E6, $I-7a E11, E22, E33

0.93E6 0.93E6 0.93E6, $I-7a G12, G13, G23

0.38 0.38 0.38, $I-7a nu12, nu13, nu23

2.0E-5, $i-7a rho

3*0.0, $i-7a CTE's

3*0.0, $i-7a CME's

0.0 0.0 $i-7a ref. temp. and moisture

C

C Fabrication data

C

SHELL_FABRICATION 1 1 0 0 0 $I-21a Panel skin for Example 2

1 $I-21a isotropic material

0.084 $I-21c thick skin

0.0 $i-21d

SHELL_FABRICATION 2 1 0 0 0 $I-21a Panel skin for Example 2

1 $I-21a isotropic material

0.050 $I-21c thin skin

0.0 $i-21d

SHELL_FABRICATION 3 1 0 0 0 $I-21a Blade stiffeners for Examples 2 and 4

1 $I-21a isotropic material

0.058 $I-21c blade stiffeners

0.0 $i-21d

SHELL_FABRICATION 4 28 0 0 0 $I-21a Panel skin for Example 1

28*2 $I-21a orthotropic material

28*0.0055 $I-21c laminated skin [+/-45 / -/+45 /0/90_9]_s

+45. -45. -45. 45. 0.0 , $i-21d

90. 90. 90. 90. 90. 90. 90. 90. 90. , $i-21d

90. 90. 90. 90. 90. 90. 90. 90. 90. , $i-21d

0.0 +45. -45. -45. 45. $i-21d

SHELL_FABRICATION 5 12 0 0 0 $I-21a Blade stiffeners for Example 1

12*2 $I-21a orthotropic material

12*0.0055 $I-21c laminated stiffener [+/-45 / -/+45 /0_2]_s

+45. -45. -45. 45. 0.0 0.0 , $i-21d

0.0 0.0 +45. -45. -45. 45. $i-21d

END

C

C --- End GCP input ---

C

C metal stringers

C

1 3 1 1 8.5481e-5 0.0 0.0 $j-1 stringer stiffener

-.029 +.029 -0.676 +0.676 $j-3b

C

C composite stringers

C
68

2 1 3 0 0.00092 0.0 0.0 $j-1 general stiffener

0.7609 0.1159 0.00023 0.0 $j-2a A, Iyy, Izz, Iyz

C

C Fabrication definitions

C (thick skin; thin skin; stringer)

C

1 1 1 $k-1 panel skin thickness - Example 2

1 0.084 $k-2 thick skin

2 1 1 $k-1 panel skin thickness - Example 4

1 0.050 $k-2 thin skin

3 1 1 $k-1 blade stringer thickness - Examples 2 & 4

1 0.058 $k-2

4 1 28 $k-1 laminated panel skin - Example 1

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

5 1 12 $k-1 laminated stringer - Example 1

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

C

C ------- Define shell units: skin segment then stringer, etc

C

C

C Panel Skin Segment

C

2 $m-1

0.0 30.0 0.0 2.5 $m-2

4 $m-5 laminated panel skin
69

410 $n-1

1 6 1 1 $p-1

0 0 0 1 $q-1

-811.35 0.0 0.0 $q-5 Nx in skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 2.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

5 $m-5 laminated stringer

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-697.67 0.0 0.0 $q-5 Nx in stringer for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 2.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

4 $m-5 laminated panel skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-811.35 0.0 0.0 $q-5 Nx in skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 7.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

5 $m-5 laminated stringer

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-697.67 0.0 0.0 $q-5 Nx in stringer for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 7.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

4 $m-5 laminated panel skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-811.35 0.0 0.0 $q-5 Nx in skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 12.5 0.0 $m-4d iglobe=4
70

-90.0 0.0 0.0 $m-4e

5 $m-5 laminated stringer

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-697.67 0.0 0.0 $q-5 Nx in stringer for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 12.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

4 $m-5 laminated panel skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-811.35 0.0 0.0 $q-5 Nx in skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 17.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

5 $m-5 laminated stringer

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-697.67 0.0 0.0 $q-5 Nx in stringer for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 17.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

4 $m-5 laminated panel skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-811.35 0.0 0.0 $q-5 Nx in skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 22.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

5 $m-5 laminated stringer

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-697.67 0.0 0.0 $q-5 Nx in stringer for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1
71

0.0 30.0 0.0 5.0 $m-2

0.0 22.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

4 $m-5 laminated panel skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-811.35 0.0 0.0 $q-5 Nx in skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 27.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

5 $m-5 laminated stringer

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-697.67 0.0 0.0 $q-5 Nx in stringer for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 2.5 $m-2

0.0 27.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

4 $m-5 laminated panel skin

410 $n-1

1 1 1 6 $p-1

0 0 0 1 $q-1

-811.35 0.0 0.0 $q-5 Nx in skin for overall Nx=1000

1 $r-1

cbranched.bin (for S2 processor)

Blade stiffened panel with laminated skin - TP-2215, Example 1 $a-1

1 1 0 $b-1

1.0 1.0 1.0 $c-1

1000 .0001 0 $d-2

4 $d-3

cbranched.pin (for STAPL processor)

Blade-stiffened Panel - TP-2215

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0
72

Branched Model of Panel 3 (metal)

Panel 3 is a metal blade-stiffened panel with a thin skin. This configuration corresponds to Example 4 in

NASA TP-2215. The input file included here is for the uniform compression case with an overall Nx

membrane loading of –1000 lb/in. This compression load is carried partly by the skin and partly by the 

stiffeners as indicated by the load magnitudes specified on the Q-5 records. The load distributions were 

taken from NASA TP-2215. These input files are given in:

../Stiffened-panel/Panel-3/Compression/Branched-plate

branched.inp (for S1 processor)

Blade stiffened panel with thin skin - TP 2215 Example 4 $a-1

0 0 0 0 0 3 $b-1

1 -240.0 / 2 0.0 / 3 -30. $b-1b model rotations

13 0 0 12 0 $b-2

2 0 5 $b-3

37 3 37 3 37 5 37 3 37 5 37 3 37 5 ,

37 3 37 5 37 3 37 5 37 3 37 3 $f-1

1 2 2 4 $g-1 connections

1 2 3 4

3 2 4 4

3 2 5 4

5 2 6 4

5 2 7 4

7 2 8 4

7 2 9 4

9 2 10 4

9 2 11 4

11 2 12 4

11 2 13 4 $ g-1 connections

C

C Material definition for Example 2 and 4

C

1 $i-1 material data

10.5e6 .32 $i-2 aluminium

C

C Material definition for Example 1

C

2 $i-1 G/E material data

19.0E+6 0.0378 0.93E+6 0.1 0.0 1.89E+6 $i-2

C

C Fabrication definitions

C (thick skin; thin skin; stringer)

C

1 1 1 $k-1 panel skin thickness - Example 2

1 0.084 $k-2 thick skin

2 1 1 $k-1 panel skin thickness - Example 4

1 0.050 $k-2 thin skin

3 1 1 $k-1 blade stringer thickness - Examples 2 & 4

1 0.058 $k-2

4 1 28 $k-1 laminated panel skin - Example 1

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2
73

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 90.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

5 1 12 $k-1 laminated stringer - Example 1

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 0.0 $k-2

2 0.0055 +45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 -45.0 $k-2

2 0.0055 +45.0 $k-2

C

C ------- Define shell units: skin segment then stringer, etc

C

C

C Panel Skin Segment

C

2 $m-1

0.0 30.0 0.0 2.5 $m-2

2 $m-5 shell wall-thin skin

410 $n-1

1 6 1 1 $p-1

0 0 0 1 $q-1

-761.23 0.0 0.0 $q-5 Nx in thin skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 2.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

3 $m-5 shell wall

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-883.03 0.0 0.0 $q-5 Nx in stringer for thin skin for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1
74

0.0 30.0 0.0 5.0 $m-2

0.0 2.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

2 $m-5 shell wall-thin skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-761.23 0.0 0.0 $q-5 Nx in thin skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 7.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

3 $m-5 shell wall

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-883.03 0.0 0.0 $q-5 Nx in stringer for thin skin for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 7.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

2 $m-5 shell wall-thin skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-761.23 0.0 0.0 $q-5 Nx in thin skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 12.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

3 $m-5 shell wall

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-883.03 0.0 0.0 $q-5 Nx in stringer for thin skin for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 12.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

2 $m-5 shell wall-thin skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-761.23 0.0 0.0 $q-5 Nx in thin skin for overall Nx=1000

1 $r-1

C

C Stringer Segment
75

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 17.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

3 $m-5 shell wall

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-883.03 0.0 0.0 $q-5 Nx in stringer for thin skin for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 17.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

2 $m-5 shell wall-thin skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-761.23 0.0 0.0 $q-5 Nx in thin skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 22.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

3 $m-5 shell wall

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-883.03 0.0 0.0 $q-5 Nx in stringer for thin skin for overall Nx=1000

1 $r-1

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 5.0 $m-2

0.0 22.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

2 $m-5 shell wall-thin skin

410 $n-1

1 6 1 6 $p-1

0 0 0 1 $q-1

-761.23 0.0 0.0 $q-5 Nx in thin skin for overall Nx=1000

1 $r-1

C

C Stringer Segment

C

2 4$m-1

0.0 30.0 0.0 1.352 $m-2

0.0 27.5 0.0 $m-4d iglobe=4

-90.0 0.0 0.0 $m-4e

3 $m-5 shell wall

410 $n-1

1 3 1 6 $p-1

0 0 0 1 $q-1

-883.03 0.0 0.0 $q-5 Nx in stringer for thin skin for overall Nx=1000

1 $r-1
76

C

C Panel Skin Segment

C

2 4$m-1

0.0 30.0 0.0 2.5 $m-2

0.0 27.5 0.0 $m-4d iglobe=4

0.0 0.0 0.0 $m-4e

1 $m-5 shell wall-thin skin

410 $n-1

1 1 1 6 $p-1

0 0 0 1 $q-1

-761.23 0.0 0.0 $q-5 Nx in thin skin for overall Nx=1000

1 $r-1

branched.bin (for S2 processor)

Blade stiffened panel with thin skin - TP-2215, Example 4 $a-1

1 1 0 $b-1

1.0 1.0 1.0 $c-1

1000 .0001 0 $d-2

4 $d-3

branched.pin (for STAPL processor)

Blade-stiffened Panel - TP-2215

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

Discrete-Stiffener Model of Panel 3 (metal)

Panel 3 is a metal blade-stiffened panel with a thin skin. This configuration corresponds to Example 4 in

NASA TP-2215. The input file included here is for the uniform compression case with an overall Nx

membrane loading of –1000 lb/in. These input files are given in:

../Stiffened-panel/Panel-3/Compression/Discrete-stiffener

discrete.inp (for S1 processor)

Discretely stiffened panel with thin skin - TP 2215 Example 4 $a-1

0 0 0 0 0 3 $b-1

1 -240.0 / 2 0.0 / 3 -30.0 $b-1b model rotations

1 0 1 $b-2

1 1 2 $b-3

37 37 $f-1

1 0 6 $ f-2 discrete stiffeners including along boundaries

1 $i-1 material records

10.5e6 .32 $i-2

1 3 1 1 8.5481e-5 0.0 0.0 $j-1 stringer stiffener
77

-.029 +.029 -0.676 +0.676 $j-3b

1 1 1 0 0 $k-1

1 .084 $k-2 thick skin

2 1 1 0 0 $k-1

1 .050 $k-2 thin skin

2 0 $m-1

0.0 30.0 0.0 30.0 $m-2a

2 $m-5 thin skin case - example 4 in TP 2215

410 $n-1

1 0.0 0.0 0.676 $o-2a discrete stringers (constant y)

0 0 0 2.5 0.0 30.0 $o-2b

1 0.0 0.0 0.676 $o-2a discrete stringers (constant y)

0 0 0 7.5 0.0 30.0 $o-2b

1 0.0 0.0 0.676 $o-2a discrete stringers (constant y)

0 0 0 12.5 0.0 30.0 $o-2b

1 0.0 0.0 0.676 $o-2a discrete stringers (constant y)

0 0 0 17.5 0.0 30.0 $o-2b

1 0.0 0.0 0.676 $o-2a discrete stringers (constant y)

0 0 0 22.5 0.0 30.0 $o-2b

1 0.0 0.0 0.676 $o-2a discrete stringers (constant y)

0 0 0 27.5 0.0 30.0 $o-2b

1 1 1 1 $p-1

0 0 0 1 $q-1

-1000.0 000.0 0.0 $q-5

1 0 0 $r-1

discrete.bin (for S2 processor)

Discretely stiffened panel with thin skin - TP 2215 Example 4 $a-1

1 1 0 $b-1

1.0 1.0 1.0 $c-1

1000 .0001 0 $d-2

4 $d-3

discrete.pin (for STAPL processor)

Blade-stiffened Panel - TP-2215

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

0 0 0 0 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-0.5 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

Smeared-Stiffener Model of Panels 3 (metal)

Panel 3 is a metal blade-stiffened panel with a thin skin. This configuration corresponds to Example 4 in

NASA TP-2215. The input file included here is for the uniform compression case with an overall Nx

membrane loading of –1000 lb/in. These input files are given in:
78

../Stiffened-panel/Panel-3/Compression/Smeared-stiffener

smeared.inp (for S1 processor)

Smeared stiffened panel with thin skin - TP-2215, Example 4 $a-1

0 0 0 0 0 3 $b-1

1 -240.0 / 2 0.0 / 3 -30.0 $b-1b model rotations

1 0 0 0 0 $b-2

1 1 2 $b-3

37 37 $f-1

1 $i-1 material records

10.5e6 .32 $i-2

1 3 1 1 8.5481e-5 0.0 0.0 $j-1 stringer stiffener

-.029 +.029 -0.676 +0.676 $j-3b

1 1 1 0 1 $k-1 thick skin with smeared stringers

1 .084 $k-2 thick skin

1 5.0 0.0 0.0 .676 $k-6 smeared stringers

2 1 1 0 1 $k-1 thin skin with smeared stringers

1 .050 $k-2 thin skin

1 5.0 0.0 0.0 .676 $k-6 smeared stringers

2 0 $m-1

0.0 30.0 0.0 30.0 $m-2a

2 $m-5 thin skin case (example 4 in TP 2215)

410 $n-1

1 1 1 1 $p-1

0 0 0 1 $q-1

-1000.0 0.0 0.0 $q-5 Nx=-1000.0 uniform stress state

1 0 0 $r-1

smeared.bin (for S2 processor)

Smeared stiffened panel with thin skin - TP-2215, Example 4 $a-1

1 1 0 $b-1

1.0 1.0 1.0 $c-1

1000 .0001 0 $d-2

4 $d-3

smeared.pin (for STAPL processor)

Blade-stiffened Panel - TP-2215

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -240.0 / 2 0.0 / 3 -30.0
79

Problem References

Rankin, C. C., Brogan F. A., Loden, W., and Cabiness, H., Structural Analysis of General Shells – STAGS

User Manual, Version 4.0, Lockheed Martin Advanced Technology Center, Palo Alto, CA, June 2000.

Stroud, W. Jefferson, Greene, William H., and Anderson, Melvin S., Buckling Loads of Stiffened Panels

Subjected to Combined Longitudinal Compression and Shear: Results Obtained with PASCO, EAL, and

STAGS Computer Programs, NASA TP-2215, January 1984.

Whetstone, W. D., “EISI-EAL: A General Engineering Analysis and Design Language,” Finite Elements

in Analysis and Design, Vol. 2, Nos. 1-2, April 1986, pp. 219-235
80

Raasch Curved Hook Problem

Background

The Raasch curved hook problem was first publicly report by Harder at the Structures Technical Forum 

during the 1991 MSC World Users’ Conference. The problem is essentially a curved 2-D structure with a 

reverse in shape near the boundary. The opposite end (or tip) is loaded by a unit in-plane shear loading.

The issue with this test case is that shell elements without shear flexibility tend to converge to within 5%

of the 3D solution, while models with shear flexibility tend not to converge unless shell normal (drilling) 

degrees of freedom are included. Hoff et al. (1995), Knight (1997), and MacNeal et al. (1998) have 

studied this problem using a variety of element formulations and mesh discretizations. The dimensions,

material properties and loading are defined in Figure 24 using U. S. customary units.

Figure 24. Raasch curved hook problem: geometry, material properties, and loading.

The hook has a uniform thickness t, and has width (in the z-direction) w, and an in-plane shear load P

along the free edge at point C having a magnitude of unity. The response of the hook exhibits coupling

between bending, extension, and twist. The mesh is defined as the number of elements in the width

direction nw by the number of elements along the hook length nL (i.e., nw×nL). Meshes involving triangular 

elements are developed by subdividing each 4-node quadrilateral element into two triangular elements.

The nodes are distributed equally in each direction. The reference solution for the tip deflection wref in

the direction of the loading is taken as 4.9352 inches as done by Knight (1997).

Modeling and Analysis Process

The STAGS model is generated using two shell units with the cylindrical shell surface geometry

(ISHELL=5). Material properties and membrane construction are defined using both the historical

STAGS approach and the current GCP approach. Mesh discretization studies include different levels of 

mesh refinement and different element types. Mesh refinement is readily performed by changing the 

number of nodes in each direction on the F-1 record (i.e., the mesh is defined a nw×nL as mesh of

elements, one less than the number of nodes). Element type is selected using the N-1 record (KELT).

Representative finite element meshes using 3-node, 4-node, and 9-node shell elements and 8-node solid

element are shown in Figure 25 for the 10×68 mesh.

C
81

Material modeling for an elastic isotropic material using the historical STAGS approach requires data on

the I-1 and I-2 records to define the material properties and the K-1 and K-2 records to define the 

construction or fabrication data. Material modeling using the current GCP approach requires data on the 

I-5a and I-6a records to define the material properties and the I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e

records to define the fabrication.

Loading is specified as a uniformly distributed shear load across the free end of the curved hook. For the 

2D shell elements, it is specified as a line load (Nxy = 1/20 lb/in.) using the Q-1, Q-2, and Q-3 records.

For the 3D 8-node solid element (E881), the nodal loads are specified manually by computing the workequivalent nodal forces per element face and then defining the assembled nodal loads for that face of the 

hook. As a check on the loading, the summation of the equilibrium forces across the loaded edge in the 

direction of applied loading should equal unity (i.e., total force equal to edge length times line load for 2D

elements and equal to face traction times the face area for 3D elements).

For the 3D meshes, only two 8-node solid elements are used through the hook thickness. The loaded face 

involves the number of elements along the hook width or nw. Thus the nodal force for each element on

that face of the hook is given by:

e

n

n

P P

4

=

where P is the total unit in-plane shear load and ne is the total number of element faces across the loaded

face – assuming equal area for the element faces. As a result corner nodes on the loaded face will have an

applied force of Pn, other nodes on the bounding edges of the loaded face will have an applied force of 2

Pn, and interior nodes of the face will have an applied force of 4 Pn. The sum of all the nodal forces

should equal the total applied shear load – which has a value of unity.

Boundary condition on the displacements are specified using the P-1 and P-2 records for the shell element

models. Finite element models using the solid elements have the homogeneous boundary conditions

imposed using the applied displacement loading records (Q-records) for each nodal layer through the

hook thickness. The one end is fully clamped and all other edges are free. The drilling degrees of

freedom are suppressed for the E480 element and they are retained for the E410 element. These drilling

freedoms are constrained for the E480 element using the Q-3 records with the exterior looping feature.

The E330 (MIN3) element does have introduce artificial drilling stiffness (a small number times the 

smallest diagonal term of the element stiffness matrix) automatically. Hence two cases are considered:

one case restrains all drilling degrees of freedom and the other case leaves all the drilling degrees of

freedom unrestrained and uses the penalty approach implemented within the element. Results are

presented for both cases.
82

Figure 25. Representative finite element discretization (10×68 mesh) 

of Raasch curved hook.

(c) 9-node E480 (ANS) quadrilateral

shell element.

(a) 4-node E410 quadrilateral

shell element.

(b) 3-node E330 (MIN3) triangular 

shell element.

(d) 8-node E881 (ANS) solid

brick element.
83

Table 9. Mesh refinement study for three shell finite element and one solid finite

elements in STAGS – reference solution is 4.9352 inches (Knight, 1997).

Mesh of Normalized Tip Deflection wc/wref

Elements

nw×nL

E330 Shell

Element

**

E410 Shell

Element

E480 Shell

Element

**

E881 Solid

Element

*

1×9 0.4407 (1.0656)+ 0.9083 0.9776 0.7445

3×17 0.3749 (1.1336)+ 0.9398 0.9993 0.9484

5×34 0.5505 (1.2623)+ 0.9512 1.0085 0.9702

10×68 0.7963 (1.6547)+ 0.9541 1.0164 0.9856

20×136 1.1548 (2.8374)+ 0.9548 1.0182 0.9967

40×272 1.2243 (3.4904)+ 0.9550 1.0056 ---

*

For the solid element models, only two 8-node solid elements through the thickness are considered. **

The shear correction factors are set equal to 5/6. +

The number inside the parentheses was computed with the drilling degrees of freedom unrestrained and a

penalty parameter is used with the drilling stiffness, while the outside number was computed by

restraining all drilling degrees of freedom to zero.

Numerical Results and Discussion

Results are presented for the tip deflection at free end in the z-direction denoted by wc normalized by the

reference solution wref equal to 4.9352 inches (Knight, 1997).

Tip displacement results shown in Table 9 indicate that finite element models using the E410 and E480

shell elements and the E881 solid element converge quickly to the reference solution, while finite element

models using the E330 shell element do not appear to be converging – with or without the drilling degrees

of freedom. For the E410 element, the membrane response is nearly bilinear except for the contribution to

edge’s in-plane normal displacement from the drilling degrees of freedom. These results are consistent

with available published solutions.

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Raasch

Typical 2D Shell Model Input Files

The following text files give the input for the hook model using the E480 9-node ANS shell element in

STAGS with a 10×68 (nw×nL) mesh of elements.

hook2D.inp (for S1 processor)

Raasch Curved Hook Problem - 2D $a-1

C

C Curved hook problem with unit in-plane shear load at tip

C Reference solution for w/t=10 is 4.9352 in. for tip

C displacement in the direction of the loading

C
84

C Problem originally posed by Ingo Raasch, BMW in Germany

C at the 1995 MSC User's Forum

C

C Ref. Knight, "Raasch Challenge for Shell Elements"

C AIAA Journal, Vol. 35, No. 2, Feb. 1997,

C pp. 375-381.

C

0 0 0 0 0 3 $b-1

1 30.0 / 2 30.0 / 3 -90.0 $ b-1b Model rotations

2 0 0 1 0 $b-2

1 0 1 0 0 1 $b-3

C

C Mesh discretization

C

CC 2 2 2 9 $f-1 mesh in both units ( 1 x 9 mesh of 4-node elements)

CC 4 3 4 16 $f-1 mesh in both units ( 3 x 17 mesh of 4-node elements)

CC 6 5 6 31 $f-1 mesh in both units ( 5 x 34 mesh of 4-node elements)

CC11 9 11 61 $f-1 mesh in both units (10 x 68 mesh of 4-node elements)

CC21 16 21 121 $f-1 mesh in both units (20 x 136 mesh of 4-node elements)

CC 3 3 3 17 $f-1 mesh in both units ( 1 x 9 mesh of 9-node elements)

CC 7 5 7 31 $f-1 mesh in both units ( 3 x 17 mesh of 9-node elements)

CC11 9 11 61 $f-1 mesh in both units ( 5 x 34 mesh of 9-node elements)

21 17 21 121 $f-1 mesh in both units (10 x 68 mesh of 9-node elements)

CC41 31 41 241 $f-1 mesh in both units (20 x 136 mesh of 9-node elements)

C

C Connect the shell units

C

1 2 2 2 $g-1 shell unit connection

C

C Material definition (traditional approach)

C

1 0 $i-1 material data

3300.0 0.35 0.0 0.03861 $i-2 Modulus, Poisson's ratio,weight density

C

C ======================================================

C Begin GCP Input for material and fabrication data

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $i-2 isotropic elastic

3300.0, $i-6a Young's modulus, psi

0.35, $i-6a Poisson's ratio

1.0e-4, $i-6a Mass density, slugs/in^3

4*0.0 $i-6a unused values

SHELL_FABRICATION 1 1 0 1 0 $i-5a shell fabrication

1 $i-21a Layer material ID

2.0 $i-21c Layer thickness, in.

0.0 $i-21d Layer orientation angle, degrees

0.8333 0.8333 $i-21e shear correction factors

SOLID_FABRICATION 1 1 0 0 $i-5a solid fabrication

1.0 $i-22a element thickness

C

END $I-5a End GCP input

C =====================================================

C

C Shell wall fabrication (traditional approach)

1 1 1 $k-1 wall card

1 2.0 0.0 $k-2 Mat ID, thickness, orientation

C

C define first segment

C

5 4 0 0 0 0 $m-1 Cylinder geometry

0.0 20.0 0.0 60.0 14.0 $m-2

0.0 14.0 0.0 $m-4d Orient shell unit

90.0 0.0 0.0 $m-4e
85

-1 $m-5 Fabrication

480 $n-1 Element selection

3 6 3 2 $p-1 boundary conditions

1 $q-1 no loading

1 1 $q-2 For E430, E480 elements only

0.0 -1 6 0 0 0 $q-3 zero-out drilling freedom

0 $r-1

C

C define second segment

C

5 4 0 0 0 0 $m-1 Cylinder geometry

0.0 20.0 0.0 150.0 46.0 $m-2

0.0 -16.0 51.96152422 $m-4d Orient shell unit

0.0 0.0 0.0 $m-4e

-1 $m-5 Fabrication

480 $n-1 Element selection

3 6 3 3 $p-1 boundary conditions

C

C Tip loading (across column of edge 1)

C

1 0 $q-1 Applied tip load

1 2 0 $q-2

0.05 3 1 0 1 0 $q-3 Uniform line load along tip

C $ For E480 elements only

0.0 -1 6 0 0 0 $q-3 zero-out drilling freedom

0 0 0 0 0 0 1 $r-1 Selected displacements at tip

0 1 $r-2

hook2D.bin (for S2 processor)

Raasch hook problem execution parameters $a-1

C

C linear stress analysis

C

0 1 0 0 0 0 0 -1 $b-1

0.202626033 $c-1 reciprocal of reference solution

Typical 3D Solid Model Input Files

The following text files give the input for the hook 3D model using the E881 8-node solid element in

STAGS with a 10×68 (nw×nL) mesh of elements and just two 8-node solid elements through the hook

thickness).

hook3D.inp (for S1 processor)

Raasch Curved Hook Problem - 3D $a-1

C

C Curved hook problem with unit in-plane shear load at tip

C Reference solution for w/t=10 is 4.9352 in. for tip

C displacement in the direction of the loading

C

C Problem originally posed by Ingo Raasch, BMW in Germany

C at the 1991 MSC User's Forum

C

C Ref. Knight, "Raasch Challenge for Shell Elements"

C AIAA Journal, Vol. 35, No. 2, Feb. 1997,

C pp. 375-381.

C

0 0 0 0 0 3 $b-1

1 30.0 / 2 30.0 / 3 -90.0 $ b-1b Model rotations

2 0 0 1 0 $b-2
86

1 0 1 0 0 1 $b-3

C

C Mesh discretization

C

CC 2 2 2 9 $f-1 mesh in both units ( 1 x 9 mesh of 4-node elements)

CC 4 3 4 16 $f-1 mesh in both units ( 3 x 17 mesh of 4-node elements)

CC 6 5 6 31 $f-1 mesh in both units ( 5 x 34 mesh of 4-node elements)

11 9 11 61 $f-1 mesh in both units (10 x 68 mesh of 4-node elements)

CC21 16 21 121 $f-1 mesh in both units (20 x 136 mesh of 4-node elements)

C

C Connect the shell units

C

1 2 2 2 $g-1 shell unit connection

C

C Material definition (traditional approach)

C

1 0 $i-1 material data

3300.0 0.35 0.0 0.03861 $i-2 Modulus, Poisson's ratio,weight density

C

C ======================================================

C Begin GCP Input for material and fabrication data

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $i-2 isotropic elastic

3300.0, $i-6a Young's modulus, psi

0.35, $i-6a Poisson's ratio

1.0e-4, $i-6a Mass density, slugs/in^3

4*0.0 $i-6a unused values

SHELL_FABRICATION 1 1 0 1 0 $i-5a shell fabrication

1 $i-21a Layer material ID

2.0 $i-21c Layer thickness, in.

0.0 $i-21d Layer orientation angle, degrees

0.8333 0.8333 $i-21e shear correction factors

SOLID_FABRICATION 1 1 0 0 $i-5a solid fabrication

1.0 $i-22a element thickness

C

END $I-5a End GCP input

C =====================================================

C

C Shell wall fabrication (traditional approach)

C

1 1 1 $k-1 wall card

1 2.0 0.0 $k-2 Mat ID, thickness, orientation

C

C define first segment

C

5 4 0 0 2 1 $m-1 Cylinder geometry, 2 layers

0.0 20.0 0.0 60.0 14.0 $m-2

0.0 14.0 0.0 $m-4d Orient shell unit by translation

90.0 0.0 0.0 $m-4e and rotation

-1 $m-5 Fabrication

881 $n-1 Element selection

3 6 3 3 $p-1 boundary conditions

1 $q-1 Impose clamped BCs on end

1 3 $q-2

0.0 -1 1 0 1 0 3 1 0 0 1 $q-3 Set u=v=w=0 on Layer 1 along Column 1

0.0 -1 1 0 1 0 3 1 0 0 2 $q-3 Set u=v=w=0 on Layer 2 along Column 1

0.0 -1 1 0 1 0 3 1 0 0 3 $q-3 Set u=v=w=0 on Layer 3 along Column 1

1 $r-1

C

C define second segment

C

5 4 0 0 2 1 $m-1 Cylinder geometry, 2 layers

0.0 20.0 0.0 150.0 46.0 $m-2
87

0.0 -16.0 51.96152422 $m-4d Orient shell unit by translation

0.0 0.0 0.0 $m-4e and rotation

-1 $m-5 Fabrication

881 $n-1 Element selection

3 6 3 3 $p-1 boundary conditions

C

C Tip loading (across column of edge 1)

C where Pn = P/4/(number of elements on tip face)

C for 8-node solid elements with equal face areas

C Mesh Ne_tipface Pn

C 1x9 2 0.1250

C 3x17 4 0.0625

C 5x34 10 0.0250

C 10x68 20 0.0125

C 20x136 40 0.00625

C

1 0 $q-1 Applied tip load

1 9 0 $q-2

0.0125 1 1 1 1 0 0 0 0 0 1 $q-3 Corner (1,1) on Layer 1, Pn

0.0125 1 1 11 1 0 0 0 0 0 1 $q-3 Corner (nrow,1) on Layer 1, Pn

0.0125 1 1 1 1 0 0 0 0 0 3 $q-3 Corner (1,1) on Layer 3, Pn

0.0125 1 1 11 1 0 0 0 0 0 3 $q-3 Corner (nrow,1) on Layer 3, Pn

0.0250 1 1 1 1 0 0 0 0 0 2 $q-3 Midside at (1,1) on Layer 2, 2Pn

0.0250 1 1 11 1 0 0 0 0 0 2 $q-3 Midside at (nrow,1) on Layer 2, 2Pn

0.0250 1 1 2 1 0 9 0 1 0 1 $q-3 Edge 1 on Layer 1, 2Pn

0.0250 1 1 2 1 0 9 0 1 0 3 $q-3 Edge 1 on Layer 3, 2Pn

0.0500 1 1 2 1 0 9 0 1 0 2 $q-3 Interior centerline at Layer 2, 4Pn

C

C Output

C

0 0 0 0 0 0 1 $r-1 Selected displacements at tip

0 1 $r-2

hook3D.bin (for S2 processor)

Raasch hook problem execution parameters $a-1

C

C linear stress analysis

C

0 1 0 0 0 0 0 -1 $b-1

0.202626033 $c-1 reciprocal of reference solution

Problem References

Harder, R. L., “The Raasch Challenge,” presentation charts (12 charts) from the Structures Technical

Forum at the 1991 MSC World Users’ Conference, Los Angeles, CA, 1991.

Hoff, C. C., Harder, R. L., Campbell, G., MacNeal, R. H., and Wilson, C. T., “Analysis of Shell

Structures using MSC/NASTRAN’s Shell Elements with Surface Normals,” Proceedings of the 1995

MSC World Users’ Conference (University City, CA), MacNeal-Schwendler Corp., Paper No. 26, Los

Angeles, CA 1995, 18 pages.

Knight, Norman F., Jr., “Raasch Challenge for Shell Elements,” AIAA Journal, Vol. 35, No. 2, February

1997, pp. 375-381.

MacNeal, R. H., Wilson, C. T., Harder, R. L., Hoff, C. C., “The Treatment of Shell Normals in Finite 

Element Analysis,” Finite Element in Analysis and Design, Vol. 30, No. 3, August 1998, pp. 235-242.
88

Buckling and Collapse of Circular Cylinder with Square Cutouts

Background

To verify the nonlinear solution algorithm and nonlinear aspects of the shell element and corotational

formulations, the elastic collapse of a circular cylinder (R/t=433 and L/R=1.5) with two opposing central

rectangular cutouts (45° by L/3 in size) loaded by uniform end-shortening is studied. This problem

involves local radial deflections along the straight edges of the cutout that develop at a low load level and

become large prior to collapse. This shell problem was part of experimental and analytical studies by

Almroth and Holmes (1972) and extended to dynamic buckling by Almroth, Meller and Brogan (1974).

Hartung and Ball (1973) included this shell structure as one of the three challenge problems to assess

shell structural analysis capabilities. Almroth and Brogan (1981) studied the computational efficiency

and capability of the shell finite elements implemented in the STAGS finite element code. Knight et al.

(1989, 1995) also used this problem to assess the CSM Testbed capabilities for the static collapse of 

elastic shell. The geometry and material properties of the problem are defined in Figure 26 using U.S.

customary units.

Figure 26. Cylinder with cutouts: geometry and material properties.

Modeling and Analysis Process

Three separate STAGS finite element models are considered in this test case problem – both involve shell

elements. A summary of each model includes:

2-D shell model – Model the shell with shell finite elements in a single shell unit and using the irregular

grid modeling option – cutout1.inp.
89

2-D shell model – Model shell with shell finite elements in three shell units to model around the cutout –

cutout3.inp.

2-D shell model – Model the shell with shell finite elements in two shell units and use the connection

across a portion of a shell unit option – cutout2.inp.

The STAGS model is generated using a single shell unit with the cylindrical shell surface geometry

(ISHELL=5). Material properties and shell wall construction are defined using both the historical

STAGS approach and the current GCP approach. Mesh discretization studies include different levels of 

mesh refinement and different element types. Mesh refinement is readily performed by changing the 

number of rows and columns of nodes in each direction on the F-1 record. Element type is selected using

the N-1 record (KELT). Note that E430 uses two E330 triangular elements for each 4-node quadrilateral

subdomain.

Representative finite element models using Mesh 3 (19×33 mesh of nodes on the shell surface) are shown

in Figure 27 for different shell unit modeling approaches. The single shell unit model shown in Figure

27a illustrates the use of the irregular mesh option (see the N-8 records) for easy inclusion of rectangular 

cutouts. However, the irregular mesh option is not available for use with the triangular elements or solid

elements. Alternatively, two or three shell units may be used as shown in Figures 27b and 27c,

respectively. The two shell unit model requires special consideration for the shell unit junction along

only a portion of a shell unit boundary (see the G-2 records of the cutout2.inp input file). The three

shell unit model is straightforward to create in that three rectangular domains are defined and discretized

(see the cutout3.inp input file). Finite element models labeled as Mesh 3 using the 3-node, 4-node,

and 9-node shell elements are shown in Figure 28.

The S1 input file for the single shell unit model (cutout1.inp) contains input records (F-1 and N-8

records) for different finite element discretizations. The different meshes can be exercised by editing the 

input file and changing the records that are “commented.”

The nonlinear solutions were obtained using the perfect shell geometry – no initial geometric surface 

imperfections. The cutouts served as a sufficient “trigger” for the geometric nonlinearities to develop.

The material behavior is treated as linear elastic – no elastic-plastic behavior was considered. The value 

of the collapse load reported by Almroth and Holmes (1972) is 2250 pounds or 0.3045 P0. Almroth and

Brogan (1981) reported a nearly converged elastic collapse load of 2750 pounds or 0.3722 P0 obtained

using the STAGS E411 shell element. Difference may be attributed to thickness variations in the test

cylinder while uniform thickness in the analysis; initial surface imperfections that are not included in the

analysis; elastic material properties that differ from nominal values used in the analysis; and possible 

local material yielding that is not accounted for in the analysis.
90

(a) Mesh 3 using a single shell unit with the E410 4-node shell elements.

(b) Mesh 3 using two shell units with the E410 4-node shell elements.

(c) Mesh 3 using three shell units with the E410 4-node shell elements.

Figure 27. Representative finite element models of the cylinder with cutouts using different numbers of 

shell units – Mesh 3.
91

(a) Mesh 3 using a single shell unit with the E410 4-node shell elements.

(b) Mesh 3 using a single shell unit with the E480 9-node shell elements.

(c) Mesh 3 using two shell units with the E430 3-node shell elements.

Figure 28. Representative finite element models of the cylinder with cutouts using different shell

elements – Mesh 3 with 4-node, 9-node and 3-node 2-D shell elements.
92

Material properties and shell-wall construction are defined using both the historical STAGS approach

(i.e., STAGS versions prior to GCP) and the current GCP approach. Material modeling for an elastic 

isotropic material using the historical STAGS approach requires data on the I-1 and I-2 records to define

the material properties and the K-1 and K-2 records to define the shell fabrication data. Material modeling

using the current GCP approach requires data on the I-5a and I-6a records to define the material

properties and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the shell fabrication data.

Boundary condition on the displacements are specified using the P-1 and P-2 records. The boundary

conditions along the curved boundary are clamped, while the boundary edges around the cutout are free.

Symmetry boundary conditions are imposed on the straight and curved edges interior to the shell.

A point load is applied at one point on the shell edge equal to one quarter of the total base load P0 because 

of the symmetry conditions. The base load given on the Q-3 record is 0.25 P0 where

2 P0 = 1.2!Et .

Then the load factor on the C-1 record of the S2 input file gives the total load amplitude (i.e., the load

factor PA is related to the total load on the shell). Since the load condition is defined as uniform endshortening loading, partial compatibility constraints on the G-2 records are employed to equate the end

shortening everywhere on the loaded edge to the end shortening at the loading point. The internal force at

that node and in the direction of the loading can be computed and used for plotting as well via the 

XYTRANS utility.

Numerical Results and Discussion

Results for this problem involve the elastic nonlinear collapse response of the shell structure with

localized deformations near the cutouts. The response exhibits buckling at a low value of the applied

loaded followed by a substantial postbuckling response before elastic collapse is detected. Elastic 

collapse is defined here as the first occurrence of a negative root in the tangent stiffness matrix upon

convergence for a given solution step. The nonlinear solutions were obtained using the arc-length control

procedure that automatically adjusts the solution step size and using the full Newton-Raphson approach

(i.e., -20 for NEWT on the D-1 record of the S2 input file).

First a series of linear bifurcation buckling analyses were performed using the single-shell-unit modeling

approach and the various finite element meshes. The finite element mesh is defined by the number of

equally spaced rows and columns of nodes on the shell surface. The irregular mesh option is used to

eliminate those nodes and elements in the cutout region. The results are presented in Table 10 for the 

E410 and E480 shell elements. Models for a given mesh (say Mesh 1) have the same number of nodes but

the model using the E410 element will have four times as many elements as the model using the E480

element – same number of degrees of freedom.
93

Table 10. Effect of Mesh Refinement on the Buckling and Collapse Loads

Mesh NROWS × NCOLS Buckling Load, P/P0 Collapse Load, P/P0

E410 E480 E410 E480

1 7×13 0.0948 0.1739 --- 0.3604

2 13×25 0.1364 0.1489 0.4072 0.4144

3 19×33 0.1372 0.1411 0.3911 0.3748

4 25×49 0.1366 0.1366 0.3845 0.3801

Convergence studies were performed for buckling solutions using the E410 and E480 shell elements.

Results for Mesh 1 are significantly away from the converged value. The E410 models appear to

converge to a value faster than the E480 models for the same number of nodes. It needs to be noted that

the Mesh 4 has four times the number of E410 shell elements as it has E480 shell elements. The lowest

five buckling modes correspond to localized patterns near the cutout straight edges. The sixth mode is

roughly an axisymmetric-like pattern, and the ninth mode is roughly a diamond- or checkerboard-like 

pattern. These modes are illustrated on Figure 29.

Convergence studies were also performed for the elastic nonlinear collapse solutions using the E410 and

E480 shell elements. Results obtained using Mesh 1 and the E410 shell element did not clearly indicate 

“collapse” as defined here (negative root in the tangent stiffness matrix upon convergence). Convergence

to a value of 0.38 P0 occurs at approximately the same rate for both element types.

Results shown in Figures 30 and 31 are for different levels of discretization using the E410 4-node and

E480 9-node shell elements, respectively. Clearly Mesh 1 results the more different results for the E410

models – perhaps due to geometry modeling issues. Results shown in Figure 32 compare the response

predicted using Mesh 3 for three shell elements (E410, E480, and E430). The results obtained using the 

E430 triangular shell elements are somewhat stiffer than the quadrilateral shell elements. The elastic 

collapse load predicted by the E430 model using Mesh 3 is 0.4052 P0.

Contour plots of the axial stress distribution for selected solution steps including after buckling, just prior 

to collapse, and just after collapse are shown in Figure 33. These plots indicate the redistribution of stress

away from just over the cutout, the tensile axial stress near the cutout corners and a compressive axial

stress concentration along the middle of the straight edge of the cutout.
94

(a) Mode 1, P/P0=0.1372 – localized near cutout.

(b) Mode 6, P/P0=0.7937 – axisymmetric-like pattern except near cutouts.

(c) Mode 9, P/P0=0.8113 – nearly diamond pattern except near cutouts.

Figure 29. Contour plots of the out-of-plane displacement component of the buckling mode shapes for 

the single-shell-unit model using Mesh 3 and the E410 shell element.

+1.0

-1.0
95

Figure 30. Effect of mesh refinement using the E410 shell element on the elastic nonlinear collapse 

response.
96

Figure 31. Effect of mesh refinement using the E410 shell element on the elastic nonlinear collapse 

response.
97

Figure 32. Effect of element type using Mesh 3 on the elastic nonlinear collapse response.
98

(a) Step 6, P=0.1049 P0

(b) Step 11, P=0.2825 P0

Figure 33. Contour plots of the axial stress in the outer surface displayed on the deformed geometry at

selected solution steps.

+10 ksi

-20 ksi

0

Axial stress

at the outer

layer
99

(c) Step 13, P=0.3905 P0

(d) Step 15, P=0.3888 P0

Figure 33. Concluded.

+10 ksi

-20 ksi

0

Axial stress

at the outer

layer
100

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Cyl-with-Cutouts

Under this directory are the files for the 2D shell finite element models and analyses described in this

section.

Single Shell Unit Input Files

The following text files give the input for the cylinder with cutouts using the E410 4-node shell element

with an 19×33 mesh of nodes on the shell surface. These files are in the 2D/ subdirectory. The S2 input

file contains input sufficient to perform the buckling computations and the elastic nonlinear collapse 

analysis. While all records of the S2 input file are read, only those associated with the first analysis type 

are active. Similarly all the records of the STAPL input file are read even though only the number of

plots specified on the PL-2 record will be drawn.

cutout1.inp (for S1 processor)

2D circular cylinder with two rectangular cutouts $A-1

C

C Cylinder with cutouts 180-degrees apart at cylinder

C mid-length; clamped at the ends and loaded by applied

C end-shortening. Elastic postbuckling response.

C R=6.06 in., L=9.0 in. (total), t=0.014 in.

C R/t=433, L/R=1.5

C

C Loading is a point axial load plus constraints for uniform u

C Px = 0.25*Po = 0.25 * (1.2*pi*E*t^^2) = 1847.256 pounds

C Critical eigenvalue is 0.137

C Linear Buckling Load = 1012.3 lbs. = 0.137 * Po

C Collapse Load from STAGS (Mesh 4, E410) = 0.3845 Po

C Collapse Load from Test [1] = 2200 lbs = 0.2977 * Po

C

C Perfect geometry assumed for linear buckling analysis

C and for the elastic collapse analysis. Use of initial

C geometric imperfections would influence the collapse load

C prediction.

C

C References:

C 1. Almroth, B. O. and Holmes, A. M. C., "Buckling of Shells with

C Cutouts, Experiment and Analysis," International Journal

C of Solids and Structures, Vol. 8, No. 8, 1972, pp. 1057-1071.

C 2. Hartung, R. F. and Ball, R. E., "A Comparison of Several

C Computer Solutions to Three Structural Shell Analysis

C Problems," AFFDL TR-73-15, 1973

C 3. Almroth, B. O. and Brogan, F. A., "Computational Efficiency

C of Shell Elements," in Nonlinear Finite Element Analysis

C of Plates and Shells, Hughes, Pifko, & Jay (editors),

C ASME AMD Vol. 48, 1981, pp. 147-165.

C 4. Knight, et al., "Large-Scale Structural Analysis: The

C Structural Analyst, The CSM Testbed, and The NAS System,"

C NASA TM-100643, March 1989.

C

0 0 0 0 0 3 0 $b-1

1 20.0 / 2 -60.0 / 3 -90.0 $b-1b model rotations

1 0 0 0 1 0 0 $b-2

1 0 1 0 0 1 $b-3

C

C FE Mesh Study

C Nrcols x Ncols
101

C

C7 13 $F-1 Mesh 1

C13 25 $F-1 Mesh 2

19 33 $F-1 Mesh 3

C25 49 $F-1 Mesh 4

C37 65 $F-1 Mesh 5

C

1 1 1 1 1 1 0 1 $G-2 set end shortening to be uniform

C

C Material Record using Historical Approach

C

1 0 $I-1 material table

10.0E+6 0.3 0.0 .1 $i-2 E, nu, G=E/2/(1+nu), rho (for volume check)

C

C GCP Input

C

ISOELASTIC_MATERIAL 1 1 1 $i-5

10.0E+6, $i-6a Young's modulus, psi

0.3, $i-6a Poisson's ratio

2.59E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Shell wall fabrications

C

SHELL_FABRICATION 1 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym

1 $I-21a matid

0.014 $i-21c thickness, inches

0.0 $i-21d angle

C

END $I-5a end GCP input

C

C Wall Record using Historical Approach

C

1 1 1 0 $k-1 thickness, inches

1 0.014 0.0 $k-2

C

C Shell Unit Definition - using 2D shell elements

C

5 0 0 0 0 0 0 $m-1 cylindrical shell geometry

0.0 4.50 0.0 90.0 6.06 $m-2 x1, x4, y1, y2, R

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

410 0 0 1 $n-1 element options

C

C Irregular mesh option for cutout boundaries

C (only works for quadrilateral shell elements)

C

C5 7 9 13 $N-8 Mesh 1 values

C9 13 19 25 $N-8 Mesh 2 values

13 19 25 33 $N-8 Mesh 3 values

C17 25 37 49 $N-8 Mesh 4 values

C25 37 49 65 $N-8 Mesh 5 values

C

C Boundary conditions

C

0 4 4 4 $p-1 clamped-sym-sym-sym

100 000 $p-2 end shortening on clamped end

C

C Loading - point load at center

C P_base = 0.25 * Po = 0.25 * (1.2 pi E t^2)

C then the load factor is related to P/Po

C

1 0 $q-1 load summary

1 1 0 $q-2
102

1847.256 1 1 1 1 0 $Q-3 imposed axial load at one node and then G-1

C0.0 -1 6 0 0 0 $Q-3 imposed RW=0 everywhere for E480 and E330

0 0 0 0 0 0 1 0 0 $r-1 Output selection

1 0 $r-2 selected displacement output

cutout1.bin (for S2 processor)

Cylinder with two rectangular cutouts $A-1

C

C Linear buckling analysis

C

1 1 0 0 0 0 0 -1 $b-1

1.0 0.0 1.0 $c-1

1000 1.0e-4 0 $d-2

10 .137 $d-3 Number of modes

C

C Nonlinear static solution control

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

0.02 0.02 1.0 $C-1 LOAD MULTIPLIERS

0 3000 5 -20 0 1.0e-4 1.0 $d-1 strategy parameters

0 0 0 $et-1

cutout1.pin (for STAPL processor)

Cylinder with two rectangular cutouts

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C plot axial stress contours

2 0 7 6 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -20000.0 10000.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 7 11 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -20000.0 10000.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 7 13 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -20000.0 10000.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 7 15 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -20000.0 10000.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

C plot stress resultant Nx at different steps

2 0 5 6 0 2 1 1 $PL-3KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -150.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 5 11 0 2 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -150.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 5 13 0 2 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -150.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 5 15 0 2 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -150.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

C plot buckling modes

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 6 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 9 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP
103

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 5 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 6 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 7 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 8 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 9 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 4 0 10 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 1 10 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

2 0 1 20 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 -60.0 / 3 -90.0

cutout1.pxy (for XYTRANS processor)

This input is generated and saved during the first execution of XYTRANS (so called journal file). Once

created it can be used over and over again to extract the same information from a STAGS run.

P $ (P)lotps or (S)pread_Sheet output

cutout1 $ STAGS solution 'Case Name'

F $ (F)ull or (C)ondensed Model

Y $ (Y)es-(N)o: setup data for another plot

5 $ x-axis variable = choice (1 to 15)

0 $ node no. (0 = ask for Unit,Row,Col)

1 19 25 $ (U)nit, (R)ow, (C)ol - Node No. = 619

3 $ comp no., dis,vel,acc (1-6) = u,v,w,ru,rv,rw

S $ (G)lobal or (S)hell ref surface

N $ (Y)es-(N)o: specify x-variable scale factor

2 $ y-axis variable = choice (1 to 15)

N $ (Y)es-(N)o: specify y-variable scale factor

N $ (Y)es-(N)o: specify subrange of loadsteps

Y $ (Y)es-(N)o: plotted points start at origin

N $ (Y)es-(N)o: setup data for another plot
104

Two-Shell-Unit Model Input Files

The following text files give the input for the cylinder with cutouts using the E410 4-node shell element

with a 19×33 mesh of nodes on the shell surface. The input files for S2 and STAPL are the same as those 

given for the single-shell-unit model.

cutout2.inp (for S1 processor)

2D circular cylinder with two rectangular cutouts - 2 shell units $A-1

C

C Mesh 3 (19 x 33) only

C

C Cylinder with cutouts 180-degrees apart at cylinder

C mid-length; clamped at the ends and loaded by applied

C end-shortening. Elastic postbuckling response.

C Only a 1/8 symmetric model is considered.

C

C R=6.06 in., L=9.0 in. (total), t=0.014 in.

C R/t=433, L/R=1.5

C

C Loading is a point axial load plus constraints for uniform u

C Px = 0.25*Po = 0.25 * (1.2*pi*E*t^^2) = 1847.256 pounds

C Critical eigenvalue is 0.137

C Linear Buckling Load = 1012.3 lbs. = 0.137 * Po

C Collapse Load from STAGS (Mesh 4, E410) = 0.3845 * Po

C Collapse load from test [1] = 2200 lbs = 0.2977 * Po

C

C Perfect geometry assumed for linear buckling analysis

C and for the elastic collapse analysis. Use of initial

C geometric imperfections would influence the collapse load

C prediction.

C

C References:

C 1. Almroth, B. O. and Holmes, A. M. C., "Buckling of Shells with

C Cutouts, Experiment and Analysis," International Journal

C of Solids and Structures, Vol. 8, No. 8, 1972, pp. 1057-1071.

C 2. Hartung, R. F. and Ball, R. E., "A Comparison of Several

C Computer Solutions to Three Structural Shell Analysis

C Problems," AFFDL TR-73-15, 1973

C 3. Almroth, B. O. and Brogan, F. A., "Computational Efficiency

C of Shell Elements," in Nonlinear Finite Element Analysis

C of Plates and Shells, Hughes, Pifko, & Jay (editors),

C ASME AMD Vol. 48, 1981, pp. 147-165.

C 4. Knight, et al., "Large-Scale Structural Analysis: The

C Structural Analyst, The CSM Testbed, and The NAS System,"

C NASA TM-100643, March 1989.

C

0 0 0 0 0 3 0 $b-1

1 20.0 / 2 -60.0 / 3 -90.0 $b-1b model rotations

2 0 0 0 3 0 0 $b-2

1 0 1 0 0 1 $b-3

C FE mesh Nrcols x Ncols

19 25 13 9 $F-1 Resulting mesh is 19 x 33

1 1 1 1 1 1 0 1 $G-2 set end shortening to be uniform

1 1 1 1 2 1 0 1 $G-2 set end shortening to be uniform

1 0 25 0 2 0 1 0 1 13 1 1 13 1 $G-2

C

C Material Record using Historical Approach

C

1 0 $I-1 material table

10.0E+6 0.3 0.0 .1 $i-2 E, nu, G=E/2/(1+nu), rho (for volume check)

C

C GCP Input

C
105

ISOELASTIC_MATERIAL 1 1 1 $i-5

10.0E+6, $i-6a Young's modulus, psi

0.3, $i-6a Poisson's ratio

2.59E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Shell wall fabrications

C

SHELL_FABRICATION 1 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym

1 $I-21a matid

0.014 $i-21c thickness, inches

0.0 $i-21d angle

C

END $I-5a end GCP input

C

C Wall Record using Historical Approach

C

1 1 1 0 $k-1 thickness, inches

1 0.014 0.0 $k-2

C

C Shell Unit Definition - using 2D shell elements

C

C ============================

C Shell unit 1 (top left side)

C ============================

5 0 0 0 0 0 0 $m-1 cylindrical shell geometry

0.0 4.50 0.0 67.5 6.06 $m-2 x1, x4, y1, y2, R

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

410 0 0 0 $n-1 element options

C

C Boundary conditions

C

0 3 4 4 $p-1 clamped-juncture-juncture-sym

100 000 $p-2 end shortening on clamped end

C

C Loading - point load at center

C

1 0 $q-1 load summary

1 1 0 $q-2

1847.256 1 1 1 1 0 $Q-3 imposed axial load at one node and then G-1

C0.0 -1 6 0 0 0 $Q-3 RW=0 everywhere for E480 & E430

0 0 0 0 0 0 1 0 0 $r-1 Output selection

1 0 $r-2 selected displacement output

C =========================================

C Shell unit 2 (top right side over cutout)

C =========================================

5 0 0 0 0 0 0 $m-1 cylindrical shell geometry

0.0 3.00 67.5 90.0 6.06 $m-2 x1, x4, y1, y2, R

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

410 0 0 0 $n-1 element options

C

C Boundary conditions

C

0 4 3 3 $p-1 clamped-sym-free-juncture

100 000 $p-2 end shortening on clamped end

C

0 0 $q-1 No loads

C1 0 $q-1 Zero out drilling freedoms for E480 & E430

C1 1 0 $q-2

C0.0 -1 6 0 0 0 $Q-3 RW=0 everywhere

0 0 0 0 0 0 1 0 0 $r-1 Output selection

1 0 $r-2 selected displacement output
106

Three-Shell-Unit Model Input Files

The following text files give the input for the cylinder with cutouts using the E430 3-node shell element

with a 19×33 mesh of nodes on the shell surface. Notice in this case that the drilling freedoms are 

suppressed everywhere in the finite element model (i.e., requires Q-3 records for each shell unit). The

input files for S2 and STAPL are the same as those given for the single-shell-unit model.

cutout3.inp (for S1 processor)

2D circular cylinder with two rectangular cutouts - 3 shell units $A-1

C

C Mesh 3 (19 x 33) only

C

C Cylinder with cutouts 180-degrees apart at cylinder

C mid-length; clamped at the ends and loaded by applied

C end-shortening. Elastic postbuckling response.

C Only a 1/8 symmetric model is considered.

C

C R=6.06 in., L=9.0 in. (total), t=0.014 in.

C R/t=433, L/R=1.5

C

C Loading is a point axial load plus constraints for uniform u

C Px = 0.25*Po = 0.25 * (1.2*pi*E*t^^2) = 1847.256 pounds

C Critical eigenvalue is 0.137

C Linear Buckling Load = 1012.3 lbs. = 0.137 * Po

C Collapse Load from STAGS (Mesh 4, E410) = 0.3845 * Po

C Collapse Load from Test [1] = 2200 lbs = 0.2977 * Po

C

C Perfect geometry assumed for linear buckling analysis

C and for the elastic collapse analysis. Use of initial

C geometric imperfections would influence the collapse load

C prediction.

C

C References:

C 1. Almroth, B. O. and Holmes, A. M. C., "Buckling of Shells with

C Cutouts, Experiment and Analysis," International Journal

C of Solids and Structures, Vol. 8, No. 8, 1972, pp. 1057-1071.

C 2. Hartung, R. F. and Ball, R. E., "A Comparison of Several

C Computer Solutions to Three Structural Shell Analysis

C Problems," AFFDL TR-73-15, 1973

C 3. Almroth, B. O. and Brogan, F. A., "Computational Efficiency

C of Shell Elements," in Nonlinear Finite Element Analysis

C of Plates and Shells, Hughes, Pifko, & Jay (editors),

C ASME AMD Vol. 48, 1981, pp. 147-165.

C 4. Knight, et al., "Large-Scale Structural Analysis: The

C Structural Analyst, The CSM Testbed, and The NAS System,"

C NASA TM-100643, March 1989.

C

0 0 0 0 0 3 0 $b-1

1 20.0 / 2 -60.0 / 3 -90.0 $b-1b model rotations

3 0 0 2 2 0 0 $b-2

1 0 1 0 0 1 $b-3

C FE mesh Nrcols x Ncols

13 25 13 9 7 25 $F-1 Resulting mesh is 19 x 33

1 2 2 4 $g-1 Shell unit connectivity

1 3 3 1 $g-1 Shell unit connectivity

1 1 1 1 1 1 0 1 $G-2 set end shortening to be uniform

1 1 1 1 2 1 0 1 $G-2 set end shortening to be uniform

C

C Material Record using Historical Approach

C

1 0 $I-1 material table
107

10.0E+6 0.3 0.0 .1 $i-2 E, nu, G=E/2/(1+nu), rho (for volume check)

C

C GCP Input

C

ISOELASTIC_MATERIAL 1 1 1 $i-5

10.0E+6, $i-6a Young's modulus, psi

0.3, $i-6a Poisson's ratio

2.59E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Shell wall fabrications

C

SHELL_FABRICATION 1 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym

1 $I-21a matid

0.014 $i-21c thickness, inches

0.0 $i-21d angle

C

END $I-5a end GCP input

C

C Wall Record using Historical Approach

C

1 1 1 0 $k-1 thickness, inches

1 0.014 0.0 $k-2

C

C Shell Unit Definition - using 2D shell elements

C

C ============================

C Shell unit 1 (top left side)

C ============================

5 0 0 0 0 0 0 $m-1 cylindrical shell geometry

0.0 3.00 0.0 67.5 6.06 $m-2 x1, x4, y1, y2, R

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

430 0 0 0 $n-1 element options

C

C Boundary conditions

C

0 6 6 4 $p-1 clamped-juncture-juncture-sym

100 000 $p-2 end shortening on clamped end

C

C Loading - point load at center

C

1 0 $q-1 load summary

1 2 0 $q-2

1847.256 1 1 1 1 0 $Q-3 imposed axial load at one node and then G-1

0.0 -1 6 0 0 0 $q-3 RW=0 everywhere

0 0 0 0 0 0 1 0 0 $r-1 Output selection

1 0 $r-2 selected displacement output

C =========================================

C Shell unit 2 (top right side over cutout)

C =========================================

5 0 0 0 0 0 0 $m-1 cylindrical shell geometry

0.0 3.00 67.5 90.0 6.06 $m-2 x1, x4, y1, y2, R

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

430 0 0 0 $n-1 element options

C

C Boundary conditions

C

0 4 3 6 $p-1 clamped-sym-free-juncture

100 000 $p-2 end shortening on clamped end

C

1 0 $q-1 Suppress drilling freedoms

1 1 $q-2

0.0 -1 6 0 0 0 $q-3 RW=0 everywhere
108

0 0 0 0 0 0 1 0 0 $r-1 Output selection

1 0 $r-2 selected displacement output

C =========================================

C Shell unit 3 (bottom side left of cutout)

C =========================================

5 0 0 0 0 0 0 $m-1 cylindrical shell geometry

3.0 4.50 0.0 67.5 6.06 $m-2 x1, x4, y1, y2, R

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

430 0 0 0 $n-1 element options

C

C Boundary conditions

C

6 3 4 4 $p-1 juncture-free-sym-sym

C

C

1 0 $q-1 Suppress drilling freedoms

1 1 $q-2

0.0 -1 6 0 0 0 $q-3 RW=0 everywhere

0 0 0 0 0 0 0 0 0 $r-1 Output selection

Problem References

Almroth, B. O. and Holmes, A. M. C., “Buckling of Shells with Cutouts, Experiment and Analysis,” 

International Journal of Solids and Structures, Vol. 8, 1972, pp. 1057-1071.

Hartung, R. F. and Ball R. E., A Comparison of Several Computer Solutions to Three Structural Shell

Analysis Problems, AFFDL Report No. AFFDL-TR-73-15, April 1973.

Almroth, B. O., Meller, E., and Brogan, F. A., “Computer Solutions for Static and Dynamic Buckling of 

Shells,” in Buckling of Structures, B. Budiansky (editor), proceedings of the IUTAM Symposium, June 

17-21, 1974, Springer-Verlag, Berlin, 1976, pp. 52-66.

Almroth, B. O. and Brogan, F. A., “Computational Efficiency of Shell Elements,” in Nonlinear Finite 

Element Analysis of Plates and Shells, T. J. R. Hughes, A. Pifko, and A. Jay (editors), ASME AMD-Vol.

48, 1981, pp. 147-165.

Knight, N. F., Jr., McCleary, S. L., Macy, S. C., and Aminpour, M. A., Large-Scale Structural Analysis: 

The Structural Analyst, The CSM Testbed, and The NAS System, NASA TM-100643, March 1989.

Knight, N. F., Jr., Macy, S. C., and McCleary, S. L., “Assessment of Structural Analysis Technology for

Static Collapse of Elastic Cylindrical Shells,” Finite Elements in Analysis and Design, Vol. 18, No. 4,

January 1995, pp. 403-431.

Hurlbut, B. J., Stanley, G. M., and Kang, D. S., The Computational Structural Mechanics (CSM) Testbed

Applications Manual, Lockheed Contract Report No. LMSC-F333007, May 1989.

Rankin, C. C., Brogan, F. A., Loden, W., and Cabiness, H., Structural Analysis of General Shells –

STAGS User Manual, Version 4.0, Lockheed Martin Advanced Technology Center, Palo Alto, CA, June

2000.
109

Scordelis-Lo Barrel Roof Problem

Background

The Scordelis-Lo barrel roof (or vault) is a singly curved shell structure shown in Figure 34 loaded by a 

gravity load or uniform dead load (UDL, loading by its own weight). This cylindrical shell is supported

along the curved ends by rigid diaphragms (v=w=0) while the straight edges are free. This problem is a 

common linear static shell analysis (e.g., Forsberg, 1971; Parisch, 1979; Thomas and Sobel, 1981;

MacNeal and Harder, 1985; Belytschko and Liu, 1986; Zienkiewicz and Taylor, 1991; Phaal and

Calladine, 1992; Rengarajan et al., 1995). This problem tests an element’s ability to represent membrane 

states. Most of the strain energy is stored in the stretching mode with little inextensional flexural

response. It is one of the MacNeal-Harder standard test problems and one of the Belytschko-Liu shell

obstacle course problems.

Figure 34. Scordelis-Lo barrel roof problem: geometry and material properties.

Modeling and Analysis Process

Two separate STAGS finite element models are considered in this test case problem: shell elements and

solid elements. A summary of each model includes:

E = 3000 ksi = 4.32×108 lb/ft2

ν = 0.0

R = 300.0 in. = 25.0 ft.

L = 300.0 in. = 25.0 ft.

h = 3.0 in. = 0.25 ft

θ = 40.0°

UDL = 90 lb/ft2 = ρgh

Free

Edg

e

2L

Supporte

d

by Rigid

Diaphrag

m

R

B

A

y

x

z
110

2-D shell models – Model the shell with plate elements (x-y plane) in a single shell unit as shown in

Figure 35.

3-D solid models – Model shell with solid elements in a single shell unit using one and two solid

elements through the thickness of the shell as shown in Figure 36.

The STAGS model is generated using a single shell unit with the cylindrical shell surface geometry

(ISHELL=5) using the mid-surface as the shell reference surface. Material properties and membrane 

construction are defined using both the historical STAGS approach and the current GCP approach. Mesh

discretization studies include different levels of mesh refinement and different element types. Mesh

refinement is readily performed by changing the number of rows and columns of nodes in each direction

on the F-1 record. Element type is selected using the N-1 record (KELT). Multiple solid elements

through the thickness are specified using the NLAYS and NFABS parameters on the M-1 record in

combination with a set of NFABS M-5 records.

Figure 35. Shell finite element models having 11 nodes per edge.

(a) Mesh using 3-node triangular elements

(b) Mesh using 4-node quadrilateral elements

(c) Mesh using 9-node quadrilateral elements

Rigid

Diaphragm

Symmetry

Symmetry

Free Edge
111

Figure 36. Solid element models having 11 nodes per edge.

(a) Mesh using 8-node hexahedral elements – NEZ=2

(b) Mesh using 27-node hexahedral elements – NEZ=1)
112

Material properties and laminate construction are defined using both the historical STAGS approach (i.e.,

STAGS versions prior to GCP) and the current GCP approach. Material modeling for an elastic 

orthotropic material using the historical STAGS approach requires data on the I-1 and I-2 records to

define the material properties and the K-1 and K-2 records to define the laminate fabrication data.

Material modeling using the current GCP approach requires data on the I-5a and I-6a records to define the 

material properties and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the shell fabrication.

In addition, records I-5a, I-22a, and I-22b are used to define the solid fabrication. As a basic check on the

finite element model, the total weight of the structure is computed and printed in the initial portion of the 

S2 output file. The total weight of one quarter of the shell is 12500π pounds.

Boundary condition on the displacements could be specified using the P-1 and P-2 records for the shell

models as indicated in the input file. However, for compatibility with the solid element models, the 

boundary conditions are imposed using specified zero displacements through the Q-records for both shell

and solid models. The boundary conditions along the curved boundary are those of a rigid diaphragm

with no circumferential or transverse displacements (v=w=0), and the boundary conditions along the 

straight boundary are free. Symmetry boundary conditions are imposed on the remaining straight and

curved interior edges. The uniform dead load (UDL) is applied as an inertial loading (B-6 records) acting

parallel to the negative z-coordinate direction. Essentially the weight density of the shell material

generates the distributed load. The weight density is computed as the UDL divided by the shell thickness

or 360 lbs/in.

3

. The inertial loading is due to the shell mass density and the acceleration due to gravity.

The default gravitational constant g in STAGS is 386.1 in./sec.

2 (32.175 ft/ sec.2

) which may be changed

using the B-4 record in the S1 input file. For this test case, a value of 386.4 in./sec.

2 (32.2 ft/ sec.2

) is

used.

Numerical Results and Discussion

Numerical results are presented to indicate the effect of uniform mesh refinement. The vertical deflection

at point B (on the free edge at panel midlength) is commonly used as the metric to judge performance.

Since STAGS prints the displacement solution in the coordinate system of the shell unit (cylindrical

coordinates for this case), the displacements at the node points need to be transformed to the global

rectangular coordinate system using the following relation:

sin ! cos ! local

B

local

B

global wB

= v " w

where θ is measured from the crown of the cylindrical panel, w is the radial displacement and v is the

tangential displacement at point B on the shell. Alternatively XYTRANS may be used to extract the

displacement in global coordinates. Theoretical solutions are given by Cowper et al. (1970) for shallow

shell theory (3.703 in. or 0.3086 ft) and by Forsberg (1970) and Thomas and Sobel (1981) for deep shell

theory (3.592 in. or 0.2994 ft). Parisch (1979) quotes a value of 2.610 in. or 0.3008 ft. for a deep shell

solution. MacNeal and Harder (1985) and Belytschko and Liu (1986) normalize their solutions using a 

value of 3.6288 in. or 0.3024 ft. This value has become the de facto standard value for comparison

purposes. The computed values obtained from STAGS are normalized by this latter value in order to be

compared with other published solutions.

Table 11 summarizes the 2D shell analysis results obtained using different STAGS shell elements and

different levels of uniform mesh refinement. Element aspect ratio is unity for all meshes considered.

Element E320 is s 3-node classical triangular shell element in STAGS; drilling degrees of freedom are not

present and hence suppressed. Element E330 is the 3-node MIN3 shear-deformable shell element;

drilling degrees of freedoms are not present and hence suppressed. Element E410 is the 4-node classical

shell element in STAGS – workhorse shell element; drilling degrees of freedom are present and free.

Element E480 is the 9-node ANS shear-deformable shell element; drilling degrees of freedom are not

present and hence suppressed. The mesh is defined by the number of nodes along each edge of the finite 
113

element model so that each finite element model has essentially the same number nodes and degrees of 

freedom even though the number of elements is different.

Table 12 summarizes the 3D analysis results obtained using different STAGS solid elements and different

levels of uniform mesh refinement. The same planar mesh discretizations as considered for the shell

elements are used herein in combination with either one (NEZ=1) or two (NEZ=2) solid elements through

the thickness of the structure. For the case of one solid element through the thickness, the through-thethickness element aspect ratio varies from 50 for the coarsest mesh to 10 for the most refined. For the case

of two solid elements through the thickness, the through-the-thickness element aspect ratio varies from 25

for the coarsest mesh to 5 for the most refined. Element E881 is an 8-node ANS-based solid element.

Element E883 is a 27-node ANS-based solid element. Element E885 is a 20-node displacement based

solid element. The value of the normalized deflection reported in Table 12 for the solid element cases

represents the value from the inner surface at Point B – only a slight variation in this value occurs through

the thickness.

Table 11. Convergence behavior of the STAGS shell elements

for the Scordelis-Lo barrel roof problem.

Normalized free edge vertical deflection at panel midlength (Point B)

Mesh E320 E330 E410 E480

3×3 0.9267 1.0235 1.3776 0.7705

5×5 0.7236 0.7322 1.0476 0.9544

7×7 0.8220 0.8273 1.0143 0.9852

9×9 0.8840 0.8893 1.0047 0.9914

11×11 0.9198 0.9255 1.0006 0.9933

Table 12. Convergence behavior of the STAGS solid elements

for the Scordelis-Lo barrel roof problem.

Normalized free edge vertical deflection at panel midlength (Point B)

E881 E883 E885

Mesh NEZ=1 NEZ=2 NEZ=1 NEZ=2 NEZ=1 NEZ=2

3×3×NEZ 1.3032 1.3046 1.0020 1.0021 0.8778 0.8784

5×5×NEZ 1.0271 1.0272 0.9435 0.9436 0.9628 0.9629

7×7×NEZ 1.0047 1.0047 0.9774 0.9775 1.0087 1.0088

9×9×NEZ 0.9965 0.9965 0.9837 0.9838 1.0014 1.0015

11×11×NEZ 0.9928 0.9928 0.9855 0.9856 0.9968 0.9969
114

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Roof

Typical 2D Shell Model Input Files

The following text files give the input for the 2D shell model using the E410 4-node shell element in

STAGS with 11 nodes per edge.

roof2d.inp (for S1 processor)

2D Scordelis-Lo barrel roof under self weight $A-1

C

C 2D shell model: Reference solution for vertical deflection

C at free edge at mid-length = 3.6288" = 0.3024 ft.

C vertical deflection = v*sin(theta) - w*cos(theta)

C

1 0 0 0 0 3 0 $b-1

1 -90.0 $b-1b rotation about x

2 0.0 $b-1b rotation about y

3 -110.0 $b-1b rotation about z

1 0 0 0 0 0 0 1 $b-2

1 0 1 0 0 1 $b-3

386.4 $b-4 gravitational constant

1 1 0 0 0 $b-6 inertial load set

0.0 0.0 386.4 $b-6a gravity loading in z-direction

11 11 $f-1 grid (nrows by ncols)

C

C Material Record using Historical Approach

C

1 0 $I-1 material table

3000000. 0.0 0.0 .208333 $i-2 E, nu, G=E/2/(1+nu), rho (90 lb/ft^2)

C

C GCP Input

C

ISOELASTIC_MATERIAL 1 1 1 $i-5

3000000.0, $i-6a Young's modulus, psi

0.0, $i-6a Poisson's ratio

5.3916494E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Solid fabrications - element thicknesses NOT total wall thickness!

C

SOLID_FABRICATION 1 1 0 0 $i-5a for one element through thickness

3.0 $i-22a element thickness

SOLID_FABRICATION 2 1 0 0 $i-5a for two elements through thickness

1.50 $i-22a element thickness

SOLID_FABRICATION 3 1 0 0 $i-5a for four elements through thickness

0.75 $i-22a element thickness

C

C Shell wall fabrications

C

SHELL_FABRICATION 1 1 0 1 0 $i-5a fabid, nlayer, ipts, ishr, isym

1 $I-21a matid

3.0 $i-21c thickness - thick

0.0 $i-21d angle

1.0 1.0 $i-21e shear factors

C

END $I-5a end GCP input

C

C Wall Record using STAGS Historical Approach

C
115

1 1 1 0 $k-1 thick shell

1 3.0 0.0 $k-2

C

C Shell Unit Definition - using 2D shell elements

C

5 0 0 0 0 0 $m-1 cylindrical shell geometry

0.0 300.0 0.0 40.0 300.0 $m-2 x1, x4, y1, y2, R

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

330 11*0 $n-1 element options

C

C Boundary conditions - specified using the Q-records

C

3 3 3 3 $p-1 completely free - see Q-records

C 4 3 0 4 $p-1 sym-free- rigid diaphragm-sym

C 100 000 $p-2 v=w=0 on curved boundary (rigid diaphragm)

C

C Loading - uniform dead load using inertial loading (B-6 records)

C

1 0 $q-1 load summary

1 8 $q-2 load set summary

C

C Impose symmetry on edge 1 (u=rv=rw=0); all layers

C

0.0 -1 1 1 1 0 11 0 0 1 1 $q-3 u=0 on edge 1, layer 1

0.0 -1 5 1 1 0 11 0 0 1 1 $q-3 rv=0 on edge 1, layer 1

0.0 -1 6 1 1 0 11 0 0 1 1 $q-3 rw=0 on edge 1, layer 1

C

C Impose symmetry on edge 4 (v=ru=rw=0); all layers

C

0.0 -1 2 1 1 0 11 0 1 0 1 $q-3 v=0 on edge 4, layer 1

0.0 -1 4 1 1 0 11 0 1 0 1 $q-3 ru=0 on edge 4, layer 1

0.0 -1 6 1 1 0 11 0 1 0 1 $q-3 rw=0 on edge 4, layer 1

C

C Impose condition v=w=0 on edge 3; all layers

C

0.0 -1 2 11 1 0 11 0 0 1 1 $q-3 v=0 on edge 1, layer 1

0.0 -1 3 11 1 0 11 0 0 1 1 $q-3 w=0 on edge 1, layer 1

C

C Zero out all drilling DOF for elements w/o them (E320, E330, E480)

C

C 0.0 -1 6 0 0 0 0 0 0 0 0 $q-3 rw=0 everywhere

C

1 0 0 0 0 0 1 0 1 $r-1 Output selection

1 0 $r-2 selected displacement output

roof2d.bin (for S2 processor)

Scordelis-Lo barrel roof problem $A-1

0 1 5*0 -1 $B-1 ANALYSIS CONTROL

1.0 1.0 1.0 $C-1 LOAD MULTIPLIERS

roof2d.pin (for STAPL processor)

Scordelis-Lo 2D roof problem

1 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 1 0 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -90.0 / 2 0.0 / 3 -110.0 $PL-6 rotations
116

Typical 3D Solid Model Input Files

The following text files give the input for the 3D shell model using the E881 8-node solid element in

STAGS with 11 nodes per edge and two elements through the thickness or three planes of nodes

(NEZ=2).

roof3d.inp (for S1 processor)

3D Scordelis-Lo barrel roof under self weight $A-1

C

C 3D solid model: Reference solution for vertical deflection

C at free edge at mid-length = 3.6288" = 0.3024 ft.

C vertical deflection = v*sin(theta) - w*cos(theta)

C

1 0 0 0 0 3 0 $b-1

1 -90.0 $b-1b rotation about x

2 0.0 $b-1b rotation about y

3 -110.0 $b-1b rotation about z

1 0 0 0 0 0 0 1 $b-2

1 0 1 0 0 1 $b-3

386.4 $b-4 gravitational constant

1 1 0 0 0 $b-6 inertial load set

0.0 0.0 386.4 $b-6a gravity loading in z-direction

11 11 $f-1 grid (nrows by ncols)

C

C Material Record using Historical Approach

C

1 0 $I-1 material table

3000000. 0.0 0.0 .208333 $i-2 E, nu, G=E/2/(1+nu), rho (90 lb/ft^2)

C

C GCP Input

C

ISOELASTIC_MATERIAL 1 1 1 $i-5

3000000.0, $i-6a Young's modulus, psi

0.0, $i-6a Poisson's ratio

5.3916494E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Solid fabrications - element thicknesses NOT total wall thickness!

C

SOLID_FABRICATION 1 1 0 0 $i-5a for one element through thickness

3.0 $i-22a element thickness

SOLID_FABRICATION 2 1 0 0 $i-5a for two elements through thickness

1.50 $i-22a element thickness

SOLID_FABRICATION 3 1 0 0 $i-5a for four elements through thickness

0.75 $i-22a element thickness

C

C Shell wall fabrications

C

SHELL_FABRICATION 1 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym

1 $I-21a matid

3.0 $i-21c thickness

0.0 $i-21d angle

C

END $I-5a end GCP input

C

C Wall Record using STAGS Historical Approach

C

1 1 1 0 $k-1 thick shell

1 3.0 0.0 $k-2

C

C Shell Unit Definition - using 3D shell elements

C 2 881-solid elements of the same material through the thickness

C this results in three layers of nodes
117

C

5 0 0 0 2 1 $m-1 cylindrical shell geometry, 2 layers of elements

0.0 300.0 0.0 40.0 300.0 $m-2 x1, x4, y1, y2, R

-2 0 0.0 0.0 0 0 $m-5 shell wall selection

881 11*0 $n-1 element options

C

C Boundary conditions - specified using the Q-records

C

3 3 3 3 $p-1 completely free - see Q-records

C

C Loading - uniform dead load using inertial loading (B-6 records)

C

1 0 $q-1 load summary

1 12 $q-2 load set summary

C

C Impose symmetry on edge 1 (u=0); all layers

C

0.0 -1 1 1 1 0 11 0 0 1 1 $q-3 u=0 on edge 1, layer 1

0.0 -1 1 1 1 0 11 0 0 1 2 $q-3 u=0 on edge 1, layer 2

0.0 -1 1 1 1 0 11 0 0 1 3 $q-3 u=0 on edge 1, layer 3

C

C Impose symmetry on edge 4 (v=0); all layers

C

0.0 -1 2 1 1 0 11 0 1 0 1 $q-3 v=0 on edge 4, layer 1

0.0 -1 2 1 1 0 11 0 1 0 2 $q-3 v=0 on edge 4, layer 2

0.0 -1 2 1 1 0 11 0 1 0 3 $q-3 v=0 on edge 4, layer 3

C

C Impose condition v=w=0 on edge 3; all layers

C

0.0 -1 2 11 1 0 11 0 0 1 1 $q-3 v=0 on edge 3, layer 1

0.0 -1 2 11 1 0 11 0 0 1 2 $q-3 v=0 on edge 3, layer 2

0.0 -1 2 11 1 0 11 0 0 1 3 $q-3 v=0 on edge 3, layer 3

0.0 -1 3 11 1 0 11 0 0 1 1 $q-3 w=0 on edge 3, layer 1

0.0 -1 3 11 1 0 11 0 0 1 2 $q-3 w=0 on edge 3, layer 2

0.0 -1 3 11 1 0 11 0 0 1 3 $q-3 w=0 on edge 3, layer 3

C

1 0 0 0 0 0 1 0 1 $r-1 Output selection

1 0 $r-2 selected displacement output

roof3d.bin (for S2 processor)

Scordelis-Lo barrel roof problem $A-1

0 1 5*0 -1 $B-1 ANALYSIS CONTROL

1.0 1.0 1.0 $C-1 LOAD MULTIPLIERS
118

Problem References

Scordelis, A. C. and Lo, K. S., “Computer Analysis of Cylindrical Shells,” Journal of the American

Concrete Institute, Vol. 61, No. 5, May 1964, pp. 539-561.

Cowper, G. R., Lindberg, G. M., and Olson, M.D., “A Shallow Shell Finite Element of Triangular 

Shape,” International Journal of Solids and Structures, Vol. 6, No. 8, August 1970, pp. 1133-1156.

Forsberg, Kevin, “An Evaluation of Finite Difference and Finite Element Techniques for Analysis of 

General Shells,” in High Speed Computing of Elastic Structures, B. Fraeijis de Veubeke (editor), IUTAM,

University of Liège, 1971, pp.837-859.

Parisch, H., “A Critical Survey of the 9-Node Degenerated Shell Element with Special Emphasis on Thin

Shell Application and Reduced Integration,” Computer Methods in Applied Mechanics and Engineering,

Vol. 20, No. 3, December 1979, pp. 323-350.

Thomas, Kevin and Sobel, L. H., Evaluation of the STAGSC-1 Shell Analysis Computer Code, Report No.

WARD-10881, Westinghouse Electric Corporation, Madison, PA, August 1981.

MacNeal, R. H. and Harder, R. L., “A Proposed Standard Set of Problems to Test Finite Element

Accuracy,” Finite Element Analysis and Design, Vol. 1, No. 1, April 1985, pp. 1-20.

Belytschko, T. and Liu, W. K., “Test Problems and Anomalies in Shell Finite Elements,” in Reliability of

Methods for Engineering Analysis, K. J. Bathe and D. R. J. Owen (editors), Pineridge Press, 1986, pp.

393-406.

Zienkiewicz, O. C. and Taylor, R. L., The Finite Element Method – Volume 2: Solid and Fluid

Mechanics, Dynamics and Non-linearity, Fourth Edition, McGraw-Hill Book Company, 1991, pp. 123,

127, 176-179.

Phaal, R. and Calladine, C. R., “A Simple Class of Finite Elements for Plate and Shell Problems. II: An

Element for Thin Shells, with Only Translational Degrees of Freedom,” International Journal for

Numerical Methods in Engineering, Vol. 35, No. 5, September 1992, pp. 979-996.

Muhanna, Rafi L., “New Assumed Natural Strain Formulation of the Shallow Shell Element,”

Communications in Numerical Methods in Engineering, Vol. 9, No. 12, December 1993, pp. 989-1004.

Rengarajan, G., Aminpour, M. A., and Knight, N. F., Jr. “Improved Assumed-Stress Hybrid Shell

Element with Drilling Degrees of Freedom for Linear Stress, Buckling and Free Vibration Analyses,” 

International Journal for Numerical Methods in Engineering, Vol. 38, No. 11, June 1995, pp. 1917-1943.
119

Transient Response of Truncated Conical Shell

Background

To verify the transient solution algorithm, the linear elastic collapse of a truncated conical shell subjected

to an impulse load (initial velocity). Hartung (1971) presented this problem as part of an assessment of 

shell analysis capabilities and Hartung and Ball (1973) included this shell structure as one of the three 

challenge problems to assess shell structural analysis capabilities of various computer codes. Knight et

al. (1989) also used this problem to assess the CSM Testbed capabilities for the linear elastic transient

dynamic analysis of shells. The geometry and material properties of the problem are defined in Figure 37

using U.S. customary units.

Figure 37. Truncated conical shell problem: geometry and material properties.

Modeling and Analysis Process

The STAGS finite element model considered in this test case problem involves a single shell unit and

only 2-D shell elements. Symmetry conditions are exploited and only a 180-degree model of the conical

shell is used. The loading is a cosine distribution of a normal initial velocity load distributed over the

upper 90-degree segment (see Figure 37). The impulse is uniform along the axis of the shell.

The STAGS model is generated using a single shell unit with the conical shell surface geometry

(ISHELL=6). Material properties and shell wall construction are defined using both the historical
120

STAGS approach and the current GCP approach. Mesh discretization studies include different levels of 

mesh refinement and different element types. Mesh refinement is readily performed by changing the 

number of rows and columns of nodes in each direction on the F-1 record. Element type is selected using

the N-1 record (KELT). Representative finite element model using 31×19 mesh of nodes is shown in

Figure 38 for the 4-node shell elements.

Material properties and shell-wall construction are defined using both the historical STAGS approach

(i.e., STAGS versions prior to GCP) and the current GCP approach. Material modeling for an elastic 

isotropic material using the historical STAGS approach requires data on the I-1 and I-2 records to define

the material properties and the K-1 and K-2 records to define the shell fabrication data. Material modeling

using the current GCP approach requires data on the I-5a and I-6a records to define the material

properties and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the shell fabrication data.

While not used, records I-5a, I-22a, and I-22b are used to define the solid fabrication data.

Boundary condition on the displacements are specified using the P-1 and P-2 records. The symmetry

boundary conditions along the straight boundary, while the curved boundaries are clamped. The STAGS

definition of these conditions is used.

The impulse loading condition is defined as an initial velocity condition using the Q-records. The looping

option on all rows is exploited to impose a uniform initial velocity condition along the shell at each

circumferential location (see the Q-3 records in the trcone.inp S1 input file). However, the 

magnitude of the initial velocity at each note must be computed externally for each finite element

discretization change in the circumferential direction. A FORTRAN computer code is developed that

creates the loading records for a given finite element mesh of uniformly distributed nodes. A listing of 

this code is given in Figure 39. The output is written to FORTRAN unit 6 (standard output) – typically

the screen. The user may then “cut-and-paste” these lines directly into the input file.
121

Figure 38. Representative finite element models of the truncated conical shell

- 31×19 mesh of nodes on the shell surface.

program velocity

double precision dtheta, vel, V0

integer ncols,nstart,nele, i

double precision pi, dtr

c

pi = acos(-1.0d0)

dtr = pi/180.0d0

c

ncols = 19

nstart = (ncols-1)/2+1

nele = ncols-nstart

dtheta = 90.0d0/nele

V0 = 444.08

print *, nele, dtheta

c

do i=1,nele

vel=V0*sin(dtr*i*dtheta)

irow = nstart+i

write(6,100) vel,irow

100 format(F10.5,' -1 3 0 ',i2,

1 3x,'$Q-3 initial velocity loading')

end do

stop

end

Figure 39. Listing of the FORTRAN computer code used to generate the initial velocity loading 

for the truncated conical shell.
122

Numerical Results and Discussion

The linear transient dynamic response is computed using the Park 3-step implicit direct time integration

procedure with a fixed time step size Δt of two microseconds for a duration of 1500 microseconds (750

time steps). The predicted linear transient response for two points on the shell is given in Figure 40 for 

the transverse normal (radial) deflection component. Both points are located 6.5 inches from the

clamped, small diameter edge: one at θ=90° (point a) and one at θ=-90° (point b). Point a is directly

under the maximum initial velocity and immediately responds to the impulse. Point b is 180-degrees

away and has no initial velocity, and hence some time passes before the point deflects.

The transient behavior of the hoop stress resultant for selected times during the linear transient dynamic

analysis is given in Figure 41. The contour levels are held constant for all plots, and the contours are

displayed on the deformed geometry shapes of the shell wherein the deflections are exaggerated for

viewing. Note that from Figure 40 the amplitude of the transverse normal deflections at points a and b is

less than ten percent of the shell thickness.
123

Figure 40. Linear transient response of truncated conical shell due to impulse load obtained 

using 31×19 mesh of nodes and the E410 4-node quadrilateral shell element.
124

Figure 41. Contour plots of the hoop stress resultant on the deformed geometry shapes of the

clamped truncated conical shell subjected to an impulse load: E410 shell element, 31×19 mesh of

nodes.

0

6000

-8000

Hoop Stress

Resultant

lb./in.

Step 5, time t=10 μ sec.

Step 200, time t=400 μ sec.

Step 100, time t=200 μ sec.

Step 300, time t=600 μ sec.

Clamped

Sym.

Sym.

Clamped
125

Figure 41. Concluded

0

6000

-8000

Hoop Stress

Resultant

lb./in.

Step 600, time t=1200 μ sec. Step 750, time t=1500 μ sec.

Step 400, time t=800 μ sec. Step 500, time t=1000 μ sec.
126

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Truncated-cone

Under this directory are the files for the 2D shell finite element models and analysis.

2D Shell Model Input Files

The following text files give the input for the hinged cylindrical shell using the E410 4-node shell element

with a 31×19 mesh of nodes on the shell surface. The S2 input file contains input sufficient to use the

transient analysis procedure.

trcone.inp (for S1 processor)

2D truncated cone subjected to impulsive loading $A-1

C

C Elastic linear transient response of a truncated conical

C shell with clamped ends and impulsively loaded by an

C initial velocity

C

C References:

C 1. Hartung, R. F., "An Assessment of Current Capability

C for Computer Analysis of Shell Structures," Computers

C and Structures, Vol. 1, 1971, pp. 3-32.

C 2. Hartung, R. F. and Ball, R. E., "A Comparison of Several

C Computer Solutions to Three Structural Shell Analysis

C Problems," Technical Report No. AFFDL-TR-73-15, April 1973.

C 3. Knight, et al., "Large-Scale Structural Analysis: The

C Structural Analyst, The CSM Testbed, and The NAS System,"

C NASA TM-100643, March 1989.

C

0 0 0 0 0 3 0 $b-1

1 20.0 / 2 60.0 / 3 0.0 $b-1b model rotations

1 0 0 0 0 0 0 $b-2

1 0 1 0 0 1 $b-3

31 19 $f-1 Nrows (length) x Ncols (circumference)

C

C Material Record using Historical Approach

C

1 0 $I-1 material table

3.52E+6 0.286 0.0 .0726 $i-2 E, nu, G=E/2/(1+nu), rho (for volume check)

C

C GCP Input

C

ISOELASTIC_MATERIAL 1 1 1 $i-5

3.52E+6, $i-6a Young's modulus, psi

0.286, $i-6a Poisson's ratio

1.88E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Solid fabrications - element thicknesses NOT total wall thickness!

C

SOLID_FABRICATION 1 1 0 0 $i-5a

0.543 $i-22a element thickness

SOLID_FABRICATION 2 1 0 0 $i-5a

0.2715 $i-22a element thickness

C

C Shell wall fabrications

C

SHELL_FABRICATION 1 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym

1 $I-21a matid
127

0.543 $i-21c thickness, inches

0.0 $i-21d angle

C

END $I-5a end GCP input

C

C Wall Record using Historical Approach

C

1 1 1 0 $k-1 thickness, inches

1 0.543 0.0 $k-2

C

C Shell Unit Definition - using 2D shell elements

C

6 0 0 0 0 0 0 $m-1 truncated cone geometry

0.0 15.004 -90.0 90.0 7.95 10.23 $m-2 x1, x4, y1, y2, Ra, Rb

-1 0 0.0 0.0 0 0 $m-5 shell wall selection

410 0 0 0 $n-1 element options

C

C Boundary conditions

C

2 4 2 4 $p-1 clamped-sym-clamped-sym

C

C Loading - point load at center

C

0 1 $q-1 load summary

-1 9 0 $q-2

-77.11368 -1 3 0 11 $Q-3 initial velocity loading

-151.88431 -1 3 0 12 $Q-3 initial velocity loading

-222.04000 -1 3 0 13 $Q-3 initial velocity loading

-285.44912 -1 3 0 14 $Q-3 initial velocity loading

-340.18502 -1 3 0 15 $Q-3 initial velocity loading

-384.58456 -1 3 0 16 $Q-3 initial velocity loading

-417.29870 -1 3 0 17 $Q-3 initial velocity loading

-437.33343 -1 3 0 18 $Q-3 initial velocity loading

-444.08000 -1 3 0 19 $Q-3 initial velocity loading

0 0 0 0 0 0 2 0 0 $r-1 Output selection

13 1 $r-2 selected displacement output (bottom)

13 19 $r-2 selected displacement output (top)

trcone.bin (for S2 processor)

Truncated conical shell with initial velocity impulsive loading $a-1

C

C Linear transient dynamic solution control

C

7 5 0 0 0 0 0 -1 $b-1

0.0 0.0 0.0 $c-1

0 400 10 -20 0 1.0e-4 $d-1

0.0 1500.E-6 2.0e-6 0.04 $e-1 Time integration parameters

0 4 0 0 0 0 0 $e-2

trcone.pin (for STAPL processor)

Truncated conical shell with impulsive loading $A-1

16 0 1 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C

C stress resultant plots for linear solution

C

2 0 5 5 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 50 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP
128

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 100 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 150 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 200 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 250 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 300 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 350 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 400 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 450 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 500 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 550 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 600 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 650 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 700 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0

2 0 5 750 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 2 0.0 -8000.0 6000.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 60.0
129

trcone.pxy (for XYTRANS processor)

This input file is generated and saved during the first execution of XYTRANS (so called journal file).

Once created it can be used over and over again to extract the same information from a STAGS run.

P $ (P)lotps or (S)pread_Sheet output

trcone $ STAGS solution 'Case Name'

F $ (F)ull or (C)ondensed Model

Y $ (Y)es-(N)o: setup data for another plot

4 $ x-axis variable = choice (1 to 15)

N $ (Y)es-(N)o: specify x-variable scale factor

5 $ y-axis variable = choice (1 to 15)

0 $ node no. (0 = ask for Unit,Row,Col)

1 14 19 $ (U)nit, (R)ow, (C)ol - Node No. = 266

3 $ comp no., dis,vel,acc (1-6) = u,v,w,ru,rv,rw

S $ (G)lobal or (S)hell ref surface

N $ (Y)es-(N)o: specify y-variable scale factor

N $ (Y)es-(N)o: specify subrange of loadsteps

Y $ (Y)es-(N)o: plotted points start at origin

Y $ (Y)es-(N)o: setup data for another plot

4 $ x-axis variable = choice (1 to 15)

N $ (Y)es-(N)o: specify x-variable scale factor

5 $ y-axis variable = choice (1 to 15)

0 $ node no. (0 = ask for Unit,Row,Col)

1 14 1 $ (U)nit, (R)ow, (C)ol - Node No. = 248

3 $ comp no., dis,vel,acc (1-6) = u,v,w,ru,rv,rw

S $ (G)lobal or (S)hell ref surface

N $ (Y)es-(N)o: specify y-variable scale factor

N $ (Y)es-(N)o: specify subrange of loadsteps

Y $ (Y)es-(N)o: plotted points start at origin

N $ (Y)es-(N)o: setup data for another plot

Problem References

Hartung, R. F., “An Assessment of Current Capability for Computer Analysis of Shell Structures,”

Computers and Structures, Vol. 1, 1971, pp. 3-32.

Hartung, R. F. and Ball R. E., A Comparison of Several Computer Solutions to Three Structural Shell

Analysis Problems, AFFDL Report No. AFFDL-TR-73-15, April 1973.

Knight, N. F., Jr., McCleary, S. L., Macy, S. C., and Aminpour, M. A., Large-Scale Structural Analysis: 

The Structural Analyst, The CSM Testbed, and The NAS System, NASA TM-100643, March 1989.

Hurlbut, B. J., Stanley, G. M., and Kang, D. S., The Computational Structural Mechanics (CSM) Testbed

Applications Manual, Lockheed Contract Report No. LMSC-F333007, May 1989.

Rankin, C. C., Brogan, F. A., Loden, W., and Cabiness, H., Structural Analysis of General Shells –

STAGS User Manual, Version 4.0, Lockheed Martin Advanced Technology Center, Palo Alto, CA, June

2000.
130

Snap-Through of Hinged Shallow Cylindrical Shell

Background

To verify the nonlinear solution algorithm and nonlinear aspects of the shell element and corotational

formulations, the snap-through response of a hinged cylindrical shallow shell under a central point force 

is studied. This problem involves only moderate geometric nonlinearities and exhibits a limit point in the 

nonlinear response. This problem posed by Sabir and Lock (1972) is a very popular test case for shell

elements and nonlinear solution procedures for quasi-static behavior (e.g., Gass and Tabarrok, 1976;

Ramm, 1981; Hinton and Lo, 1982; Jeusette et al., 1989; Eriksson , 1989; Hurlbut et al., 1989; Moy and

Lam, 1991). The geometry and material properties of the problem are defined in Figure 42 using U.S.

customary units and SI units. Three values of shell thickness are considered: 1.00 in. (25.4 mm); 0.50 in.

(12.7 mm); and 0.25 in. (6.35 mm). The rise of the shell H is 0.5 inches (12.7 mm).

Figure 42. Hinged cylindrical shallow shell problem: geometry and material properties.

Modeling and Analysis Process

Two separate STAGS finite element models are considered in this test case problem: shell elements and

solid elements. A summary of each model includes:

2-D shell model – Model the shell with plate elements (x-y plane) in a single shell unit.

3-D solid model – Model shell with solid elements in a single shell unit and having multiple elements

through the shell thickness.

E = 450 ksi = 3102.642 N/mm

2

ν = 0.3

R = 100.0 in. = 2540 mm

L = 10.0 in. = 254.0 mm

θ = 0.1 radians = 5.7296°

H = R (1-cos θ)

Hinge

2L

P

Free R
131

The STAGS model is generated using a single shell unit with the cylindrical shell surface geometry

(ISHELL=5). Material properties and shell wall construction are defined using both the historical

STAGS approach and the current GCP approach. Mesh discretization studies include different levels of 

mesh refinement and different element types. Mesh refinement is readily performed by changing the 

number of rows and columns of nodes in each direction on the F-1 record. Element type is selected using

the N-1 record (KELT). Note that E430 uses two E330 triangular elements for each 4-node quadrilateral

subdomain. Multiple solid elements through the thickness are specified using the NLAYS and NFABS 

parameters on the M-1 record in combination with NFABS sets of M-5 records. For this study, only two

and four solid elements through the shell wall thickness are used. Representative finite element models

using 11x11 mesh of nodes in the plane are shown in Figure 42 for the 3-node, 4-node, and 9-node shell

elements as well as for the 8-node solid element with four elements in the thickness direction.

Material properties and shell-wall construction are defined using both the historical STAGS approach

(i.e., STAGS versions prior to GCP) and the current GCP approach. Material modeling for an elastic 

isotropic material using the historical STAGS approach requires data on the I-1 and I-2 records to define

the material properties and the K-1 and K-2 records to define the shell fabrication data. Material modeling

using the current GCP approach requires data on the I-5a and I-6a records to define the material

properties and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the shell fabrication data. In

addition, records I-5a, I-22a, and I-22b are used to define the solid fabrication data.

Boundary condition on the displacements are specified using the P-1 and P-2 records. The boundary

conditions along the straight boundary are hinged (v=w=0 and ry=rz=0), while the curved boundary are 

free. Symmetry boundary conditions are imposed on the interior straight and curved edges. For the 3D

finite element models, the displacement boundary conditions are imposed using the Q-3 records and on

each nodal layer in the model.

A point load is applied at the center of the panel that is at the origin of the finite element model coordinate

frame. Because of the symmetry conditions, only one fourth of the applied load is used on the quarter 

model. The base load given on the Q-3 record is 0.25 and then the load factor on the C-1 record of the S2

input file gives the total load amplitude (i.e., the load factor PA is related to the total load on the shell).

The internal force at that node and in the direction of the loading can be computed and used for plotting as

well via the XYTRANS utility.
132

Figure 42. Representative finite element models of the hinged cylinder

- 11×11 mesh of nodes on the shell surface.

Numerical Results and Discussion

Results for this problem are more complicated to present because of the nonlinear snap-through response 

of the shell structure. Three different values of the shell thickness are studied: 25.40-mm thick, 12.70-

mm thick, and 6.35-mm thick. For the 25.40-mm-thick shell, the nonlinear response exhibits an

inflection point but does not snap through. For the 12.70-mm-thick shell, the nonlinear response exhibits

a limit point and using displacement-control or the arc-length-control procedure the unstable branch of the

nonlinear response can be traced. For the 6.35-mm-thick shell, the nonlinear response exhibits a 

horizontal limit point and a vertical limit (snap-through and snap-back behavior, respectively). These 

characteristics are displayed in Figure 43 for an 11×11 mesh of nodes and the E410 4-node quadrilateral

shell element. The solutions were obtained using the arc-length control procedure that automatically

adjusts the solution step size.

Convergence studies were performed for the E410 and E480 shell elements. Results shown in Figures 44

through 46 are for different levels of discretization using the E410 4-node and E480 9-node shell elements

for the three shell thickness values considered. These convergence studies included meshes where the

number of nodes per edge equaled 3, 5, 7, 11, and 21. For the E410 element, these meshes correspond to

2, 4, 6, 10, and 20 4-node elements per edge, respectively. For the E480 element, these meshes

correspond to 1, 2, 3, 5, and 10 9-node elements per edge, respectively.

(a) E330 model. (b) E410 model.

(c) E480 model. (d) E881 model.
133

Figure 43. Basic hinged cylindrical shell response for three values of shell thickness obtained 

using 11×11 mesh of nodes and the E410 4-node quadrilateral element.

25.40-mm-thick

6.35-mm-thick

12.70-mm-thick
134

(a) 4-node E410 shell element.

(b) 9-node E480 shell element.

Figure 44. Hinged cylindrical shell response to a central point load – 25.40-mm thick.
135

(a) 4-node E410 shell element.

(b) 9-node E480 shell element.

Figure 45. Hinged cylindrical shell response to a central point load – 12.70-mm thick.
136

(a) 4-node E410 shell element.

(b) 9-node E480 shell element.

Figure 46. Hinged cylindrical shell response to a central point load – 6.35-mm thick.
137

These results indicate that good solutions can be obtained even with just one or two elements

along an edge of the quarter model. As the shell thickness decreases, the number of elements

required for a converged solution increases. It is interesting that with as few as two elements per

edge, the E410 shell element captures the first limit point very well for even the thinnest shell but

the response exhibits a greater degree of snap-back. With a single E480 shell element, the basic

behavior is captured, but additional elements are required to capture the snap-through and snapback behavior.

Contour plots of the transverse normal deflection for the 12.70-mm-thick shell are shown in

Figure 47 for an 11×11 mesh of nodes and the E410 shell element. Initially the center point

deflects and pulls the shell surface down. As the limit point is approached, the shell deflection 

patterns approach that of an arch response. Following complete snap through, the center point

deflects further, causing stretching of the middle surface.

Prediction of the hinged cylindrical shell response using the E330 MIN3 triangular shell

elements in STAGS was not as readily obtained. Note that STAGS will automatically subdivide

a 4-node subregion into two 3-node regions. Users typically use the designation E430 on the N1 record to cause this result. First, in all other simulations the response was obtained using no 

more than five step size cuts – the E330 model required more but fewer than ten. Second, the

E330 element has artificial drilling stiffness based on a penalty approach. Leaving the drilling 

degrees of freedom free or unrestrained caused the solution to bog down and well below the first

limit point as shown in Figure 48. Constraining all drilling degrees of freedom resulted in a

solution comparable to that obtained using the E410. Note the E410 element does have drilling

degrees of freedom; however, these freedoms contribute to the in-plane displacement field

approximations and do not use artificial stiffness for those freedoms.

Results obtained using the E881 8-node ANS solid element are shown in Figure 49. For the

solid models, the symmetry boundary conditions were imposed on all nodes on the symmetry

plane. To simulate the hinged condition, the transverse normal deflection was restrained on all

nodes on the hinged plane, while the in-plane circumferential displacement was only restrained

at the midplane of shell. Three different discretizations of the shell surface are considered: 11

nodes per edge, 21 nodes per edge and 41 nodes per edge. The solid models had either two or

four elements through the shell thickness. Results from the E410 simulation are included for

comparison. These results indicate that increasing the number of elements through the thickness

had only a minor effect on the center transverse normal deflection. Increasing the number of

nodes per edge had a significant effect on the response; however, even with 41 nodes per edge,

the second limit point was still not accurately predicted – the first limit point was predicted

satisfactorily.
138

Figure 47. Contour plots of the transverse normal deflection on the deformed surface for

selected values of the applied point load – 12.7-mm-thick shell, E410 element, 11×11 mesh of

nodes.

Step 7 – approaching the limit

point.

Step 11 – near the limit point.

Step 17 – just past the limit

point. Step 19 – just past the limit

point.

Step 23 – near the second limit

point.

Step 24 – past the second limit

point.

0

-24

Transverse

Normal

Deflection

w, mm

Hinged

Free

Sym.

Sym.

P
139

Figure 48. Hinged cylindrical shell response to a central point load – 12.70-mm thick.
140

Figure 49. Hinged cylindrical shell response to a central point load – 12.7-mm thick.
141

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Sample-Testcases/Snap-Through

Under this directory are two subdirectories: 2D/ contains the files for the 2D shell finite element models

and analyses and 3D/ contains the files for the 3D solid finite element models and analyses.

2D Shell Model Input Files

The following text files give the input for the hinged cylindrical shell using the E410 4-node shell element

with an 11×11 mesh of nodes on the shell surface. These files are in the 2D/ subdirectory. The S2 input

file contains input sufficient to use the hybrid transient-static procedure in the event a load control

solution algorithm is used for the nonlinear static analysis. If so, then the solution will stop at or near the

limit point. Then using information from a linear vibration analysis, a nonlinear transient analysis can be

started using a higher load to cause the shell to snap through – too small a value will just bring you closer 

to the limit point. After the transient is completed, the nonlinear static analysis can be resumed starting

with a load relaxation step to guarantee equilibrium is re-established.

hinge2d.inp (for S1 processor)

2D Hinged Cylindrical Shallow Shell with Central Point Load $A-1

0 0 0 0 0 3 0 $b-1

1 -67.0 / 2 0.0 / 3 -34.0 $b-1b model rotations

1 0 0 0 0 0 0 $b-2

2 0 3 0 0 1 $b-3

11 11 $f-1 grid (nrows by ncols of NODES)

C

C Material Record using Historical Approach

C

1 0 $I-1 material table

450000. 0.3 0.0 .1 $i-2 E, nu, G=E/2/(1+nu), rho (for volume check)

2 0 $I-1 material table

3.10275E3 0.3 0.0 0.1 $i-2 N/mm^2

C

C GCP Input

C

ISOELASTIC_MATERIAL 1 1 1 $i-5

450000.0, $i-6a Young's modulus, psi

0.3, $i-6a Poisson's ratio

2.58799E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

ISOELASTIC_MATERIAL 2 1 1 $i-5

3.10275E3, $i-6a Young's modulus, N/mm^2

0.3, $i-6a Poisson's ratio

2.58799E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Solid fabrications - element thicknesses NOT total wall thickness!

C

SOLID_FABRICATION 1 1 0 0 $i-5a

25.4 $i-22a element thickness

SOLID_FABRICATION 2 1 0 0 $i-5a

12.7 $i-22a element thickness

SOLID_FABRICATION 3 1 0 0 $i-5a

6.35 $i-22a element thickness

C

C Shell wall fabrications (total thicknesses)

C

SHELL_FABRICATION 1 1 0 1 0 $i-5a fabid, nlayer, ipts, ishr, isym

2 $I-21a matid
142

25.4 $i-21c thickness - thick

0.0 $i-21d angle

0.83333 0.83333 $i-21e shear correction factors

SHELL_FABRICATION 2 1 0 1 0 $i-5a fabid, nlayer, ipts, ishr, isym

2 $I-21a matid

12.7 $i-21c thickness - thin

0.0 $i-21d angle

0.83333 0.83333 $i-21e shear correction factors

SHELL_FABRICATION 3 1 0 1 0 $i-5a fabid, nlayer, ipts, ishr, isym

2 $I-21a matid

6.35 $i-21c thickness - very thin

0.0 $i-21d angle

0.83333 0.83333 $i-21e shear correction factors

C

END $I-5a end GCP input

C

C Wall Record using Historical Approach (total thicknesses)

C

1 1 1 0 $k-1 thick shell

2 25.40 0.0 $k-2

2 1 1 0 $k-1 thin shell

2 12.7 0.0 $k-2

3 1 1 0 $k-1 very thin shell

2 6.35 0.0 $k-2

C

C Shell Unit Definition - using 2D shell elements

C

5 0 0 0 0 0 0 $m-1 cylindrical shell geometry

0.0 254.0 0.0 5.7296 2540.0 $m-2 x1, x4, y1, y2, R

-2 0 0.0 0.0 0 0 $m-5 shell wall selection

410 $n-1 element options

C

C Boundary conditions

C

4 0 3 4 $p-1 sym-hinged-free-sym

100 100 $p-2 v=w=0 and ry=rz=0 on straight boundary (hinged; immovable)

C

C Loading - point load at center

C

1 0 $q-1 load summary

1 1 0 $q-2

C0.0 -1 6 0 0 0 $Q-3 Set RW=0 for E480 and E330 elements

-0.25E+3 1 3 1 1 0 $Q-3 0.25*P*1000 at panel center

0 0 0 0 0 0 1 0 1 $r-1 Output selection

1 0 $r-2 selected displacement output

hinge2d.bin (for S2 processor)

Hinged Cylindrical Shallow Shell Problem $A-1

C

C Nonlinear static solution control

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

0.2 0.1 20.0 $C-1 LOAD MULTIPLIERS

0 1000 5 20 0 1.0e-4 1.0 $d-1 strategy parameters

0 0 0 $et-1

C

C Nonlinear static restart after transient

C with load relaxation as a first step

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

2.3 0.1 20.0 $C-1 LOAD MULTIPLIERS
143

32 100 5 20 1 1.0e-4 1.0 $d-1 strategy parameters

5 0 1 $et-1 do load relaxation and use previous solution as estimate

C

C Nonlinear transient dynamic solution control from static solution

C

6 1 1 0 0 0 0 -1 $b-1

2.20430 0.0 2.20430 $c-1

10 200 10 -20 0 1.0e-4 $d-1

0.0 200.0 1.0e-3 100.0 0.1295 0.772 $e-1

0 4 1 0 0 1 0 $e-2

2.30 0.0 0.0 1000.0 1000.0 0.0 $e-3

C

C Linear free vibration analysis

C

2 1 1 0 0 0 0 -1 $b-1

1.0 0.0 1.0

0 0 0

2

C

C Nonlinear transient dynamic solution control from static solution

C

6 1 1 0 0 0 0 -1 $b-1

2.20430 0.0 2.20430 $c-1

10 200 10 -20 0 1.0e-4 $d-1

0.0 0.2 1.0e-8 100.0 0.1295 0.772 $e-1

0 4 1 0 0 1 0 $e-2

2.20430 0.0 0.0 100.0 100.0 0.0 $e-3

hinge2d.pin (for STAPL processor)

Hinged Cylindrical Shell with center point load $a-1 shell thickness = 12.7mm

6 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C contour plots of w-deflection with fixed range of values (-24mm to 0)

2 0 1 7 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -24.0 1.0e-8 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 11 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -24.0 1.0e-8 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 17 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -24.0 1.0e-8 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 19 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -24.0 1.0e-8 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 23 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -24.0 1.0e-8 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 24 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -24.0 1.0e-8 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2

hinge2d.pxy (for XYTRANS processor)

This input is generated and saved during the first execution of XYTRANS (so called journal file). Once

created it can be used over and over again to extract the same information from a STAGS run.

P $ (P)lotps or (S)pread_Sheet output

hinge2d $ STAGS solution 'Case Name'

F $ (F)ull or (C)ondensed Model

Y $ (Y)es-(N)o: setup data for another plot
144

5 $ x-axis variable = choice (1 to 15)

0 $ node no. (0 = ask for Unit,Row,Col)

1 1 1$ (U)nit, (R)ow, (C)ol - Node No. = 1

3 $ comp no., dis,vel,acc (1-6) = u,v,w,ru,rv,rw

G $ (G)lobal or (S)hell ref surface

8 $ y-axis variable = choice (1 to 15)

0 $ node no. (0 = ask for Unit,Row,Col)

1 1 1$ (U)nit, (R)ow, (C)ol - Node No. = 1

3 $ comp no., int-for (1-6) = Fu,Fv,Fw,Mu,Mv,Mw

G $ (G)lobal or (S)hell ref surface

N $ (Y)es-(N)o: specify subrange of loadsteps

Y $ (Y)es-(N)o: plotted points start at origin

N $ (Y)es-(N)o: setup data for another plot

3D Solid Model Input Files

The following text files give the input for the hinged cylindrical shell using the E881 8-node solid

element with an 11×11 mesh of nodes on the shell surface and four elements through the shell thickness

(five nodal layers). These files are under the 3D/ subdirectory.

hinge3d.inp (for S1 processor)

3D Hinged Cylindrical Shallow Shell with Central Point Load $A-1

0 0 0 0 0 3 0 $b-1

1 -67.0 / 2 0.0 / 3 -34.0 $b-1b model rotations

1 0 0 0 0 0 0 $b-2

2 0 3 0 0 1 $b-3

21 21 $f-1 grid (nrows by ncols of NODES)

C

C Material Record using Historical Approach

C

1 0 $I-1 material table (US Customary UNITS)

450000. 0.3 0.0 .1 $i-2 E, nu, G=E/2/(1+nu), rho (for volume check)

2 0 $I-1 material table (Metric)

3.10275E3 0.3 0.0 0.1 $i-2 N/mm^2

C

C GCP Input

C

ISOELASTIC_MATERIAL 1 1 1 $i-5

450000.0, $i-6a Young's modulus, psi

0.3, $i-6a Poisson's ratio

2.58799E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

ISOELASTIC_MATERIAL 2 1 1 $i-5

3.10275E3, $i-6a Young's modulus, N/mm^2

0.3, $i-6a Poisson's ratio

2.58799E-4, $i-6a Mass density

4*0.0 $i-6a unused properties

C

C Solid fabrications - element thicknesses NOT total wall thickness!

C Note: these models have 2 or more elements through the thickness

C

SOLID_FABRICATION 1 2 0 0 $i-5a

12.7 $i-22a element thickness

SOLID_FABRICATION 2 2 0 0 $i-5a

6.35 $i-22a element thickness

SOLID_FABRICATION 3 2 0 0 $i-5a

3.175 $i-22a element thickness

C

C Shell wall fabrications ( these are total thicknesses)

C

SHELL_FABRICATION 1 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym
145

2 $I-21a matid

25.4 $i-21c thickness - thick

0.0 $i-21d angle

SHELL_FABRICATION 2 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym

2 $I-21a matid

12.7 $i-21c thickness - thin

0.0 $i-21d angle

SHELL_FABRICATION 3 1 0 0 0 $i-5a fabid, nlayer, ipts, ishr, isym

2 $I-21a matid

6.35 $i-21c thickness - very thin

0.0 $i-21d angle

C

END $I-5a end GCP input

C

C Wall Record using Historical Approach (total thicknesses)

C

1 1 1 0 $k-1 thick shell

2 25.4 0.0 $k-2

2 1 1 0 $k-1 thin shell

2 12.7 0.0 $k-2

3 1 1 0 $k-1 very thin shell

2 6.35 0.0 $k-2

C

C Shell Unit Definition - using 3D solid elements

C

5 0 0 0 4 4 $m-1 cylindrical shell geometry

0.0 254.0 0.0 5.7296 2540.0 $m-2 x1, x4, y1, y2, R

-3 0 0.0 0.0 0 0 $m-5 shell wall selection

-3 0 0.0 0.0 0 0 $m-5 shell wall selection

-3 0 0.0 0.0 0 0 $m-5 shell wall selection

-3 0 0.0 0.0 0 0 $m-5 shell wall selection

881 $n-1 element options

C

C Boundary conditions (see q-3 records)

C BC: sym-hinged-free-sym

C

3 3 3 3 $p-1 all edges free

C

C Loading - point load at center

C

1 0 $q-1 load summary

1 16 0 $q-2

-0.25E+3 1 3 1 1 0 0 0 0 0 1 $Q-3 0.25*P*1000 at panel center

0.0 -1 1 1 0 0 0 0 0 0 1 $q-3 u=0 on Row 1 of Layer 1

0.0 -1 1 1 0 0 0 0 0 0 2 $q-3 u=0 on Row 1 of Layer 2

0.0 -1 1 1 0 0 0 0 0 0 3 $q-3 u=0 on Row 1 of Layer 3

0.0 -1 1 1 0 0 0 0 0 0 4 $q-3 u=0 on Row 1 of Layer 4

0.0 -1 1 1 0 0 0 0 0 0 5 $q-3 u=0 on Row 1 of Layer 5

0.0 -1 2 0 1 0 0 0 0 0 1 $q-3 v=0 on Col 1 of Layer 1

0.0 -1 2 0 1 0 0 0 0 0 2 $q-3 v=0 on Col 1 of Layer 2

0.0 -1 2 0 1 0 0 0 0 0 3 $q-3 v=0 on Col 1 of Layer 3

0.0 -1 2 0 1 0 0 0 0 0 4 $q-3 v=0 on Col 1 of Layer 4

0.0 -1 2 0 1 0 0 0 0 0 5 $q-3 v=0 on Col 1 of Layer 5

0.0 -1 3 0 21 0 0 0 0 0 1 $q-3 v=w=0 on Col NCOL of Layer 1

0.0 -1 3 0 21 0 0 0 0 0 2 $q-3 v=w=0 on Col NCOL of Layer 2

0.0 -1 2 0 21 0 2 1 0 0 3 $q-3 v=w=0 on Col NCOL of Layer 3

0.0 -1 3 0 21 0 0 0 0 0 4 $q-3 v=w=0 on Col NCOL of Layer 4

0.0 -1 3 0 21 0 0 0 0 0 5 $q-3 v=w=0 on Col NCOL of Layer 5

0 0 0 0 0 0 1 0 1 $r-1 Output selection

1 0 $r-2 selected displacement output

hinge3d.bin (for S2 processor)

Hinged Cylindrical Shallow Shell Problem $A-1
146

C

C Nonlinear static solution control

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

0.2 0.1 20.0 $C-1 LOAD MULTIPLIERS

0 6000 5 20 0 1.0e-4 1.0 $d-1 strategy parameters

0 0 0 $et-1

hinge3d.pin (for STAPL processor)

Hinged Cylindrical Shell with center point load $a-1

5 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C contour plots of w-deflection on deformed shape

2 0 1 9 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 12 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 18 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 22 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0

2 0 1 25 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -67.0 / 2 0.0 / 3 -34.0
147

Problem References

Sabir, A. B. and Lock, A. C., “The Application of Finite Elements to the Large Deflection Geometrically

Nonlinear Behaviour of Cylindrical Shells,” in Variational Methods in Engineering – Volume II, C. A.

Brebbia and H. Tottenham (editors), Southampton University Press, 1972, pp. 7/66-7/75.

Gass, N. and Tabarrok, B., “Large Deformation Analysis of Plates and Cylindrical Shells by a Mixed

Finite Element Method,” International Journal for Numerical Methods in Engineering, Vol. 10, No. 4,

1976, pp. 731-746.

Ramm, E., “Strategies for Tracing the Nonlinear Response Near Limit Points,” in Nonlinear Finite 

Element Analysis in Structural Mechanics, W. Wunderlich, E. Stein, and K.-J. Bathe (editors), SpringerVerlag, Berlin, 1981, pp. 63-89

Hinton, E. and Lo, C. S., “Large Deflection Analysis of Imperfect Mindlin Plates using the Modified Riks

Method,” in The Mathematics of Finite Elements and Applications IV, MAFELAP 1981, J. R. Whiteman

(editor), Academic Press, London, 1982, pp. 111-118.

Jeusette, Jean-Pierre, Laschet, Gottfried, and Idelsohn, Sergio, “An Effective Automatic

Incremental/Iterative Method for Static Nonlinear Structural Analysis,” Computers and Structures, Vol.

32, No. 1, 1989, pp. 125-135.

Eriksson, Anders, “On Linear Constraints for Newton-Raphson Corrections and Critical Point Searches in

Structural F. E. Problems,” International Journal for Numerical Methods in Engineering, Vol. 28, No. 6,

June 1989, pp. 1317-1334.

Hurlbut, B. J., Stanley, G. M., and Kang, D. S., The Computational Structural Mechanics (CSM) Testbed

Applications Manual, Lockheed Contract Report No. LMSC-F333007, May 1989.

Moy, S. S. J. and Lam, S. S. E., “Geometrically Non-Linear Analysis of Shell Structures,”

Communications in Applied Numerical Methods, Vol. 7, No. 5, July 1991, pp. 377-391.
148

Advanced-Features Example Problems

The advanced-features example problems focus on the application of recent STAGS enhancements and

unique capabilities. These problems illustrate how to use and intrepret results for these applications. The 

problems include the analysis of a sandwich panel, the crack propagation of a middle-crack-tension panel

and a panel with multiple site damage, the application of the hybrid solution procedure using a composite 

curved panel with a central circular hole, the progressive failure analysis of a composite square panel

loaded in in-plane shear, two membrane wrinkling problems, and an actuator problem.
149

Buckling of Sandwich Panels

Background

Sandwich panels are generally described by two face sheets held apart by material referred to as the core.

The face sheets can be isotropic, orthotropic, or laminated, and each face sheet can be distinctly different.

The core material is often a foam or honeycomb material modeled as an orthotropic continuum. The core 

material usually has low in-plane stiffness compared to its transverse normal stiffness The geometry and

material properties of the problem are defined in Figure 50 using U.S. customary units and SI units.

Figure 50. Sandwich panel problem: geometry and material properties.

Geometry:

a = 20.0 in. = 508.0 mm

b = 10.0 in. = 254.0 mm

Face Sheet Material:

E = 10.0 Msi = 68.95 GPa

ν = 0.3

!

"

#

=

=

=

0.11in. 2.794 mm

0.02 in. 0.508 mm

f t

Core Material:

Ecx = 0.1 ksi = 0.6895 MPa

Ecy = 0.1 ksi = 0.6895 MPa

Ecz = 10.0 ksi = 68.95 MPa

Gcxy = 0.0384 ksi = 0.265 MPa 

Gcxz = 12.000 ksi = 82.74 MPa

Gcyz = 7.200 ksi = 49.64 MPa 

νcxy = 0.30

νcxz = 0.01

νcyz = 0.01

!

"

#

=

=

=

5.50 in. 139.70 mm

0.20 in. 5.08 mm

hc
150

Modeling and Analysis Process

Sandwich panel finite element modeling has generally taken one of three approaches depending on panel

geometry and constituent materials. The buckling behavior of a sandwich panel is dependent on the 

sandwich panel geometry and properties and may involve a general instability mode, a local instability

mode, or an interaction between the two. Accurate prediction of general or overall instability modes

requires adequate representation of the sandwich stiffnesses whereas prediction of local instabilities

requires detailed through-the-thickness modeling. The first modeling approach exploits standard shell

finite elements. These models are referred to herein as layered shell models (using either E410, E330, or

E480 shell elements), and for thin sandwich panels may provide a first approximation of the global

behavior. The second approach uses standard shell finite elements for the face sheets and solid threedimensional finite elements for the core. These models are referred to as layered shell/solid models (uses

E480 shell element for each face sheet and E883 solid element for the core) and provide a modeling

approach for both general and local response predictions. The accuracy of this approach, as well as its

computational cost, is related to the through-the-thickness modeling of the core material and the 

displacement field compatibility between the shell and solid elements (both quadratic). The third

approach is a full three-dimensional finite element model, in which solid three-dimensional elements are 

used to model both the face sheets and the core. These models are referred to as three-dimensional solid

models (using either E881, 883, or 885 solid elements) and they are typically reserved for detailed local

modeling because of their computational cost. Recently, an additional modeling approach has been

implemented in the STAGS nonlinear finite element code. This modeling approach, referred to herein as

sandwich element models (see Riks and Rankin, 2001, 2002), uses a specialty element developed

specifically for the analysis of sandwich structures (E840 sandwich element). Sandwich element models

embody the kinematics and stiffness of the sandwich structure for less computational cost than the layered

shell/solid models. Sandwich element models provide a cost-effective analysis approach for capturing

sandwich behavior for large-scale sandwich structure simulations and avoid the through-the-thickness

element aspect ratio issue associated with the use of solid elements. Sandwich elements provide accurate 

solutions for detailed local analyses as well. Several STAGS finite element models are considered for

this problem:

Full panel model using:

Layered shell modeling approach

Layered shell/solid modeling approach

Sandwich element modeling approach

Local strip model using:

Sandwich element modeling approach

The STAGS models for the layered shell and sandwich element modeling approaches (full panel and local

strip) are generated using a single shell unit for the rectangular panel surface geometry (ISHELL=1).

Finite element models for the thick sandwich case are shown in Figure 51 for the layered shell approach,

in Figure 52 for the sandwich element approach, in Figure 53 for the layered shell/solid approach, and in

Figure 54 for the local strip model.
151

(a) 4-node E410 quadrilateral shell element.

(b) 9-node E480 quadrilateral shell element.

Figure 51. Finite element model for the layered shell approach.
152

Figure 52. Finite element model for the sandwich element approach with two sandwich elements through

the thickness – three nodal planes, one “phantom” face sheet on the interior of the panel.

Figure 53. Portion of a finite element model for the layered shell/solid modeling approach with two E883

solid elements through the core thickness – five nodal planes plus E480 shell elements for each face sheet.

Note: some of the solid element faces shown in this view are “showing through” the face-sheet shell

elements in some locations.
153

Figure 54. Finite element model for the local strip model using 25 layers of sandwich elements through

the thickness, one element in width, 20 elements along the 2.5-in.-long strip length.
154

In these approaches, the reference surface is also the middle surface of the panel with no eccentricity

specified. The STAGS model for the layered shell/solid modeling approach is generated using three shell

units – one for each face sheet and one for the core. In the layered shell/solid approach, the reference

surface can be defined as the middle surface of the panel provided the face sheet shell elements are 

located properly. The reference surface for the bottom face sheet (nodal plane) is located by translating

the nodal plane to

hc z = !0.5

using the M-4d record and the middle surface of the shell element has and

eccentricity of

z f e = !0.5t

on the M-5 record. Similarly, the reference surface for the top face sheet is

located by translating the nodal plane to

hc z = +0.5

using the M-4d record and the middle surface of the

shell element has and eccentricity of 

z f e = +0.5t

on the M-5 record. The shell unit modeling the core 

using solid elements locates the reference surface at the middle of the accumulated thickness of the solid

elements – the bounding nodal planes are located at

hc z = ±0.5 .

Material properties and sandwich construction are defined using the GCP approach and also using the 

historical STAGS approach (I and K records). Material modeling using the current GCP approach

requires data on the I-5a and I-6a records to define the material properties and records I-5a, I-21a, I-21b,

I-21c, I-21d, and I-21e to define the shell fabrication. In addition, records I-5a, I-22a, and I-22b are used

to define the solid fabrication. For the sandwich elements, the core material properties are defined using

the solid fabrication records, while the face sheet properties are defined using the shell fabrication

records. The core material is defined using a solid fabrication type where the thickness represents half the

total core thickness (the finite element models used here have just two elements through the thickness).

The face sheet material is defined using the shell fabrication type. Two solid fabrications are included to

represent a thin core (

= 0.20 in. hc

) and a thick core (

= 5.50 in. hc

). Two shell fabrications are also

included to represent a thin face sheet (

= 0.02 in. f t ) and a thick face sheet (= 0.11in. f t ).

Mesh discretization studies include different levels of mesh refinement and different element types. Mesh

refinement is readily performed by changing the number of rows and columns of nodes in each planar

direction on the F-1 record. Element type is selected using the N-1 record (KELT). Multiple solid

elements through the thickness are specified using the NLAYS and NFABS parameters on the M-1 record

in combination with NFABS M-5 records. All of the full panel finite element models use 81 grid points

along the panel length and 21 grid points along the panel width.

Boundary conditions on the displacements are specified using the P-1 and P-2 records for the layered

shell modeling approach. Boundary conditions for the layered shell/solid and sandwich modeling

approaches are specified using the Q records – the P records will only constrain the degrees of freedom 

associated with the first nodal plane of a solid model. In the pre-stress condition, the sandwich panel is

loaded by a uniform end shortening, uo, applied to the sandwich face sheets on the ends of the panel at

x=0 and x=a (see Figure 52). The boundary conditions applied to all grid points along each edge are:

u = u0 and w = !x =!z = 0

along Edge 1 (x=0);

w =! y = 0

along Edges 2 and 4 (y=b and y=0,

respectively); and

u = !u0 and w = "x ="z = 0

along Edge 3 (x=a). In addition, the v displacement

component is fixed at the center of the panel on all nodal planes.

Numerical Results and Discussion

Full panel models are defined as finite element models of the entire sandwich panel. Spatial discretization

of the full panel is related to the anticipated buckling mode. Thus, some knowledge of the panel buckling

response is needed to develop these full panel analysis models. For a rectangular panel, the number of 

half-waves, m, along the panel length in a general-instability panel-buckling mode is a function of the
155

panel aspect ratio a/b, assuming a single half-wave across the width of the panel. Generally, five to six

grid points per half-wave are required for accurate buckling predictions. To capture a face-sheetwrinkling mode, the finite element mesh needs to be sufficiently refined to represent short-wavelength

buckles.

Local strip models are defined as finite element models of a localized region with significant through-thethickness modeling detail so that short wavelength wrinkling modes can readily be detected. A local strip

model is used to verify short-wavelength face-sheet-wrinkling behavior predictions obtained with the full

panel models. Local strip models represent a thin longitudinal slice of a panel away from edge effects. In

the present study this strip model has a width equal to 0.1 inches (2.54 mm) and has 25 layers of 

sandwich elements through the core thickness. One integration point is used through the thickness of

each core layer. The length of the local strip model depends on the wavelength of the buckling mode.

Therefore, several local models, with different lengths, are typically analyzed to ensure that the lowest

buckling load is determined. For the thick case, the buckling halfwave length from the full panel models

is 2.5 inches (8 halfwaves along the panel length).

Analytical solution from Brush and Almroth (1975) is obtained from:

Q

f f c f Q c c

cr

b C

D D E t h t C G h r

a

mb

r

mb

a

a

mb

k

b

D P k

2

2

2

2

2

2

( ) 2

1

1 1

 where 

!

!

= + = =

"

"

#

$

%

%

&

' (

)

* +

,

- + +

(

)

* +

,

- +

= =

PANDA2 solutions have also been computed. Face sheet wrinkling using Vinson’s model and general

panel instability buckling are predicted using PANDA2.

Results for two cases are presented. The first case has thin face sheets (each 0.02-inches thick) and a thin

core (0.2-inches thick), and the buckling results are given in Table 13. The general instability buckling

behavior predicted by the STAGS models has two halfwaves in the loading direction and one across the 

panel width – the analytical solution corresponds to three but is very close to the value corresponding to

two halfwaves (within 0.4%). The buckling loads predicted using the layered shell modeling approach are

quite unconservative (~30% higher buckling load) for both the E410 and E480 shell elements when the 

shear correction factors are set to 5/6 because the layered shell model ignores through the thickness

effects. However, when the shear correction factors (SCFs) are computed internally by the STAGS

generic constitutive processor (GCP) if the SCFs are defined as -1 for the GCP shell fabrication input, the 

results obtained using the E480 element in the layered shell model gives very good results. The computed

shear correction factors are reported in the S1 output as 0.0186 and 0.0112 rather than 5/6. The layered

shell/solid and sandwich element modeling approaches give results consistent with the result obtained

using PANDA2. The local strip model predicted short wave length buckling modes with the buckling

load dependent upon the length of the local strip. For a one-inch-long strip, the panel wrinkling

instability load is 260.915 lb. with 20 halfwaves; for a 5.0-in.-long strip, it is 90.442 lb. with 8 halfwaves;

and for a 10.0-in.-long strip, it is 91,376 lb. with 8 halfwaves. Buckling mode shapes for the global and

local models are given in Figure 55. Users need to examine different local strip lengths in order to

account for various wave length buckles. PANDA2 provides insight into this aspect of the modeling.

Hence the global result is the critical buckling load.

The second case has thick face sheets (each 0.11-inches thick) and a thick core (5.5-inches thick), and the

buckling results are given in Table 14. The general short wavelength instability buckling behavior 
156

predicted by the STAGS sandwich element models has eight halfwaves in the loading direction and one 

across the panel width – the analytical solution corresponds to eight as well. Buckling loads predicted

using the layered shell modeling approach are in significant error since these shell elements neglect the 

transverse normal stiffness of the core and the core thickness is quite large (half the panel width). Use of

this modeling approach for this geometry (i.e., hc ≈ a or b) is not appropriate unless three-dimensional

effects are accounted for in the model. The layered shell/solid and sandwich element modeling

approaches give comparable results consistent with the result obtained using PANDA2. The local strip

model (0.1 inches wide) also predicts the short wave length buckling mode shape. For a 1.25-inch-long

strip, the panel wrinkling instability load is 182,652 lb. with 16 halfwaves; for a 2.50-in.-long strip, it is

90,208 lb. with 8 halfwaves; and for a 5.0-in.-long strip, it is 90,442 lb. with 8 halfwaves. Buckling mode

shapes for the global and local models are given in Figure 56. Again the global result is the critical value,

which is also confirmed by the local strip analysis.

Table 13. Sandwich panel buckling results for the thin face sheet, thin core case.

Analysis Type Modeling

Buckling

factor, λ

Critical

Buckling

Load, lb.

Brush & Almroth Analytical --- 13,620

PANDA2 Face Sheet Wrinkling --- 33,400

PANDA2 Panel Buckling --- 12,100

STAGS Layered Shell, E410 0.5276 21,107

STAGS Layered Shell, E480 w/SCF=5/6 0.5221 20,886

STAGS Layered Shell, E480 w/SCF computed 0.3565 14,261

STAGS Layered Shell/Solid, E480/E883 0.3707 14,603

STAGS Sandwich element, E840 0.3709 14,675

STAGS Local strip, E840, 5-inch-long 0.2055 90,442*

*

The buckling load for the local strip model is obtained by computing the critical running load for the local strip

width (0.1 in.) and then multiplying by the panel width (10 in.).

Table 14. Sandwich panel buckling results for the thick face sheet, thick core case.

Analysis Type Modeling

Buckling

factor, λ

Critical

Buckling

Load, lb.

Brush & Almroth Analytical --- 699,656

PANDA2 Face Sheet Wrinkling --- 88,400

PANDA2 Panel Buckling --- 557,000

STAGS Layered Shell/Solid, E480/E883 0.4959 98,486

STAGS Sandwich element, E840 0.4694 94,651

STAGS Local strip, E840, 2.5-inch-long 0.1025 90,208*

*

The buckling load for the local strip model is obtained by computing the critical running load for the local strip

width (0.1 in.) and then multiplying by the panel width (10 in.).
157

(a) Global model result.

(b) Local strip model result.

Figure 55. Buckling results using the sandwich element for the thin face sheets, thin core case.
158

(a) Global model result.

(b) Local strip model result.

Figure 56. Buckling results using the sandwich element for the thick face sheets, thick core case.
159

STAGS Input Files

The modeling strategy for sandwich panels depends on the nature of the structural response that is

anticipated. However, a thorough examination of other possible response patterns needs to be performed.

This strategy is needed due to the nature of the sandwich panel structural response. It may be governing

by overall or general instability buckling mode shapes having a halfwave length on the order of the panel

planar dimensions. These long wavelength mode shapes are easily represented using coarse finite 

element models over the plane of the sandwich panel. Face sheet wrinkling response, on the other hand,

required a refined finite element model because halfwave length of the wrinkling mode (symmetric or

asymmetric) is typically of the order of the sandwich panel thickness. Asymmetric face sheet wrinkling

can be described as a short wave length general instability mode shape that does not cause compression or 

extension of the core material along the panel length. This behave can be captured by full panel finite 

element models that are sufficiently refined (i.e., element size on the order of the sandwich thickness).

Symmetric face sheet wrinkling requires, in addition to a refined planar mesh discretization, through-thethickness effects to be accounted for in the finite element model (i.e., layered shell/solid models or 

sandwich element models). The STAGS input files included herein illustrate the various finite element

modeling approaches. These input files are located under the following subdirectory:

$STAGSHOME/Advanced-Testcases/Type-A-sandwich

with specific modeling approaches given under the appropriate subdirectory as given by: layered-shell;

layered-shell-solid; sandwich-element; and local-strip

Full Panel Layered Shell Model Input Files with E410

In this modeling approach, the sandwich panel is represented by shell elements only. Through-thethickness modeling involves a three-layer laminate (bottom face sheet, core, and top face sheet) definition

of the sandwich. The 4-node displacement-based E410 shell element is used. The E410 element neglect

transverse shear flexibility but does have a cubic C1 bending approximation.

sand410.inp (for S1 processor)

Sandwich panel buckling under compressive loading $ A-1

C

C Layered shell modeling approach using the 410 shell element

C

C Ref. Brush & Almroth, "Buckling of Bars, Plates, and Shells,"

C McGraw-Hill, 1975, pp. 108-112.

C

C a=20 in., b=10 in., simple-supported on all edges

C

0 0 0 0 $ B-1

1 0 0 0 0 0 0 0 0 0 $ B-2

0 0 0 0 0 1 $ B-3

81 21 $ F-1 Planar mesh definition over "a" by "b" panel

$--------------GCP-------------------------------------

ORTHOELAST_MATERIAL 1 1 1 $ core material

100.0 100.0 10.0e3, $ E1, E2, E3

38.4 12.E3 7.2e3, $ G12, G13, G23

0.30 0.01 0.01, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

ORTHOELAST_MATERIAL 2 1 1 $ isotropic face sheet material

10.0E6 10.0e6 10.0E6, $ E1, E2, E3

3.846E6 3.846e6 3.846e6, $ G12, G13, G23

0.30 0.30 0.30, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

C

C Laminate definition of the sandwich structure
160

C

SHELL_FABRICATION 1 3 0 1 0 $i-21 Thin F/S and thin core

2 1 2 $i-21 Facesheet/Core/Facesheet

0.02 0.2 0.02 $i-21 h_fs=0.02 in.; h_core=0.2 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

SHELL_FABRICATION 2 3 0 1 0 $i-21 Thick F/S and thin core

2 1 2 $i-21 Facesheet/Core/Facesheet

0.11 0.2 0.11 $i-21 h_fs=0.11 in.; h_core=0.2 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

SHELL_FABRICATION 3 3 0 1 0 $i-21 Thin F/S and thick core

2 1 2 $i-21 Facesheet/Core/Facesheet

0.02 5.5 0.02 $i-21 h_fs=0.02 in.; h_core=5.5 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

SHELL_FABRICATION 4 3 0 1 0 $i-21 Thick F/S and thick core

2 1 2 $i-21 Facesheet/Core/Facesheet

0.11 5.5 0.11 $i-21 h_fs=0.11 in.; h_core=5.5 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

END

$--------------GCP-------------------------------------

$ Define the shell unit for the rectangular panel

2 0 0 0 0 0 $ M-1 Unit No. 1

0.0 20.0 0.00 10.00 $ M-2 Define Geometry of rectangular plate

-1 $ M-5 layered shell model

410 $ N-1 Select element type

0 0 0 0 $ P-1 Specify BC's on each edge

110 010 $ P-2, w=ru=rw=0 along x=0

110 101 $ P-2, w=rv=0 along y=b

110 010 $ P-2, w=ru=rw=0 along x=a

110 101 $ P-2, w=rv=0 along y=0

1 $ Q-1 Loading system

1 3 $ Q-2 Load system A only; 3 records

-0.1 -1 1 81 0 0 0 0 0 0 0 $ Q-3 Applied end shortening at x=a

+0.1 -1 1 1 0 0 0 0 0 0 0 $ Q-3 Applied end shortening at x=0

+0.0 -1 2 41 11 0 0 0 0 0 0 $ Q-3 Remove rigid body motion; v=0 at center

C+0.0 -1 6 0 0 0 0 0 0 0 0 $ Q-3 RW=0 everywhere for 480 element

1 4*0 1 $ R-1 Output displ. and internal forces

sand410.bin (for S2 processor)

Sandwich panel buckling under compressive loading $ A-1

C *** analysis type definition ***

C indic ipost ilist icor impthe ioptim iflu newent $ b-1

1 1 1 0 0 0 0 -1 $ b-1

C *** load multiplier record ***

C stld(1) step(1) facm(1) stld(2) step(2) facm(2) itemp $ c-1

1.0 0.0 0.0 0.0 0.0 0.0 0 $ c-1

C

C *** eigenvalue control   d-2

C nsec delev iprint ** * d-2

100 .0001 1 $ d-2

C

C **** eigenvalue cluster definition   d-3

C neig shift eiga eigb ** *** d-3

4 0.00 $ d-3

sand410.pin (for STAPL processor)

Sandwich panel studies

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP
161

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -90.0 / 2 0.0 / 3 0.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -90.0 / 2 0.0 / 3 0.0

Full Panel Layered Shell Model Input Files with E480

In this modeling approach, the sandwich panel is represented by shell elements only. Through-thethickness modeling involves a three-layer laminate (bottom face sheet, core, and top face sheet) definition

of the sandwich. The 9-node ANS-based E480 shell element is used since it includes transverse shear 

flexibility. As result, the number of rows and columns defined on the F-1 record must be odd numbers

because the element has three nodes per edge (e.g., a model with three rows and three columns defines

just a single 9-node element). Also, this element does not include drilling freedoms, and hence they must

be suppressed (see the last Q-3 record).

sand480.inp (for S1 processor)

Sandwich panel buckling under compressive loading $ A-1

C

C Layered shell modeling approach using the 480 shell element

C

C Ref. Brush & Almroth, "Buckling of Bars, Plates, and Shells,"

C McGraw-Hill, 1975, pp. 108-112.

C

C a=20 in., b=10 in., simple-supported on all edges

C

0 0 0 0 $ B-1

1 0 0 0 0 0 0 0 0 0 $ B-2

0 0 0 0 0 1 $ B-3

81 21 $ F-1 Planar mesh definition over "a" by "b" panel

$--------------GCP-------------------------------------

ORTHOELAST_MATERIAL 1 1 1 $ core material

100.0 100.0 10.0e3, $ E1, E2, E3

38.4 12.E3 7.2e3, $ G12, G13, G23

0.30 0.01 0.01, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

ORTHOELAST_MATERIAL 2 1 1 $ isotropic face sheet material

10.0E6 10.0e6 10.0E6, $ E1, E2, E3

3.846E6 3.846e6 3.846e6, $ G12, G13, G23

0.30 0.30 0.30, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

C

C Laminate definition of the sandwich structure

C

SHELL_FABRICATION 1 3 0 1 0 $i-21 Thin F/S and thin core
162

2 1 2 $i-21 Facesheet/Core/Facesheet

0.02 0.2 0.02 $i-21 h_fs=0.02 in.; h_core=0.2 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

SHELL_FABRICATION 2 3 0 1 0 $i-21 Thick F/S and thin core

2 1 2 $i-21 Facesheet/Core/Facesheet

0.11 0.2 0.11 $i-21 h_fs=0.11 in.; h_core=0.2 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

SHELL_FABRICATION 3 3 0 1 0 $i-21 Thin F/S and thick core

2 1 2 $i-21 Facesheet/Core/Facesheet

0.02 5.5 0.02 $i-21 h_fs=0.02 in.; h_core=5.5 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

SHELL_FABRICATION 4 3 0 1 0 $i-21 Thick F/S and thick core

2 1 2 $i-21 Facesheet/Core/Facesheet

0.11 5.5 0.11 $i-21 h_fs=0.11 in.; h_core=5.5 in.

3*0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

END

$--------------GCP-------------------------------------

$ Define the shell unit for the rectangular panel

2 0 0 0 0 0 $ M-1 Unit No. 1

0.0 20.0 0.00 10.00 $ M-2 Define Geometry of rectangular plate

-1 $ M-5 layered shell model

480 $ N-1 Select element type

0 0 0 0 $ P-1 Specify BC's on each edge

110 010 $ P-2, w=ru=rw=0 along x=0

110 101 $ P-2, w=rv=0 along y=b

110 010 $ P-2, w=ru=rw=0 along x=a

110 101 $ P-2, w=rv=0 along y=0

1 $ Q-1 Loading system

1 4 $ Q-2 Load system A only; 3 records

-0.1 -1 1 81 0 0 0 0 0 0 0 $ Q-3 Applied end shortening at x=a

+0.1 -1 1 1 0 0 0 0 0 0 0 $ Q-3 Applied end shortening at x=0

+0.0 -1 2 41 11 0 0 0 0 0 0 $ Q-3 Remove rigid body motion; v=0 at center

+0.0 -1 6 0 0 0 0 0 0 0 0 $ Q-3 RW=0 everywhere for 480 element

1 4*0 1 $ R-1 Output displ. and internal forces

Full Panel Layered Shell/Solid Model Input Files

In this modeling approach, the sandwich panel is modeled using shell elements for each face sheet (with

appropriate reference surface eccentricities) and one or more solid elements through the core thickness.

This approach is the layered shell/solid (LSS) approach. Using this approach within STAGS, limits the 

finite element selection to only the E480 shell element with bi-quadratic displacement shape functions

and the E883 solid element with bi-quadratic shape functions on each element face – displacement field

compatibility over the connected face. The finite element model used herein has two solid elements

through the core thickness (one of either side of the middle surface). Two input files are included since 

the input differs for the thin and thick sandwich panel models. Only a single set of the S2 and STAPL

input files are included since they are identical in either case – except for file name, of course.

thinLSS.inp (for S1 processor; thin sandwich case)

Compression-loaded rectangular sandwich panel $A-1

C

C Sandwich panel modeled using the layered shell/solid approach

C with two E883 solid elements through the core thickness

C and the E480 shell elements for the face sheets

C (i.e., five planes of nodes through the sandwich thickness)

C Shell unit 1 = bottom face sheet using E480 9-node shell element

C Shell unit 2 = top face sheet using E480 9-node shell element
163

C Shell unit 3 = core using two E883 27-node bricks through thickness

C

C Ref. Brush & Almroth, "Buckling of Bars, Plates, and Shells,"

C McGraw-Hill, 1975, pp. 108-112.

C

C a=20 in., b=10 in., simple-supported on all edges

C

0 0 0 0 $ B-1

3 0 0 0 0 0 0 0 0 2 $ B-2

1 0 3 0 0 1 $ B-3

81 21 81 21 81 21 $ F-1 Three shell units (2 face sheets & core)

1 0 0 1 0 3 0 0 1 0/ 0 $G-2c/G-2d

2 0 0 1 0 3 0 0 5 0/ 0 $G-2c/G-2d

1 $ I-1 Face-sheet data

10.0E6 0.300 3.85E6 0.100 6.0E-7 10.00E6 1.9439E-5 $ I-2

$--------------GCP-------------------------------------

$ sandwich core,

ORTHOELAST_MATERIAL 1 1 1 $ core material

100.0 100.0 100.0e2, $ E1, E2, E3

38.4 12.0e3 7.2e3, $ G12, G13, G23

0.30 0.01 0.01, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

ORTHOELAST_MATERIAL 2 1 1 $ isotropic face sheet material

10.0E6 10.0e6 10.0E6, $ E1, E2, E3

3.846E6 3.846e6 3.846e6, $ G12, G13, G23

0.30 0.30 0.30, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

C Core definitions - 2 layers across core

SOLID_FABRICATION 1 1 0 0 $ fabid, matid, iang, nipz: thin core

0.10 $ thickness of core element

SOLID_FABRICATION 2 1 0 0 $ fabid, matid, iang, nipz: thick core

2.75 $ thickness of core element

C Face sheet definitions

SHELL_FABRICATION 1 1 0 0 0 $i-21 Thin F/S

2 $i-21 Facesheet material

0.02 $i-21 h_fs=0.02 in.

0.0

SHELL_FABRICATION 2 1 0 0 0 $i-21 Thick F/S

2 $i-21 Facesheet material

0.11 $i-21 h_fs=0.11 in.

0.0

END

$--------------GCP-------------------------------------------------

$----Shell Wall Data using historical STAGS approach --------------

1 1 1 / 1 .020 0.0 $K-1/K-2 Thin face sheet

2 1 1 / 1 .110 0.0 $K-1/K-2 Thick face sheet

3 1 1 / 1 .000 0.0 $K-1/K-2 Phantom face sheet definition

C

C Shell unit to define Bottom Face Sheet

C

2 4 0 0 0 1 $ M-1 Unit No. 1

0.0 20.0 0.00 10.00 $ M-2

0.0 0.0 -0.10 / 3*0.0 $ M-4d/M-4e shift reference plane by -h_c/2

-1 0 0.0 -0.010 0 0 0 $ M-5 Lower Face Sheet with ecz=-t_fs/2

480 $ N-1 Element definition for face sheet

0 0 0 0 $ P-1 Specify BC's on each edge

110 010 $ P-2, w=ru=rw=0 along x=0

110 101 $ P-2, w=rv=0 along y=b

110 010 $ P-2, w=ru=rw=0 along x=a

110 101 $ P-2, w=rv=0 along y=0

1 $ Q-1

1 4 $ Q-2

-.1 -1 1 81 0 0 0 0 0 0 1 $ Q-3 u=-u0 at x=a on face sheet
164

+.1 -1 1 1 0 0 0 0 0 0 1 $ Q-3 u=+u0 at x=0 on face sheet

0.0 -1 2 41 11 0 0 0 0 0 1 $ Q-3 v=0 at center of face sheet

0.0 -1 6 0 0 0 0 0 0 0 1 $ Q-3 RW=0 everywhere (no drilling freedoms)

1 4*0 1 $ R-1

C

C Shell unit to define Upper Face Sheet

C

2 4 0 0 0 1 $ M-1 Unit No. 2

0.0 20.0 0.00 10.00 $ M-2

0.0 0.0 +0.10 / 3*0.0 $ M-4d/M-4e shift reference plane by +h_c/2

-1 0 0.0 +0.010 0 0 0 $ M-5 Lower Face Sheet with ecz=+t_fs/2

480 $ N-1

0 0 0 0 $ P-1 Specify BC's on each edge

110 010 $ P-2, w=ru=rw=0 along x=0

110 101 $ P-2, w=rv=0 along y=b

110 010 $ P-2, w=ru=rw=0 along x=a

110 101 $ P-2, w=rv=0 along y=0

1 $ Q-1

1 4 $ Q-2

-.1 -1 1 81 0 0 0 0 0 0 1 $ Q-3 u=-u0 at x=a on face sheet

+.1 -1 1 1 0 0 0 0 0 0 1 $ Q-3 u=+u0 at x=0 on face sheet

0.0 -1 2 41 11 0 0 0 0 0 1 $ Q-3 v=0 at center of face sheet

0.0 -1 6 0 0 0 0 0 0 0 1 $ Q-3 RW=0 everywhere (no drilling freedoms)

1 4*0 1 $ R-1

C

C Shell unit definition for the core using 2 layers of E883 elements

C

2 0 0 0 2 1 $ M-1 Unit No. 3

0.0 20.0 0.00 10.00 $ M-2

-1 0 0.0 0.0 0 0 0 $ M-5 Core using GCP solid fab.

883 $ N-1 Element definition for core

3 3 3 3 $ P-1 Specify BC's on each edge, solids have no rotations

1 $ Q-1 Loading system

1 21 $ Q-2 Load system A; 21 records for intermediate nodal planes

C impose uniform end shortening

-.1 -1 1 81 0 0 0 0 0 0 2 $ Q-3 u=-u0 at x=a on 2nd nodal plane

+.1 -1 1 1 0 0 0 0 0 0 2 $ Q-3 u=+u0 at x=0 on 2nd nodal plane

-.1 -1 1 81 0 0 0 0 0 0 3 $ Q-3 u=-u0 at x=a on 3rd nodal plane

+.1 -1 1 1 0 0 0 0 0 0 3 $ Q-3 u=+u0 at x=0 on 3rd nodal plane

-.1 -1 1 81 0 0 0 0 0 0 4 $ Q-3 u=-u0 at x=a on 4th nodal plane

+.1 -1 1 1 0 0 0 0 0 0 4 $ Q-3 u=+u0 at x=0 on 4th nodal plane

C impose w=0 along edges

0. -1 3 1 0 0 0 0 0 0 2 $ Q-3 w=0 at x = 0, layer 2

0. -1 3 1 0 0 0 0 0 0 3 $ Q-3 w=0 at x = 0, layer 3

0. -1 3 1 0 0 0 0 0 0 4 $ Q-3 w=0 at x = 0, layer 4

0. -1 3 81 0 0 0 0 0 0 2 $ Q-3 w=0 at x = a, layer 2

0. -1 3 81 0 0 0 0 0 0 3 $ Q-3 w=0 at x = a, layer 3

0. -1 3 81 0 0 0 0 0 0 4 $ Q-3 w=0 at x = a, layer 4

0. -1 3 0 1 0 0 0 0 0 2 $ Q-3 w=0 at y = 0, layer 2

0. -1 3 0 1 0 0 0 0 0 3 $ Q-3 w=0 at y = 0, layer 3

0. -1 3 0 1 0 0 0 0 0 4 $ Q-3 w=0 at y = 0, layer 4

0. -1 3 0 21 0 0 0 0 0 2 $ Q-3 w=0 at y = b, layer 2

0. -1 3 0 21 0 0 0 0 0 3 $ Q-3 w=0 at y = b, layer 3

0. -1 3 0 21 0 0 0 0 0 4 $ Q-3 w=0 at y = b, layer 4

0.0 -1 2 41 11 0 0 0 0 0 2 $ Q-3 v=0 at center of layer 2

0.0 -1 2 41 11 0 0 0 0 0 3 $ Q-3 v=0 at center of layer 3

0.0 -1 2 41 11 0 0 0 0 0 4 $ Q-3 v=0 at center of layer 4

1 4*0 1 $ R-1 Print displacements and internal forces

thickLSS.inp (for S1 processor; thick sandwich case)

Compression-loaded rectangular sandwich panel $A-1
165

C

C Sandwich panel modeled using the layered shell/solid approach

C with two E883 solid elements through the core thickness

C and the E480 shell elements for the face sheets

C (i.e., five planes of nodes through the sandwich thickness)

C Shell unit 1 = bottom face sheet using E480 9-node shell element

C Shell unit 2 = top face sheet using E480 9-node shell element

C Shell unit 3 = core using two E883 27-node bricks through thickness

C

C Ref. Brush & Almroth, "Buckling of Bars, Plates, and Shells,"

C McGraw-Hill, 1975, pp. 108-112.

C

C a=20 in., b=10 in., simple-supported on all edges

C

0 0 0 0 $ B-1

3 0 0 0 0 0 0 0 0 2 $ B-2

1 0 3 0 0 1 $ B-3

81 21 81 21 81 21 $ F-1 Three shell units (2 face sheets & core)

1 0 0 1 0 3 0 0 1 0/ 0 $G-2c/G-2d

2 0 0 1 0 3 0 0 5 0/ 0 $G-2c/G-2d

1 $ I-1 Face-sheet data

10.0E6 0.300 3.85E6 0.100 6.0E-7 10.00E6 1.9439E-5 $ I-2

$--------------GCP-------------------------------------

$ sandwich core,

ORTHOELAST_MATERIAL 1 1 1 $ core material

100.0 100.0 100.0e2, $ E1, E2, E3

38.4 12.0e3 7.2e3, $ G12, G13, G23

0.30 0.01 0.01, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

ORTHOELAST_MATERIAL 2 1 1 $ isotropic face sheet material

10.0E6 10.0e6 10.0E6, $ E1, E2, E3

3.846E6 3.846e6 3.846e6, $ G12, G13, G23

0.30 0.30 0.30, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

C Core definitions - 2 layers across core

SOLID_FABRICATION 1 1 0 0 $ fabid, matid, iang, nipz: thin core

0.10 $ thickness of core element

SOLID_FABRICATION 2 1 0 0 $ fabid, matid, iang, nipz: thick core

2.75 $ thickness of core element

C Face sheet definitions

SHELL_FABRICATION 1 1 0 1 0 $i-21 Thin F/S

2 $i-21 Facesheet material

0.02 $i-21 h_fs=0.02 in.

0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

SHELL_FABRICATION 2 1 0 1 0 $i-21 Thick F/S

2 $i-21 Facesheet material

0.11 $i-21 h_fs=0.11 in.

0.0

0.83333 0.83333 $i-21 shear correction factors, 5/6

END

$--------------GCP-------------------------------------------------

$----Shell Wall Data using historical STAGS approach --------------

1 1 1 / 1 .020 0.0 $K-1/K-2 Thin face sheet

2 1 1 / 1 .110 0.0 $K-1/K-2 Thick face sheet

3 1 1 / 1 .000 0.0 $K-1/K-2 Phantom face sheet definition

C

C Shell unit to define Bottom Face Sheet

C

2 4 0 0 0 1 $ M-1 Unit No. 1

0.0 20.0 0.00 10.00 $ M-2

0.0 0.0 -2.75 / 3*0.0 $ M-4d/M-4e shift reference plane by -h_c/2

-2 0 0.0 -0.055 0 0 0 $ M-5 Lower Face Sheet with ecz=-t_fs/2
166

480 $ N-1 Element definition for face sheet

0 0 0 0 $ P-1 Specify BC's on each edge

110 010 $ P-2, w=ru=rw=0 along x=0

110 101 $ P-2, w=rv=0 along y=b

110 010 $ P-2, w=ru=rw=0 along x=a

110 101 $ P-2, w=rv=0 along y=0

1 $ Q-1

1 4 $ Q-2

-.1 -1 1 81 0 0 0 0 0 0 1 $ Q-3 u=-u0 at x=a on face sheet

+.1 -1 1 1 0 0 0 0 0 0 1 $ Q-3 u=+u0 at x=0 on face sheet

0.0 -1 2 41 11 0 0 0 0 0 1 $ Q-3 v=0 at center of face sheet

0.0 -1 6 0 0 0 0 0 0 0 1 $ Q-3 RW=0 everywhere (no drilling freedoms)

1 4*0 1 $ R-1

C

C Shell unit to define Upper Face Sheet

C

2 4 0 0 0 1 $ M-1 Unit No. 2

0.0 20.0 0.00 10.00 $ M-2

0.0 0.0 +2.75 / 3*0.0 $ M-4d/M-4e shift reference plane by +h_c/2

-2 0 0.0 +0.055 0 0 0 $ M-5 Lower Face Sheet with ecz=+t_fs/2

480 $ N-1

0 0 0 0 $ P-1 Specify BC's on each edge

110 010 $ P-2, w=ru=rw=0 along x=0

110 101 $ P-2, w=rv=0 along y=b

110 010 $ P-2, w=ru=rw=0 along x=a

110 101 $ P-2, w=rv=0 along y=0

1 $ Q-1

1 4 $ Q-2

-.1 -1 1 81 0 0 0 0 0 0 1 $ Q-3 u=-u0 at x=a on face sheet

+.1 -1 1 1 0 0 0 0 0 0 1 $ Q-3 u=+u0 at x=0 on face sheet

0.0 -1 2 41 11 0 0 0 0 0 1 $ Q-3 v=0 at center of face sheet

0.0 -1 6 0 0 0 0 0 0 0 1 $ Q-3 RW=0 everywhere (no drilling freedoms)

1 4*0 1 $ R-1

C

C Shell unit definition for the core using 2 layers of E883 elements

C

2 0 0 0 2 1 $ M-1 Unit No. 3

0.0 20.0 0.00 10.00 $ M-2

-2 0 0.0 0.0 0 0 0 $ M-5 Core using GCP solid fab.

883 $ N-1 Element definition for core

3 3 3 3 $ P-1 Specify BC's on each edge, solids have no rotations

1 $ Q-1 Loading system

1 21 $ Q-2 Load system A; 21 records for intermediate nodal planes

C impose uniform end shortening

-.1 -1 1 81 0 0 0 0 0 0 2 $ Q-3 u=-u0 at x=a on 2nd nodal plane

+.1 -1 1 1 0 0 0 0 0 0 2 $ Q-3 u=+u0 at x=0 on 2nd nodal plane

-.1 -1 1 81 0 0 0 0 0 0 3 $ Q-3 u=-u0 at x=a on 3rd nodal plane

+.1 -1 1 1 0 0 0 0 0 0 3 $ Q-3 u=+u0 at x=0 on 3rd nodal plane

-.1 -1 1 81 0 0 0 0 0 0 4 $ Q-3 u=-u0 at x=a on 4th nodal plane

+.1 -1 1 1 0 0 0 0 0 0 4 $ Q-3 u=+u0 at x=0 on 4th nodal plane

C impose w=0 along edges

0. -1 3 1 0 0 0 0 0 0 2 $ Q-3 w=0 at x = 0, layer 2

0. -1 3 1 0 0 0 0 0 0 3 $ Q-3 w=0 at x = 0, layer 3

0. -1 3 1 0 0 0 0 0 0 4 $ Q-3 w=0 at x = 0, layer 4

0. -1 3 81 0 0 0 0 0 0 2 $ Q-3 w=0 at x = a, layer 2

0. -1 3 81 0 0 0 0 0 0 3 $ Q-3 w=0 at x = a, layer 3

0. -1 3 81 0 0 0 0 0 0 4 $ Q-3 w=0 at x = a, layer 4

0. -1 3 0 1 0 0 0 0 0 2 $ Q-3 w=0 at y = 0, layer 2

0. -1 3 0 1 0 0 0 0 0 3 $ Q-3 w=0 at y = 0, layer 3

0. -1 3 0 1 0 0 0 0 0 4 $ Q-3 w=0 at y = 0, layer 4

0. -1 3 0 21 0 0 0 0 0 2 $ Q-3 w=0 at y = b, layer 2

0. -1 3 0 21 0 0 0 0 0 3 $ Q-3 w=0 at y = b, layer 3

0. -1 3 0 21 0 0 0 0 0 4 $ Q-3 w=0 at y = b, layer 4
167

0.0 -1 2 41 11 0 0 0 0 0 2 $ Q-3 v=0 at center of layer 2

0.0 -1 2 41 11 0 0 0 0 0 3 $ Q-3 v=0 at center of layer 3

0.0 -1 2 41 11 0 0 0 0 0 4 $ Q-3 v=0 at center of layer 4

1 4*0 1 $ R-1 Print displacements and internal forces

thickLSS.bin (for S2 processor; thick sandwich case)

Sandwich panel buckling under compressive loading $ A-1

C *** analysis type definition ***

C indic ipost ilist icor impthe ioptim iflu newent $ b-1

1 1 0 0 0 0 0 -1 $ b-1

C *** load multiplier record ***

C stld(1) step(1) facm(1) stld(2) step(2) facm(2) itemp $ c-1

1.0 0.0 0.0 0.0 0.0 0.0 0 $ c-1

C

C *** eigenvalue control   d-2

C nsec delev iprint ** * d-2

2000 .0001 0 $ d-2

C

C **** eigenvalue cluster definition   d-3

C neig shift eiga eigb ** *** d-3

4 0.0 $ d-3

thickLSS.pin (for STAPL processor; thick sandwich case)

Sandwich panel studies

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -90.0 / 2 0.0 / 3 0.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -90.0 / 2 0.0 / 3 0.0

Full Panel Sandwich Model Input Files

In this modeling approach, the sandwich panel is modeled using one or more sandwich elements through

the thickness of the sandwich panel. If multiple sandwich elements are used through the thickness, the 

intermediate face sheets are “phantom face sheets” having zero thickness and are only used for modeling

purposes through the core thickness. A piecewise linear approximation can thereby be represented. The 

STAGS sandwich element denoted by E840 exploits the E410 shell element for the face sheet response as

well as for the core deformations. This finite element model has twice the number of elements over the 

surface of the panel compared to models using the 9-node E480 elements – the number of nodes on each

plane is the same for the two element types.
168

The finite element model used herein has two sandwich elements through the core thickness (one of either

side of the middle surface). This gives one “phantom face sheet” with zero thickness at the middle 

surface of the sandwich panel. Users also may select the number of the through-the-thickness integration

points (one or two). Depending on the sandwich panel thickness and the structural response for the

specified loading, spurious zero-energy mechanisms, stemming from the E840 dependence on the E410

shell element, may occur that can be suppressed by increasing the number of through-the-thickness

integration points or increasing the through-the-thickness discretization (more sandwich elements). The 

reference surface is the middle of the sandwich panel.

sandwich2.inp (for S1 processor)

Compression-loaded rectangular sandwich panel $A-1

C

C Sandwich panel modeled using the E840 sandwich element

C with two elements through the core thickness (i.e., three

C planes of nodes)

C

C Ref. Brush & Almroth, "Buckling of Bars, Plates, and Shells,"

C McGraw-Hill, 1975, pp. 108-112.

C

C a=20 in., b=10 in., simple-supported on all edges

C

0 0 0 0 $ B-1

1 0 0 0 0 0 0 0 0 0 $ B-2

1 0 3 0 0 1 $ B-3

81 21 $ F-1 Planar mesh definition over "a" by "b" panel

1 $ I-1 Face-sheet data using historical STAGS approach

10.0E6 0.300 3.85E6 0.100 6.0E-7 10.00E6 1.9439E-5 $ I-2

$--------------GCP-------------------------------------

$ Homogeneous core

ORTHOELAST_MATERIAL 1 1 1 $ core material

100.0 100.0 100.0E2, $ E1, E2, E3

38.4 12.0E3 7.2E3, $ G12, G13, G23

0.30 0.01 0.01, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

ORTHOELAST_MATERIAL 2 1 1 $ isotropic face sheet material

10.0E6 10.0e6 10.0E6, $ E1, E2, E3

3.846E6 3.846e6 3.846e6, $ G12, G13, G23

0.30 0.30 0.30, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces

C Core definitions - 2 layers across core

SOLID_FABRICATION 1 1 0 1 $ fabid, matid, iang, nipz: thin core

0.10 $ thickness of core element

SOLID_FABRICATION 2 1 0 1 $ fabid, matid, iang, nipz: thick core

2.75 $ thickness of core element

C Face sheet definitions

SHELL_FABRICATION 1 1 0 0 0 $i-21 Thin F/S

2 $i-21 Facesheet material

0.02 $i-21 h_fs=0.02 in.

0.0

SHELL_FABRICATION 2 1 0 0 0 $i-21 Thick F/S

2 $i-21 Facesheet material

0.11 $i-21 h_fs=0.11 in.

0.0

SHELL_FABRICATION 3 1 0 0 0 $i-21 Phantom F/S

2 $i-21 Facesheet material

0.0 $i-21 h_fs=0.0

0.0

END

$--------------GCP------------------------------------------------

$----Shell Wall Data using historical STAGS approach--------------

1 1 1 / 1 .020 0.0 $K-1/K-2 Thin face sheet
169

2 1 1 / 1 .110 0.0 $K-1/K-2 Thick face sheet

3 1 1 / 1 .000 0.0 $K-1/K-2 Phantom face sheet definition

$ Define the shell unit for the rectangular sandwich panel

2 0 0 0 2 5 $ M-1 Unit No. 1 - two layers of sandwich elements

0.0 20.0 0.00 10.00 $ M-2

-2 0 0.0 0.0 0 0 0 $ M-5 Bottom Face Sheet - GCP shell fab.

-2 0 0.0 0.0 0 0 0 $ M-5 First core element - GCP solid fab.

-2 0 0.0 0.0 0 0 0 $ M-5 Second core element - GCP solid fab.

-2 0 0.0 0.0 0 0 0 $ M-5 Top Face Sheet - GCP shell fab.

-3 0 0.0 0.0 0 0 0 $ M-5 Phantom Face Sheet - GCP shell fab.

840 $ N-1 Selement element type

3 3 3 3 $ P-1 Specify BC's on each edge using Q records

1 $ Q-1 Loading system

1 39 $ Q-2 Load system A; 39 records

+0.1 -1 1 1 0 0 0 0 0 0 1 $ Q-3 u=+u0 at x=0 in bottom face sheet

+0.1 -1 1 1 0 0 0 0 0 0 2 $ Q-3 u=+u0 at x=0 in phantom face sheet

+0.1 -1 1 1 0 0 0 0 0 0 3 $ Q-3 u=+u0 at x=0 in top face sheet

-0.1 -1 1 81 0 0 0 0 0 0 1 $ Q-3 u=-u0 at x=a in bottom face sheet

-0.1 -1 1 81 0 0 0 0 0 0 2 $ Q-3 u=-u0 at x=a in phantom face sheet

-0.1 -1 1 81 0 0 0 0 0 0 3 $ Q-3 u=-u0 at x=a in top face sheet

C w=rx=rz=0 on x=0 edge

0.0 -1 3 1 0 0 0 0 0 0 1 $ Q-3 w=0 at x=0 in bottom face sheet

0.0 -1 4 1 0 0 0 0 0 0 1 $ Q-3 rx=0 at x=0 in bottom face sheet

0.0 -1 6 1 0 0 0 0 0 0 1 $ Q-3 rz=0 at x=0 in bottom face sheet

0.0 -1 3 1 0 0 0 0 0 0 2 $ Q-3 w=0 at x=0 in phantom face sheet

0.0 -1 4 1 0 0 0 0 0 0 2 $ Q-3 rx=0 at x=0 in phantom face sheet

0.0 -1 6 1 0 0 0 0 0 0 2 $ Q-3 rz=0 at x=0 in phantom face sheet

0.0 -1 3 1 0 0 0 0 0 0 3 $ Q-3 w=0 at x=0 in top face sheet

0.0 -1 4 1 0 0 0 0 0 0 3 $ Q-3 rx=0 at x=0 in top face sheet

0.0 -1 6 1 0 0 0 0 0 0 3 $ Q-3 rz=0 at x=0 in top face sheet

C w=rx=rz=0 on x=a edge

0.0 -1 3 81 0 0 0 0 0 0 1 $ Q-3 w=0 at x=a in bottom face sheet

0.0 -1 4 81 0 0 0 0 0 0 1 $ Q-3 rx=0 at x=a in bottom face sheet

0.0 -1 6 81 0 0 0 0 0 0 1 $ Q-3 rz=0 at x=a in bottom face sheet

0.0 -1 3 81 0 0 0 0 0 0 2 $ Q-3 w=0 at x=a in phantom face sheet

0.0 -1 4 81 0 0 0 0 0 0 2 $ Q-3 rx=0 at x=a in phantom face sheet

0.0 -1 6 81 0 0 0 0 0 0 2 $ Q-3 rz=0 at x=a in phantom face sheet

0.0 -1 3 81 0 0 0 0 0 0 3 $ Q-3 w=0 at x=a in top face sheet

0.0 -1 4 81 0 0 0 0 0 0 3 $ Q-3 rx=0 at x=a in top face sheet

0.0 -1 6 81 0 0 0 0 0 0 3 $ Q-3 rz=0 at x=a in top face sheet

C w=ry=0 on y=0 edge

0.0 -1 3 0 1 0 0 0 0 0 1 $ Q-3 w=0 at y=0 in bottom face sheet

0.0 -1 5 0 1 0 0 0 0 0 1 $ Q-3 ry=0 at y=0 in bottom face sheet

0.0 -1 3 0 1 0 0 0 0 0 2 $ Q-3 w=0 at y=0 in phantom face sheet

0.0 -1 5 0 1 0 0 0 0 0 2 $ Q-3 ry=0 at y=0 in phantom face sheet

0.0 -1 3 0 1 0 0 0 0 0 3 $ Q-3 w=0 at y=0 in top face sheet

0.0 -1 5 0 1 0 0 0 0 0 3 $ Q-3 ry=0 at y=0 in top face sheet

C w=ry=0 on y=b edge

0.0 -1 3 0 21 0 0 0 0 0 1 $ Q-3 w=0 at y=b in bottom face sheet

0.0 -1 5 0 21 0 0 0 0 0 1 $ Q-3 ry=0 at y=b in bottom face sheet

0.0 -1 3 0 21 0 0 0 0 0 2 $ Q-3 w=0 at y=b in phantom face sheet

0.0 -1 5 0 21 0 0 0 0 0 2 $ Q-3 ry=0 at y=b in phantom face sheet

0.0 -1 3 0 21 0 0 0 0 0 3 $ Q-3 w=0 at y=b in top face sheet

0.0 -1 5 0 21 0 0 0 0 0 3 $ Q-3 ry=0 at y=b in top face sheet

C v=0 at center of nodal plane

0.0 -1 2 41 11 0 0 0 0 0 1 $ Q-3 v=0 at center in bottom face sheet

0.0 -1 2 41 11 0 0 0 0 0 2 $ Q-3 v=0 at center in phantom face sheet

0.0 -1 2 41 11 0 0 0 0 0 3 $ Q-3 v=0 at center in top face sheet

1 4*0 1 $ R-1 Print displacements and internal forces
170

sandwich2.bin (for S2 processor)

Sandwich panel buckling under compressive loading $ A-1

C *** analysis type definition ***

C indic ipost ilist icor impthe ioptim iflu newent $ b-1

1 1 0 0 0 0 0 -1 $ b-1

C *** load multiplier record ***

C stld(1) step(1) facm(1) stld(2) step(2) facm(2) itemp $ c-1

1.0 0.0 0.0 0.0 0.0 0.0 0 $ c-1

C

C *** eigenvalue control   d-2

C nsec delev iprint ** * d-2

1000 .0001 0 $ d-2

C

C **** eigenvalue cluster definition   d-3

C neig shift eiga eigb ** *** d-3

4 0.0 $ d-3

sandwich2.pin (for STAPL processor)

Sandwich panel studies

4 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

Local Strip Sandwich Model Input Files

In this modeling approach, a local strip of the sandwich panel is modeled using many sandwich elements

through the thickness of the sandwich panel. The intermediate face sheets are “phantom face sheets”

having zero thickness and are only used for modeling purposes through the core thickness. A piecewise

linear approximation results from layer to layer. The local strip is very narrow compared to the panel

width, and its length is typically less than the panel length. Care must be taken in choosing the local strip

length so that the lowest buckling load is captured. That is, the length of the local strip should be a 

multiple of the buckling mode shape halfwave length corresponding to the lowest buckling load. It may

be necessary to examine more than one local strip length.

strip.inp (for S1 processor)

Local Strip Model of compression-loaded rectangular sandwich panel $A-1

C

C Local strip model with 25 layers through the thickness

C (strip length=2.5 in., strip width=0.1 in. based on

C full panel model which gave 8 halfwaves along length;

C so if more than 1 halfwave in local strip then local

C buckling may occur if buckling load below full panel

C buckling load).

C

C Ref. Brush & Almroth, "Buckling of Bars, Plates, and Shells,"

C McGraw-Hill, 1975, pp. 108-112.

C

C a=20 in., b=10 in., simple-supported on all edges

C

0 0 0 0 $ B-1

1 8*0 1 $ B-2

1 0 3 0 0 1 $ B-3
171

21 2 $ F-1

1 1 1 1 2 1 0 1 1 2/ 26 5*0 3*0 1 0 $G-2c/G-2d

C

C face sheet material data using historical STAGS approach

C

1 $ I-1 Face-sheet data

10.0E6 0.300 3.85E6 0.100 6.0E-7 10.00E6 1.9439E-5 $ I-2

$--------------GCP-------------------------------------

$ Homogeneous core

ORTHOELAST_MATERIAL 1 1 1 $ core material

100.0 100.0 100.0E2, $ E1, E2, E3

38.4 12.0E3 7.2E3, $ G12, G13, G23

0.30 0.01 0.01, $ P12, P13, P23

0. 0. 0. 0. 0. 0. 0. 0. 0. $ Filler spaces (unused)

SOLID_FABRICATION 1 1 0 1 $ fabid & matid for core material - thick case

.22000 $ element thickness (5.5 in./25 ele.=0.22 in.)

SOLID_FABRICATION 2 1 0 1 $ fabid & matid for core material - thin case

.00800 $ element thickness (0.2 in./25 ele.=0.008 in.)

END

$--------------GCP-------------------------------------

$----Shell Wall Data using historical STAGS approach --------------

1 1 1 / 1 .110 0.0 $K-1/K-2 Face sheet thickness

2 1 1 / 1 .020 0.0 $K-1/K-2 Face sheet thickness

3 1 1 / 1 0. $K-1/K-2 Phantom face sheet

C

C Local strip model (2.5 in. long by 0.1 inches wide)

C

2 0 0 0 25 28 $ M-1 Unit No. 1

0.0 1.25 0.00 .100 $ M-2

+1 0 0.0 0.0 0 0 0 $ M-5 Bottom Face Sheet

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 1

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 2

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 3

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 4

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 5

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 6

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 7

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 8

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 9

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 10

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 11

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 12

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 13

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 14

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 15

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 16

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 17

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 18

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 19

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 20

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 21

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 22

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 23

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 24

-1 0 0.0 0.0 0 0 0 $ M-5 Core element 25

+1 0 0.0 0.0 0 0 0 $ M-5 Top Face Sheet

+3 0 0.0 0.0 0 0 0 $ M-5 Phantom face sheets

840 4*0 0 $ N-1

0 4 4 0 $ P-1

111 100 $ P-2 Edge at x=0

111 010 $ P-2 Edge at y=0

1 $ Q-1 Loading system

1 27 $ Q-2 Load system A; 27 records
172

0.1 -1 1 1 0 0 0 0 0 0 1 $ Q-3 u=u0 along edge at x=0 on nodal plane 1

0.1 -1 1 1 0 0 0 0 0 0 2 $ Q-3 u=u0 along edge at x=0 on nodal plane 2

0.1 -1 1 1 0 0 0 0 0 0 3 $ Q-3 u=u0 along edge at x=0 on nodal plane 3

0.1 -1 1 1 0 0 0 0 0 0 4 $ Q-3 u=u0 along edge at x=0 on nodal plane 4

0.1 -1 1 1 0 0 0 0 0 0 5 $ Q-3 u=u0 along edge at x=0 on nodal plane 5

0.1 -1 1 1 0 0 0 0 0 0 6 $ Q-3 u=u0 along edge at x=0 on nodal plane 6

0.1 -1 1 1 0 0 0 0 0 0 7 $ Q-3 u=u0 along edge at x=0 on nodal plane 7

0.1 -1 1 1 0 0 0 0 0 0 8 $ Q-3 u=u0 along edge at x=0 on nodal plane 8

0.1 -1 1 1 0 0 0 0 0 0 9 $ Q-3 u=u0 along edge at x=0 on nodal plane 9

0.1 -1 1 1 0 0 0 0 0 0 10 $ Q-3 u=u0 along edge at x=0 on nodal plane 10

0.1 -1 1 1 0 0 0 0 0 0 11 $ Q-3 u=u0 along edge at x=0 on nodal plane 11

0.1 -1 1 1 0 0 0 0 0 0 12 $ Q-3 u=u0 along edge at x=0 on nodal plane 12

0.1 -1 1 1 0 0 0 0 0 0 13 $ Q-3 u=u0 along edge at x=0 on nodal plane 13

0.1 -1 1 1 0 0 0 0 0 0 14 $ Q-3 u=u0 along edge at x=0 on nodal plane 14

0.1 -1 1 1 0 0 0 0 0 0 15 $ Q-3 u=u0 along edge at x=0 on nodal plane 15

0.1 -1 1 1 0 0 0 0 0 0 16 $ Q-3 u=u0 along edge at x=0 on nodal plane 16

0.1 -1 1 1 0 0 0 0 0 0 17 $ Q-3 u=u0 along edge at x=0 on nodal plane 17

0.1 -1 1 1 0 0 0 0 0 0 18 $ Q-3 u=u0 along edge at x=0 on nodal plane 18

0.1 -1 1 1 0 0 0 0 0 0 19 $ Q-3 u=u0 along edge at x=0 on nodal plane 19

0.1 -1 1 1 0 0 0 0 0 0 20 $ Q-3 u=u0 along edge at x=0 on nodal plane 20

0.1 -1 1 1 0 0 0 0 0 0 21 $ Q-3 u=u0 along edge at x=0 on nodal plane 21

0.1 -1 1 1 0 0 0 0 0 0 22 $ Q-3 u=u0 along edge at x=0 on nodal plane 22

0.1 -1 1 1 0 0 0 0 0 0 23 $ Q-3 u=u0 along edge at x=0 on nodal plane 23

0.1 -1 1 1 0 0 0 0 0 0 24 $ Q-3 u=u0 along edge at x=0 on nodal plane 24

0.1 -1 1 1 0 0 0 0 0 0 25 $ Q-3 u=u0 along edge at x=0 on nodal plane 25

0.1 -1 1 1 0 0 0 0 0 0 26 $ Q-3 u=u0 along edge at x=0 on nodal plane 26

0.0 -1 3 1 1 0 0 0 0 0 1 $ Q-3 w=0 at point to remove rigid body motion

1 4*0 1 $ R-1

strip.bin (for S2 processor)

Sandwich panel buckling under compressive loading - local strip $ A-1

C *** analysis type definition ***

C indic ipost ilist icor impthe ioptim iflu newent $ b-1

1 1 1 0 0 0 0 -1 $ b-1

C *** load multiplier record ***

C stld(1) step(1) facm(1) stld(2) step(2) facm(2) itemp $ c-1

1.0 0.0 0.0 0.0 0.0 0.0 0 $ c-1

C

C *** eigenvalue control   d-2

C nsec delev iprint ** * d-2

100 .0001 1 $ d-2

C

C **** eigenvalue cluster definition   d-3

C neig shift eiga eigb ** *** d-3

4 0.0 $ d-3

strip.pin (for STAPL processor)

Local Strip model of sandwich panel (25 layers) $A-1

2 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -90.0 /2 0.0 / 3 0.0

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -64.0 /2 -4.0 / 3 -135.0
173

Problem References

Brush, D. O. and Almroth, B. O., Buckling of Bars, Plates, and Shells, McGraw-Hill Book Company,

New York, 1975.

Bushnell, D., “Optimum Design via PANDA2 of Composite Sandwich Panels with Honeycomb or Foam 

Cores,” AIAA Paper No. 97-1142, April 1997.

Riks, E. and Rankin, C. C., “Sandwich Modeling with an Application to the Residual Strength Analysis

of a Damaged Composite Compression Panel,” AIAA Paper No. 2001-1323, April 2001.

Riks, E. and Rankin, C. C., “Sandwich Modeling with an Application to the Residual Strength Analysis

of a Damaged Compression Panel,” International Journal of Non-Linear Mechanics, Vol. 37, Nos. 4-5,

June-July 2002, pp. 897-908.

Rose, C. A., Moore, D. F., Knight, N. F., Jr., and Rankin, C. C., “Finite Element Modeling of the

Buckling Response of Sandwich Panels,” AIAA Paper No. 2002-1517, April 2002.
174

Crack Growth Simulation for Middle-Crack Tension Panel

Background

An isotropic linear elastic panel with a center through-crack loaded in tension (M(T) panel) is a common

analysis problem in fracture mechanics applications. The geometry is a standard configuration used in

material testing and validation of computational methods (e.g., Riks et al., 1992; Dawicke et al., 1994,

Viz et al., 1995; Dawicke, 1997; Seshadri and Newman, 1998; Seshadri et al., 1998; Gullerud et al.,

1999; Rankin and Riks, 2000, 2001). The total panel length is 2L, the total panel width is 2w, and the

initial total crack length is 2a. The initial crack is located at x=L and is centered about the line y=0. The

geometry and material properties of the problem are defined in Figure 57 using U.S. customary units and

SI units and represent a test configuration of Dawicke (1997).

Figure 57. Center-crack panel problem: geometry and material properties.

Geometry:

2L = 24.0 in. = 609.6 mm

2w = 12.0 in. = 304.8 mm

2a = 4.0 in. = 101.6 mm

Panel Material:

E = 10.356 Msi = 71.400 GPa

ν = 0.3

2a

w w

L

δ

y

x

L
175

Modeling and Analysis Process

The finite element model represents half the width and the full length of the panel even though quarter 

symmetry could have been used. While the rectangular panel can easily be modeled with a single shell

unit, multiple shell units are used in order to refine the finite element mesh near the crack at panel

midlength. The overall finite element model is shown in Figure 58 with inset figures showing the model

near the crack (shell unit 5) for the shell-element and solid-element models. The inset figures represent

the linear solution under a small load level so that the crack location can be viewed.
176

Figure 58. Overall finite element model and close-up views near the crack.

(b) Close-up view of center-crack

region modeled using shell elements.

(a) Overview of center-crack panel

using a shell element model.

(c) Close-up view of center-crack

region modeled using solid elements.

Symmetry Edge

Free

Edge

Applied End

Extension

Clamped Edge
177

Table 15. Stress-strain data for 2024-T3 (LT) aluminum alloy.

Strain, ε

(in./in.)

Stress, σ

(MPa)

Stress, σ

(psi)

0.0 0 0

0.00483 345 50,000

0.15 390 56,600

0.4 430 62,300

0.1 470 68,200

0.16 491 71,200

Material properties and shell wall construction are defined using the GCP approach.. Material modeling

using the current GCP approach requires data on the I-5a and I-6a records to define the material

properties and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the shell fabrication. The

elastic-plastic stress-strain curve for 2024-T3 (LT) aluminum alloy (0.09-inches or 2.3-mm thick) is

defined for the White-Besseling plasticity model in STAGS using the values given in Table 15. Note that

STAGS does not require (or allow) the origin of the stress-strain curve to be defined – it is implicitly

assumed.

From this data, the elastic modulus E of the material is 10.35197 Msi (71.400 GPa) and Poisson’s ratio ν

is taken as 0.3. STAGS compares the computed value of the elastic modulus from the first nonzero pair 

of stress-strain values with the input modulus value on the I-2 record (or appropriate GCP record). The

ratio of this difference and the elastic modulus read as input must be less than 10-6 or STAGS will stop.

The yield stress is 50,000 psi or 345 MPa, and the ultimate stress is 71,200 psi or 491 MPa. The stressstrain curve is treated as a piecewise linear curve using table-lookup in STAGS with linear interpolation

for values between data points. In the finite element model, shell units 4, 5, and 6 (i.e., the center two

inches of the model) use the elasto-plastic material definition while the other shell units use only the 

elastic properties.

Boundary condition on the displacements are specified using the P-1 and P-2 records. An applied end

displacement is specified across edge 1 on shell unit 1. Because of the coordinate system used,

extensional end displacements have a negative value. The opposite end of the panel is clamped, the right

edge of the finite element model is free, and the left edge has symmetric conditions imposed. Even

though the degrees of freedom associated with interior nodes are unrestrained, a nonlinear analysis will

not automatically lead to out-of-plane deflections (local buckling) near the crack unless an initial

geometric surface imperfection is used to “trigger” the nonlinear effects. The initial geometric

imperfection can be generated by first performing a buckling calculation and then using the mode shape 

corresponding to the lowest eigenvalue scaled by a small number (e.g., 1% of panel thickness) as the

initial imperfection. Such a buckling-mode-based imperfection is defined using the B-6 record.

Mesh refinement using shell transition elements (E510 and E710) is performed automatically across shell

unit boundaries. In the present case, there are four shell units on either side of a center shell unit since the

entire panel length is modeled as shown in Figure 58. The element size in the width direction is cut in

half in each shell unit as the center shell unit is approached. The element width is 0.5 inches in shell unit

1, 0.25 inches in shell unit 2, 0.125 inches in shell unit 3, and 0.0625 inches in shell unit 4. The element

width in the center shell unit is held at 0.0625 inches. This level of mesh refinement gives 96 elements

across the half width of the panel.
178

Transition from shell elements to solid elements is defined using several STAGS input records. In this

discussion (and in the example case provided), the shell-to-solid transition occurs along shell unit

boundaries. In the crack1sm.inp file, shell units 4 and 6 are modeled using E410 shell elements,

while shell unit 5 is modeled using four layers of E881 solid elements through the thickness of the panel.

The number of grid points along the shell-to-solid transition boundary is the same for the affected shell

units (i.e., the same number of rows in shell units 4, 5, and 6 in this case). The first step is to define a set

of G-3/G-4 records along the shell/solid transition boundary for averaging the translational degrees of 

freedom between the shell element node and the solid element nodes. The second step is to define 

“softlinks” (element E121) between the shell element node and the through-the-thickness nodes of the 

solid elements at that planar nodal location. This step is performed by defining an element unit with

nodes (S-1 records) and elements (T-1 records) defined along the shell-to-solid transition boundary.

These nodes and elements are defined using the existing shell unit values and their generation exploits the 

in-line looping capability of the STAGS S1 input processor. No shell unit connection record (G-1 record) 

is defined for these boundaries. The connections are done explicitly with the constraints just described

and the element unit definition for the E121 softlink elements. This shell-to-solid modeling approach is

illustrated in the S1 input file named crack1sm.inp – for manual input of the shell-to-solid

connections.

This overall shell-to-solid modeling process is rather cumbersome and error prone; hence, an automated

procedure is available within STAGS to connect shell and solid elements along shell-unit boundary lines.

The analyst simply defines the shell units as before using shell elements and solid elements in the

appropriate shell units. Then define a shell unit connection record (G-1 record) for the shell-to-solid

juncture using a negative value for MUNIT. STAGS then examines the two shell units and automatically

generates the constraints and softlinks along the shell-to-solid element boundary line. . This shell-to-solid

modeling approach is illustrated in the S1 input file named crack1sa.inp – for automatic input of the

shell-to-solid connections.

Crack modeling is achieved using the G-5, G-6 and G-7 records that generate constraints along a

predetermined path with coincident nodes generated along that path. A single crack definition is defined

with “open” segments as well as “closed” segments. Crack tips occur at the intersection of open and

closed segments. That is, a 2-inch-long crack would require 32 0.0625-inch-long elements with node 33

defining the crack tip (assuming nodes 1 through 32 are used with the 32 elements along the initial crack

length). Additional nodes are then used to define a “closed” crack. Crack growth is then defined along a

predetermined path built directly into the finite element model.

Modeling a single crack with a single tip using three-dimensional solid elements is slightly more complex

than for shell element models. For a through-crack in a solid element model, the open and closed crack

concept is applied for each plane of nodes through the thickness. For the bounding surface planes of the

solid model, a single element crack record (G-7 record) is required. For interior planes, two records are

needed to account for adjacent elements through the thickness.

Single cracks with multiple tips can be generated to simulate multi-site damage (MSD) cases. In such

cases, multiple nodal-crack records (G-6 records) are needed to define several open and closed crack

segments (single crack with multiple crack tips). These records are mesh dependent in their definition but

are straightforward to generate.

Crack growth is simulated using the nodal release procedure in combination with the load relaxation

procedure to re-establish equilibrium in the structure once a crack growth criterion is met and nodal

release occurs. STAGS currently uses the crack-tip opening angle or CTOA criterion for crack growth.

The analyst provides the critical value consistent for the material, the panel thickness, the kinematics

assumption near the crack (plane stress or plane strain), and the finite element mesh size near the crack
179

tip. The critical CTOA value strongly affects the computed solution and typically involves repeated

solution of standard test configurations for a particular material and a particular thickness before an

analysis critical value for a given finite element model can be defined.

Numerical Results and Discussion

Dawicke (1997) reported M(T) fracture test results for 0.090-inch-thick 2024-T3 aluminum panels in the 

LT orientation. The test configuration for a 12-inch-wide M(T) panel with an initial 4.0-inch-long center 

through-crack is analyzed in this study. Fracture test results are report by Dawicke (1997) for specimens

with and without guide plates to prevent local buckling near the crack. Test results are also reported for 

multiple-site damage cases.

The present modeling strategy for these panels assumes a symmetrical response in the width direction.

The finite element discretization process uses the mesh transition feature with the E410 shell elements

and doubles the number of the elements (or halves the element size) in the width direction as the panel

midlength is approached. Initially the element size in the width direction of shell unit 1 is one inch. Then

several shell units are used to change the mesh refinement. Mesh doubling occurs in the first four shell

units so that the element size in the width direction of shell unit 5 is reduced to 0.0625 inches. This

element size is somewhat larger than the 1-mm-rule (0.040-inch-rule) recommended for finite element

models near the crack front – based on the constant-strain triangular element. Then mesh halving is used

in the last four shell units. The critical value of CTOA is taken as 4.6 degrees. This value is strongly

dependent on the material, geometry, and finite element discretization near the crack front. There is no

initial geometric surface imperfection used with the finite element model and thus the simulation is for the 

M(T) panel with guide plates to present local buckling near the crack.

After each converged load step, a computation is made to evaluate the current value of the CTOA. If this

computed value exceeds the critical value given on the G-5 input record, then the constraints on the

coincident nodes at the crack tip are released (i.e., nodal release). At this point, the model is no longer in

equilibrium unless forces necessary to keep the “released” nodes together (i.e., to “close” the crack) are 

applied to the released nodes. This force imbalance is treated as a right-hand-side vector with its own

load factor PX while holding the applied load factors (PA and PB) fixed. This new load factor PX is then

decremented from a value of one to zero and nonlinear solutions are obtained for each PX value until the 

load imbalance is relaxed and the structure with the new crack extension is again in equilibrium. This

procedure is called load relaxation and facilitates the crack growth simulation in an automated manner 

using the CTOA criterion.

The first analysis case is an M(T) panel 12-inches wide, 24-inches long, 0.09-inches thick, and with an

initial 4-inch-long center through-crack. This panel was analyzed first using 4-node plane-stress shell

E410 elements throughout the finite element model. Then the panel is analyzed again using threedimensional 8-node solid E881 elements in shell unit 5 which treats a 0.25-inch region above and below

the crack as a three-dimensional region.

Results from the two-dimensional plane stress model are summarized in Figures 59 through 61. Crack

extension Δa as a function of the far-field stress is shown in Figure 59. Test data from Tables 10 (with

buckling guide plates) and 13 (without buckling guide plates) of Dawicke (1997) are compared with the 

STAGS predictions. The far-field stress from the STAGS model is computed by dividing the equilibrium 

force summation across the loaded edge of the panel by the panel cross-sectional area (product of panel

width and thickness). Crack extension is in terms of discrete incremental changes associated with the 

nodal-release approach and is based on the element size at the crack front. Test and simulation results are 

compared in Figure 59. The load relaxation steps are shown in this figure to illustrate the process;

however, only the peak far-field stress values for a given value of crack extension are typically plotted.
180

Good correlation between test and analysis is indicated for the case when local buckling near the crack is

prevented. Contour plots of the longitudinal displacement component and the longitudinal stress

component are shown in Figures 60 and 61, respectively, for three solution steps. A compressiondominated region around the crack is evident from Figure 61 and indicates that a local instability may

occur.

Results from the transition shell/solid model are summarized in Figures 62 through 64. Crack extension

as a function of the far-field stress is shown in Figure 62 where test data from Table 10 of Dawicke 

(1997) are compared with the STAGS predictions (plane stress model and local solid model). The load

relaxation process is again illustrated in this figure. Good correlation between test and analysis is

indicated. Contour plots of the longitudinal displacement component and the longitudinal stress

component are shown in Figures 63 and 64, respectively, for three solution steps. These plots illustrate 

that the response transitions smoothly across the shell/solid transition boundary. The results from the

local solid model are below those obtained from the plane stress model due to using the same critical

CTOA value.

A second analysis case is considered that includes multiple-site damage (MSD) in the form of two 0.30-

inch-long cracks on either side of the center 4-inch-long crack with approximately 0.70-inch spacing

between crack tips. The crack lengths and spacing between the crack tips in the test are not exactly

symmetric across the panel centerline. In addition, the finite element mesh size used in the single crack

case is also used for the MSD case and therefore certain limitations are imposed. In the STAGS model,

the spacing between the crack tips (i.e., “closed” crack regions) is 0.6875 inches and the length of the

smaller cracks (i.e., “open” crack regions) is 0.3125 inches – clearly some differences between test and

simulation are anticipated. STAGS does have the capability to specialize the mesh layout (using the N-1

and N-9 records) to match the test configuration; however, since only a symmetric model was being

consider this was not done. Within the STAGS modeling approach, this case is treated as a single crack

with multiple tips rather than multiple cracks.

Results from the two-dimensional plane stress model are summarized in Figures 65 through 68. Crack

extension as a function of the far-field stress is shown in Figure 65 where test data from Table 19 of 

Dawicke (1997) for the 5-crack MSD case (configuration E shown in Figure 3 of that report) are

compared with the STAGS predictions. Good correlation between test and analysis is indicated. Contour 

plots of the longitudinal displacement component and the longitudinal stress component are shown in

Figures 66 and 67, respectively, for three solution steps. These results illustrate the crack “linking” 

behavior where the center crack grows and links with the smaller cracks as load is applied. The size of

the compression-dominated region appears to expand quickly as the link-up process occurs.

Contour plots of the plastic strain component in the longitudinal direction are shown in Figure 68 for the 

center two-inch region of the panel. As the load increases the crack extends and the local plastic strain

field also expands around each of the cracks in the MSD panel. In these simulations, it was assumed that

the elasto-plastic behavior was confined to this region. This modeling assumption appears to be true.
181

Figure 59. Crack extension as a function of far-field applied stress for NASA M(T) 0.09-inch-thick, 12-

inch-wide panel with a 4-inch-long center through-crack using plane stress modeling
182

(a) Step 40, Δa=0.5 in. (b) Step 90, Δa=1.0 in. (c) Step 166, Δa=1.6875 in.

Figure 60. Contour plots of the longitudinal displacement component from the plane stress model for 

NASA M(T) 0.09-inch-thick, 12-inch-wide panel with a 4-inch-long center through-crack.

-0.12

0

(inches)
183

(a) Step 40, Δa=0.5 in. (b) Step 90, Δa=1.0 in. (c) Step 166, Δa=1.6875 in.

Figure 61. Contour plots of the longitudinal stress component from the plane stress model for NASA

M(T) 0.09-inch-thick, 12-inch-wide panel with a 4-inch-long center through-crack.

-6,000

84,000

(psi)
184

Figure 62. Crack extension as a function of far-field applied stress for NASA M(T) 0.09-inch-thick, 12-

inch-wide panel with a 4-inch-long center through-crack using shell-solid transition modeling
185

(a) Step 52, Δa=0.5 in. (b) Step 111, Δa=1.0 in. (c) Step 151, Δa=1.4375 in.

Figure 63. Contour plots of the longitudinal displacement component from the shell-solid transition

model for NASA M(T) 0.09-inch-thick, 12-inch-wide panel with a 4-inch-long center through-crack.

-0.12

0

(inches)
186

(a) Step 52, Δa=0.5 in. (b) Step 111, Δa=1.0 in. (c) Step 151, Δa=1.4375 in.

Figure 64. Contour plots of the longitudinal stress component from the shell-solid transition model for 

NASA M(T) 0.09-inch-thick, 12-inch-wide panel with a 4-inch-long center through-crack.

-6,000

84,000

(psi)
187

Figure 65. Crack extension as a function of far-field applied stress for NASA M(T) 0.09-inch-thick, 12-

inch-wide panel with multiple site damage using plane stress modeling
188

(a) Step 61, Δa=1.125 in. (b) Step 71, Δa=1.5 in. (c) Step 100, Δa=1.9375 in.

Figure 66. Contour plots of the longitudinal displacement component from the plane stress model for 

NASA M(T) 0.09-inch-thick, 12-inch-wide panel with multiple site damage.

-0.08

0

(inches)
189

(a) Step 61, Δa=1.125 in. (b) Step 71, Δa=1.5 in. (c) Step 100, Δa=1.9375 in.

Figure 67. Contour plots of the longitudinal stress component from the plane stress model for NASA

M(T) 0.09-inch-thick, 12-inch-wide panel with multiple site damage.

-6,000

84,000

(psi)
190

(a) Step 61

.

(b) Step 71.

(c) Step 100.

Figure 68. Contour plots of longitudinal plastic strain component from the plane stress model for NASA

M(T) 0.09-inch-thick, 12-inch-wide panel with multiple site damage – close-up view of shell units 4, 5,

and 6 (center two inches of the panel).

0.16

0
191

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Advanced-Testcases/Type-B-crack

where separate subdirectories are provided for three cases: center-crack shell-element model; centercrack shell/solid-element model; and multiple-site-damage shell-element model. These directories are:

shell

solid/manual

solid/auto

msd

Three different STAGS models are presented here. The first two models are for the middle-crack-tension

(or M(T)) panel. Both models have the same planar finite element discretization and both use nine shell

units over the full panel length and half the width (half symmetry model). However, one model uses shell

elements (E410) only for all shell units, while the other model uses four solid elements (E881) through

the shell thickness for the shell unit containing the crack (shell unit 5) and shell elements (E410)

elsewhere.

The third STAGS model is a variation on the first model except that there are two additional smaller 

cracks along the panel midlength. It can be viewed as a single crack with multiple tips. This model

exhibits multiple-site damage or MSD. This simulation is similar to the 5-crack MSD fracture test

reported by Dawicke (1997). The finite element model approximates the actual test configuration

because of the uniform element size along the panel width and the symmetry conditions. The MSD

configuration features a center 4-inch-long crack followed by a 0.6875-inch-long space then a 0.3125-

inch-long crack then another 0.6875-inch-long space and another 0.3125-inch-long crack. The remainder 

of the panel width (2-inches) has no additional initial cracks but forms the crack extension path. The 

finite element model of the MSD case assumes a symmetric distribution of the damage across the panel

width even though the test configuration is not precisely symmetric.

Typical Center-Crack Panel Input Files – Shell Element Model

crack1.inp (for S1 processor)

Middle crack tension panel - M(T) $a-1

C

C 24 in. long, 12 in. wide, 0.09 in. thick

C with 4" long through center crack

C (2L=24; 2W=12; 2a=4; 2a/2W=1/3)

C

C Modeled region is 24 in. long, 6 in. wide

C with a 2 inch long crack (full length, half

C width).

C

0 0 0 0 0 0 0 $B-1 ANALYSIS TYPE

9 0 0 8 1 0 0 0 1 $B-2 MODEL SUMMARY

2 0 2 0 0 1 $B-3 DATA TABLE SUMMARY -> use gcp

C

C Use mesh refinement

C Unit 1 is 6" x 6"; use dx=0.5" and dy=0.5"

C Unit 2 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 3 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 4 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 5 is .50" x 6"; use dx=0.0625" and dy=0.0625"
192

C Unit 6 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 7 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 8 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 9 is 6" x 6"; use dx=dy=1.0"

C

13 13 7 25 9 49 ,

7 97 9 97 7 97 ,

9 49 7 25 13 13 $F-1 GRID SUMMARY

C

C Shell unit connection records

C - don't connect solids to shells with g-1 records

C

1 3 2 1 $G-1

2 3 3 1 $G-1

3 3 4 1 $G-1

4 3 5 1 $G-1

5 3 6 1 $G-1

6 3 7 1 $g-1

7 3 8 1 $g-1

8 3 9 1 $g-1

C

C Impose u=u at row 1 col. 1 across top of panel

C

1 1 1 1 1 1 0 1 $G-2 PARTIAL COMPATIBILITY U=CONSTANT AT EDGE

C

C Crack definition (element size is 0.0625")

C Note: nodes 1 to 32 open which gives an initial half crack length

C equal to 32 elements or 2" long; node 33 is at crack tip

C

1 2 1 1 4.6 0.0625 $G-5 Crack Inserted Node Set

1 5 5 1 5 32 $G-6 "open" crack (2" long)

0 5 5 33 5 97 $G-6 "closed" crack (4" long)

0 5 4 1 4 96 $G-7

C

C Input historical STAGS material tables

C

1 0 0 $I-1 Elastic only

10.351967E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

2 5 0 $i-1 Elasto-plastic

10.351967E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

0.00483 50000.0, $i-3 yield stress

0.015 56600.0, $i-3

0.04 62400.0, $I-3

0.1 68200.0, $I-3

0.16 71100.0 $I-3 ultimate stress

C -------------------------GCP------------------------------------

C 2024-T3 (LT) Aluminum alloy - ISOTROPIC MATERIAL

C

ISOELASTIC_MATERIAL 1 1 1 $I-5A GCP COMMAND RECORD

10.351967E+6, $I-7A E

0.30 , $I-7A NU

2.59E-5 , $I-7A MASS DENSITY

0.0 , $I-7A CTE (alpha)

0.0 , $I-7A CHE (beta)

0.0 0.0 $I-7A REF. TEMP AND REF. MOISTURE CONTENT

PLASTIC_WB_MATERIAL 2 1 1 2 0 $ WHITE-BESSELING PLASTICITY MODEL

10.351967E+6 0.3 2.59E-5 0.0 5 $I-9a E, nu, rho, cte, npoints

0.00483 50000.0, $i-9b yield stress

0.015 56600.0, $i-9b

0.04 62400.0, $I-9b

0.1 68200.0, $I-9b

0.16 71100.0 $I-9b ultimate stress
193

C

SHELL_FABRICATION 1 1 0 0 0 $I-5A Elastic only

1 $I-21A Aluminum MATID

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION

SHELL_FABRICATION 2 1 1 0 0 $I-5A Elasto-plastic

2 $I-21A Aluminum MATID

5 $I-21B Integration points through thickness

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION

SOLID_FABRICATION 1 2 0 1 0 $I-5A Elasto-plastic

0.0225 $I-21C Solid Element THICKNESSES

END $I-5A END GCP INPUT

C --------------------------------------------------------------

C

C define historical STAGS shell wall data

C

1 1 1 0 $K-1 elastic regions

1 0.09 0.0 0 $k-2 single layer

2 1 1 5 $K-1 elastic regions

2 0.09 0.0 0 $k-2 single layer

C

C Unit 1 - top part of panel

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

0.0 6.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

0 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

110 000 $P-2 X=0 EDGE

1 0 0 $Q-1 LOADING (base load with Area=1.08 sq. in. gives

1 1 0 $Q-2 LOAD SET far field stress of 10 ksi)

-0.02 -1 1 1 1 0 $Q-3 applied displ. at point plus constraints

C-10800.0 1 1 1 1 0 $Q-3 applied load at point plus constraints

0 0 0 0 0 0 1 0 $R-1 OUTPUT FLAGS

1 0 $ output displacements across top of panel

C

C Unit 2 - segment 2

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

6.0 9.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 3 - segment 3

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

9.0 11.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 4 - segment 4

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.0 11.75 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH
194

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 5 - center section with center crack - can be elasto-plastic

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.75 12.25 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 6 - section 6 - can be elasto-plastic

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

12.25 13.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 7 - segment 7

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

13.0 15.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 8

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

15.0 18.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 9 Bottom section

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

18.0 24.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 2 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 $R-1 OUTPUT FLAGS

crack1.bin (for S2 processor)

Middle crack tension panel X_ck $a-1

C

C nonlinear elasto-plastic crack growth analysis

C

3 1 0 0 0 0 0 -1 $b-1 analysis type and options
195

1.0 0.50 6.0 $c-1

0 6000 10 -20 0 1.0e-4 $d-1

0 0 0 $et-1

C

C linear elastic stress analysis

C

0 1 0 0 0 0 0 -1 $b-1 analysis type and options

1.0 1.00 1.0 $c-1 Apply just the base load

crack1.pin (for STAPL processor)

Panel with center crack

4 0 1 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C contour plot of u-displ component

2 0 1 20 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 40 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 90 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 166 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

C contour plot of longitudinal stress component

2 0 7 20 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 40 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 90 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 166 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

C plot model

0 0 0 0 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 45.0 / 3 -90.0 $PL-6 rotations

C plot first solution close to crack so you can see it!

1 3 1 1 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot unit = 5 only

0.0 3 0. -0.1 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 45.0 / 3 -90.0 $PL-6 rotations

Typical Center-Crack Panel Input Files – Manual Shell/Solid Element Model

crack1sm.inp (for S1 processor)

Middle crack tension panel - M(T) $a-1

C

C 24 in. long, 12 in. wide, 0.09 in. thick

C with 4" long through center crack

C (2L=24; 2W=12; 2a=4; 2a/2W=1/3)

C

C Modeled region is 24 in. long, 6 in. wide

C with a 2 inch long crack (full length, half
196

C width). 3D model near crack (.25 inches on

C either side).

C

0 0 0 0 0 0 0 $B-1 ANALYSIS TYPE

9 1 0 6 1 -6 0 0 5 $B-2 MODEL SUMMARY

2 0 2 0 0 1 $B-3 DATA TABLE SUMMARY -> use gcp

C

C Use mesh refinement

C Unit 1 is 6" x 6"; use dx=0.5" and dy=0.5"

C Unit 2 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 3 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 4 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 5 is .50" x 6"; use dx=0.0625" and dy=0.0625"

C Unit 6 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 7 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 8 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 9 is 6" x 6"; use dx=dy=1.0"

C

13 13 7 25 9 49 ,

7 97 9 97 7 97 ,

9 49 7 25 13 13 $F-1 GRID SUMMARY

C

C Shell unit connection records

C - don't connect solids to shells with g-1 records

C

1 3 2 1 $G-1

2 3 3 1 $G-1

3 3 4 1 $G-1

6 3 7 1 $g-1

7 3 8 1 $g-1

8 3 9 1 $g-1

C

C Impose u=u at row 1 col. 1 across top of panel

C

1 1 1 1 1 1 0 1 $G-2 PARTIAL COMPATIBILITY U=CONSTANT AT EDGE

C

C Impose Lagrtanian constraints to average displacements at

C shell-solid interface

C

6 97 0 0 1 0 $G-3

4 7 1 1 -5.e4 $G-4

5 1 1 1 +1.e4 1 $G-4

5 1 1 1 +1.e4 2 $G-4

5 1 1 1 +1.e4 3 $G-4

5 1 1 1 +1.e4 4 $G-4

5 1 1 1 +1.e4 5 $G-4

C

6 97 0 0 1 0 $G-3

4 7 1 2 -5.e4 $G-4

5 1 1 2 +1.e4 1 $G-4

5 1 1 2 +1.e4 2 $G-4

5 1 1 2 +1.e4 3 $G-4

5 1 1 2 +1.e4 4 $G-4

5 1 1 2 +1.e4 5 $G-4

C

6 97 0 0 1 0 $G-3

4 7 1 3 -5.e4 $G-4

5 1 1 3 +1.e4 1 $G-4

5 1 1 3 +1.e4 2 $G-4

5 1 1 3 +1.e4 3 $G-4

5 1 1 3 +1.e4 4 $G-4

5 1 1 3 +1.e4 5 $G-4

C
197

6 97 0 0 1 0 $G-3

6 1 1 1 -5.e4 $G-4

5 9 1 1 +1.e4 1 $G-4

5 9 1 1 +1.e4 2 $G-4

5 9 1 1 +1.e4 3 $G-4

5 9 1 1 +1.e4 4 $G-4

5 9 1 1 +1.e4 5 $G-4

C

6 97 0 0 1 0 $G-3

6 1 1 2 -5.e4 $G-4

5 9 1 2 +1.e4 1 $G-4

5 9 1 2 +1.e4 2 $G-4

5 9 1 2 +1.e4 3 $G-4

5 9 1 2 +1.e4 4 $G-4

5 9 1 2 +1.e4 5 $G-4

C

6 97 0 0 1 0 $G-3

6 1 1 3 -5.e4 $G-4

5 9 1 3 +1.e4 1 $G-4

5 9 1 3 +1.e4 2 $G-4

5 9 1 3 +1.e4 3 $G-4

5 9 1 3 +1.e4 4 $G-4

5 9 1 3 +1.e4 5 $G-4

C

C Crack definition (element size is 0.0625")

C Note: nodes 1 to 32 open which gives an initial crack length

C equal to 32 elements or 2" long; node 33 is at crack tip

C

1 2 1 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 1 5 32 1 $G-6 "open" crack (2" long)

0 5 5 33 1 5 97 1 $G-6 "closed" crack (4" long)

0 5 4 1 1 4 96 1 $G-7

C

2 2 2 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 2 5 32 2 $G-6 "open" crack (2" long)

0 5 5 33 2 5 97 2 $G-6 "closed" crack (4" long)

0 5 4 1 1 4 96 1 $G-7

0 5 4 1 2 4 96 2 $G-7

C

3 2 2 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 3 5 32 3 $G-6 "open" crack (2" long)

0 5 5 33 3 5 97 3 $G-6 "closed" crack (4" long)

0 5 4 1 2 4 96 2 $G-7

0 5 4 1 3 4 96 3 $G-7

C

4 2 2 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 4 5 32 4 $G-6 "open" crack (2" long)

0 5 5 33 4 5 97 4 $G-6 "closed" crack (4" long)

0 5 4 1 3 4 96 3 $G-7

0 5 4 1 4 4 96 4 $G-7

C

5 2 1 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 5 5 32 5 $G-6 "open" crack (2" long)

0 5 5 33 5 5 97 5 $G-6 "closed" crack (4" long)

0 5 4 1 4 4 96 4 $G-7

C

C Define element unit data for softlink elements

C

1164 776 $H-1 spring "softlink" elements connecting shells and solids

C

C Input historical STAGS material tables

C

1 0 0 $I-1 Elastic only
198

10.351967E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

2 5 0 $i-1 Elasto-plastic

10.351967E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

0.00483 50000.0, $i-3 yield stress

0.015 56600.0, $i-3

0.04 62400.0, $I-3

0.1 68200.0, $I-3

0.16 71100.0 $I-3 ultimate stress

C -------------------------GCP------------------------------------

C 2024-T3 (LT) Aluminum alloy - ISOTROPIC MATERIAL

C

ISOELASTIC_MATERIAL 1 1 1 $I-5A GCP COMMAND RECORD

10.351967E+6, $I-7A E

0.30 , $I-7A NU

2.59E-5 , $I-7A MASS DENSITY

0.0 , $I-7A CTE (alpha)

0.0 , $I-7A CHE (beta)

0.0 0.0 $I-7A REF. TEMP AND REF. MOISTURE CONTENT

PLASTIC_WB_MATERIAL 2 1 1 2 0 $ WHITE-BESSELING PLASTICITY MODEL

10.351967E+6 0.3 2.59E-5 0.0 5 $I-9a E, nu, rho, cte, npoints

0.00483 50000.0, $i-9b yield stress

0.015 56600.0, $i-9b

0.04 62400.0, $I-9b

0.1 68200.0, $I-9b

0.16 71100.0 $I-9b ultimate stress

C

SHELL_FABRICATION 1 1 0 0 0 $I-5A Elastic only

1 $I-21A Aluminum MATID

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION

SHELL_FABRICATION 2 1 1 0 0 $I-5A Elasto-plastic

2 $I-21A Aluminum MATID

5 $I-21B Integration points through thickness

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION

SOLID_FABRICATION 1 2 0 1 0 $I-5A Elasto-plastic

0.0225 $I-21C Solid Element THICKNESSES

END $I-5A END GCP INPUT

C --------------------------------------------------------------

C

C define historical STAGS shell wall data

C

1 1 1 0 $K-1 elastic regions

1 0.09 0.0 0 $k-2 single layer

2 1 1 5 $K-1 elastic regions

2 0.09 0.0 0 $k-2 single layer

C

C Unit 1 - top part of panel

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

0.0 6.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

0 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

110 000 $P-2 X=0 EDGE

1 0 0 $Q-1 LOADING (base load with Area=1.08 sq. in. gives

1 1 0 $Q-2 LOAD SET far field stress of 10 ksi)

-0.02 -1 1 1 1 0 $Q-3 applied displ. at point plus constraints

C-10800.0 1 1 1 1 0 $Q-3 applied load at point plus constraints

0 0 0 0 0 0 1 0 $R-1 OUTPUT FLAGS

1 0 $ output displacements across top of panel

C

C Unit 2 - segment 2
199

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

6.0 9.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 3 - segment 3

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

9.0 11.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 4 - segment 4

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.0 11.75 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 5 - center section with center crack - can be elasto-plastic

C

2 0 0 0 4 4 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.75 12.25 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

881 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 6 - section 6 - can be elasto-plastic

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

12.25 13.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 7 - segment 7

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

13.0 15.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 8
200

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

15.0 18.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 9 Bottom section

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

18.0 24.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 2 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 $R-1 OUTPUT FLAGS

C

C Generate the "softlinks" to connect shells to solids

C

C Connect unit 4 shells to unit 5 solids

C

1 4 7 1 3*0. 3*0 97 / 1 0 0 1 $S1/S1-1A

98 5 1 1 3*0. 3*0 97 1 / 1 0 0 1 $S1/S1-1A

195 5 1 1 3*0. 3*0 97 2 / 1 0 0 1 $S1/S1-1A

292 5 1 1 3*0. 3*0 97 3 / 1 0 0 1 $S1/S1-1A

389 5 1 1 3*0. 3*0 97 4 / 1 0 0 1 $S1/S1-1A

486 5 1 1 3*0. 3*0 97 5 / 1 0 0 1 $S1/S1-1A

C

C Connect unit 6 shells to unit 5 solids

C

C

583 6 1 1 3*0. 3*0 97 / 1 0 0 1 $S1/S1-1A

680 5 9 1 3*0. 3*0 97 1 / 1 0 0 1 $S1/S1-1A

777 5 9 1 3*0. 3*0 97 2 / 1 0 0 1 $S1/S1-1A

874 5 9 1 3*0. 3*0 97 3 / 1 0 0 1 $S1/S1-1A

971 5 9 1 3*0. 3*0 97 4 / 1 0 0 1 $S1/S1-1A

1068 5 9 1 3*0. 3*0 97 5 / 1 0 0 1 $S1/S1-1A

C

C generate soflinks from unit 4 shells to unit 5 solids

C

1 98 195 121 97 1 1 1 / 1.e4 $T1/T1-B

1 98 292 121 97 1 1 1 / 1.e4 $T1/T1-B

1 98 389 121 97 1 1 1 / 1.e4 $T1/T1-B

1 98 486 121 97 1 1 1 / 1.e4 $T1/T1-B

C

C generate soflinks from unit 6 shells to unit 5 solids

C

583 680 777 121 97 1 1 1 / 1.e4 $T1/T1-B

583 680 874 121 97 1 1 1 / 1.e4 $T1/T1-B

583 680 971 121 97 1 1 1 / 1.e4 $T1/T1-B

583 680 1068 121 97 1 1 1 / 1.e4 $T1/T1-B

C

0 0 $U

0 $ 1 0 0 0 0 1 $V

crack1sm.bin (for S2 processor)

Middle crack tension panel $a-1

C

C nonlinear elasto-plastic crack growth analysis

C

3 1 0 0 0 0 0 -1 $b-1 analysis type and options
201

1.0 0.50 6.0 $c-1

0 30000 20 -20 0 1.0e-4 $d-1

0 0 0 $et-1

C

C linear elastic stress analysis

C

0 1 0 0 0 0 0 -1 $b-1 analysis type and options

1.0 1.00 1.0 $c-1 Apply just the base load

crack1sm.pin (for STAPL processor)

Panel with center crack

4 0 1 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C contour plot of longitudinal stress component

2 0 7 22 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 52 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 111 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 151 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

C contour plot of u-displ component

2 0 1 22 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 52 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 111 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 151 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -.12 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

C plot model

0 0 0 0 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1.0 0.0 0. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 45.0 / 3 -90.0 $PL-6 rotations

C plot first solution close to crack so you can see it!

1 3 1 1 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot unit = 5 only

0.0 3 0. -0.1 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 20.0 / 2 45.0 / 3 -90.0 $PL-6 rotations

Typical Center-Crack Panel Input Files – Automatic Shell/Solid Element Model

crack1sa.inp (for S1 processor)

Middle crack tension panel - M(T) $a-1

C

C 24 in. long, 12 in. wide, 0.09 in. thick

C with 4" long through center crack

C

0 0 0 0 1 3 0 $B-1 ANALYSIS TYPE

5

3 -90.0 / 2 0.0 / 1 -20.0

9 0 0 8 1 0 0 0 5 $B-2 MODEL SUMMARY
202

2 0 2 0 0 1 $B-3 DATA TABLE SUMMARY -> use gcp

C

C Use mesh refinement

C Unit 1 is 6" x 6"; use dx=0.5" and dy=0.5"

C Unit 2 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 3 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 4 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 5 is .50" x 6"; use dx=0.0625" and dy=0.0625"

C Unit 6 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 7 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 8 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 9 is 6" x 6"; use dx=dy=1.0"

C

13 13 7 25 9 49 ,

7 97 9 97 7 97 ,

9 49 7 25 13 13 $F-1 GRID SUMMARY

C

C Shell unit connection records

C - don't connect solids to shells with g-1 records

C

1 3 2 1 $G-1

2 3 3 1 $G-1

3 3 4 1 $G-1

-4 3 5 1 $G-1

-5 3 6 1 $G-1

6 3 7 1 $g-1

7 3 8 1 $g-1

8 3 9 1 $g-1

C

C Impose u=u at row 1 col. 1 across top of panel

C

1 1 1 1 1 1 0 1 $G-2 PARTIAL COMPATIBILITY U=CONSTANT AT EDGE

C

C Crack definition (element size is 0.0625")

C Note: nodes 1 to 32 open which gives an initial crack length

C equal to 32 elements or 2" long; node 33 is at crack tip

C

1 2 1 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 1 5 32 1 $G-6 "open" crack (2" long)

0 5 5 33 1 5 97 1 $G-6 "closed" crack (4" long)

0 5 4 1 1 4 96 1 $G-7

C

2 2 2 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 2 5 32 2 $G-6 "open" crack (2" long)

0 5 5 33 2 5 97 2 $G-6 "closed" crack (4" long)

0 5 4 1 1 4 96 1 $G-7

0 5 4 1 2 4 96 2 $G-7

C

3 2 2 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 3 5 32 3 $G-6 "open" crack (2" long)

0 5 5 33 3 5 97 3 $G-6 "closed" crack (4" long)

0 5 4 1 2 4 96 2 $G-7

0 5 4 1 3 4 96 3 $G-7

C

4 2 2 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 4 5 32 4 $G-6 "open" crack (2" long)

0 5 5 33 4 5 97 4 $G-6 "closed" crack (4" long)

0 5 4 1 3 4 96 3 $G-7

0 5 4 1 4 4 96 4 $G-7

C

5 2 1 1 4.6 0.0 $G-5 Crack Inserted Node Set

1 5 5 1 5 5 32 5 $G-6 "open" crack (2" long)

0 5 5 33 5 5 97 5 $G-6 "closed" crack (4" long)
203

0 5 4 1 4 4 96 4 $G-7

C

C Input historical STAGS material tables

C

1 0 0 $I-1 Elastic only

10.359834E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

2 5 0 $i-1 Elasto-plastic

10.359834E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

0.00483 50000.0, $i-3 yield stress

0.015 56600.0, $i-3

0.04 62400.0, $I-3

0.1 68200.0, $I-3

0.16 71100.0 $I-3 ultimate stress

C -------------------------GCP------------------------------------

C 2024-T3 (LT) Aluminum alloy - ISOTROPIC MATERIAL

C

ISOELASTIC_MATERIAL 1 1 1 $I-5A GCP COMMAND RECORD

10.359834E+6, $I-7A E

0.30 , $I-7A NU

2.59E-5 , $I-7A MASS DENSITY

0.0 , $I-7A CTE (alpha)

0.0 , $I-7A CHE (beta)

0.0 0.0 $I-7A REF. TEMP AND REF. MOISTURE CONTENT

PLASTIC_WB_MATERIAL 2 1 1 2 0 $ WHITE-BESSELING PLASTICITY MODEL

10.359834E+6 0.3 2.59E-5 0.0 5 $I-9a E, nu, rho, cte, npoints

0.00483 50000.0, $i-9b yield stress

0.015 56600.0, $i-9b

0.04 62400.0, $I-9b

0.1 68200.0, $I-9b

0.16 71100.0 $I-9b ultimate stress

C

SHELL_FABRICATION 1 1 0 0 0 $I-5A Elastic only

1 $I-21A Aluminum MATID

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION

SHELL_FABRICATION 2 1 1 0 0 $I-5A Elasto-plastic

2 $I-21A Aluminum MATID

5 $I-21B Integration points through thickness

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION

SOLID_FABRICATION 1 2 0 1 0 $I-5A Elasto-plastic

0.0225 $I-21C Solid Element THICKNESSES

END $I-5A END GCP INPUT

C --------------------------------------------------------------

C

C define historical STAGS shell wall data

C

1 1 1 0 $K-1 elastic regions

1 0.09 0.0 0 $k-2 single layer

2 1 1 5 $K-1 elastic regions

2 0.09 0.0 0 $k-2 single layer

C

C Unit 1 - top part of panel

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

0.0 6.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

0 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

110 000 $P-2 X=0 EDGE

1 0 0 $Q-1 LOADING (base load with Area=1.08 sq. in. gives

1 1 0 $Q-2 LOAD SET far field stress of 10 ksi)

-10800.0 1 1 1 1 0 $Q-3 applied load at point plus constraints
204

0 0 0 0 0 0 1 0 $R-1 OUTPUT FLAGS

1 0 $ output displacements across top of panel

C

C Unit 2 - segment 2

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

6.0 9.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 3 - segment 3

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

9.0 11.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 4 - segment 4

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.0 11.75 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 5 - center section with center crack - can be elasto-plastic

C

2 0 0 0 4 4 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.75 12.25 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

-1 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

881 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 6 - section 6 - can be elasto-plastic

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

12.25 13.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 7 - segment 7

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

13.0 15.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)
205

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 8

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

15.0 18.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 9 Bottom section

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

18.0 24.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

-1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 2 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 $R-1 OUTPUT FLAGS

Typical MSD Panel Input Files – Shell Element Model

crack5.inp (for S1 processor)

Middle crack tension panel - M(T) 5-crack MSD simulation $a-1

C

C 24 in. long, 12 in. wide, 0.09 in. thick

C with 4" long through center crack + MSD

C (2L=24; 2W=12; 2a=4; 2a/2W=1/3)

C

C Modeled region is 24 in. long, 6 in. wide

C with a 2 inch long crack (full length, half

C width). MSD Configuration E with 5 total

C cracks - 2 additional 0.3125" long cracks

C on either side of center crack. The spacing

C between the center crack and the next crack is

C 0.75" and between the next 2 cracks is 0.6875"

C

0 0 0 0 0 0 0 $B-1 ANALYSIS TYPE

9 0 0 8 1 0 0 0 1 $B-2 MODEL SUMMARY

2 0 2 0 0 1 $B-3 DATA TABLE SUMMARY -> use gcp

C

C Use mesh refinement

C Unit 1 is 6" x 6"; use dx=0.5" and dy=0.5"

C Unit 2 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 3 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 4 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 5 is .50" x 6"; use dx=0.0625" and dy=0.0625"

C Unit 6 is .75" x 6"; use dx=0.125" and dy=0.0625"

C Unit 7 is 2" x 6"; use dx=0.25" and dy=0.125"

C Unit 8 is 3" x 6"; use dx=0.5" and dy=0.25"

C Unit 9 is 6" x 6"; use dx=dy=1.0"

C

13 13 7 25 9 49 ,

7 97 9 97 7 97 ,

9 49 7 25 13 13 $F-1 GRID SUMMARY

C

C Shell unit connection records
206

C - don't connect solids to shells with g-1 records

C

1 3 2 1 $G-1

2 3 3 1 $G-1

3 3 4 1 $G-1

4 3 5 1 $G-1

5 3 6 1 $G-1

6 3 7 1 $g-1

7 3 8 1 $g-1

8 3 9 1 $g-1

C

C Impose u=u at row 1 col. 1 across top of panel

C

1 1 1 1 1 1 0 1 $G-2 PARTIAL COMPATIBILITY U=CONSTANT AT EDGE

C

C Crack definition (element size is 0.0625")

C Note: nodes 1 to 32 open which gives an initial half crack length

C equal to 32 elements or 2" long; node 33 is at crack tip

C plus 2 MSD 0.3125"-long cracks with a spacing of 0.75"

C and 0.6875" (tip-to-tip)

C

1 6 1 1 4.6 0.0625 $G-5 Crack Inserted Node Set

1 5 5 1 5 32 $G-6 "open" crack (2" long)

0 5 5 33 5 45 $G-6 "closed" crack (0.75" long)

1 5 5 46 5 49 $G-6 "open" crack (.3125" long)

0 5 5 50 5 61 $G-6 "closed" crack (0.6875" long)

1 5 5 62 5 65 $G-6 "open" crack (.3125" long)

0 5 5 66 5 97 $G-6 "closed" crack (1.9375" long)

0 5 4 1 4 96 $G-7

C

C Input historical STAGS material tables

C

1 0 0 $I-1 Elastic only

10.351967E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

2 5 0 $i-1 Elasto-plastic

10.351967E+6 0.3 0.0 0.1 $I-2 E, nu, skip, rho_weight

0.00483 50000.0, $i-3 yield stress

0.015 56600.0, $i-3

0.04 62400.0, $I-3

0.1 68200.0, $I-3

0.16 71100.0 $I-3 ultimate stress

C -------------------------GCP------------------------------------

C 2024-T3 (LT) Aluminum alloy - ISOTROPIC MATERIAL

C

ISOELASTIC_MATERIAL 1 1 1 $I-5A GCP COMMAND RECORD

10.351967E+6, $I-7A E

0.30 , $I-7A NU

2.59E-5 , $I-7A MASS DENSITY

0.0 , $I-7A CTE (alpha)

0.0 , $I-7A CHE (beta)

0.0 0.0 $I-7A REF. TEMP AND REF. MOISTURE CONTENT

PLASTIC_WB_MATERIAL 2 1 1 2 0 $ WHITE-BESSELING PLASTICITY MODEL

10.351967E+6 0.3 2.59E-5 0.0 5 $I-9a E, nu, rho, cte, npoints

0.00483 50000.0, $i-9b yield stress

0.015 56600.0, $i-9b

0.04 62400.0, $I-9b

0.1 68200.0, $I-9b

0.16 71100.0 $I-9b ultimate stress

C

SHELL_FABRICATION 1 1 0 0 0 $I-5A Elastic only

1 $I-21A Aluminum MATID

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION
207

SHELL_FABRICATION 2 1 1 0 0 $I-5A Elasto-plastic

2 $I-21A Aluminum MATID

5 $I-21B Integration points through thickness

0.090 $I-21C LAYER THICKNESSES

0.0 $I-21D LAYER ORIENTATION

SOLID_FABRICATION 1 2 0 1 0 $I-5A Elasto-plastic

0.0225 $I-21C Solid Element THICKNESSES

END $I-5A END GCP INPUT

C --------------------------------------------------------------

C

C define historical STAGS shell wall data

C

1 1 1 0 $K-1 elastic regions

1 0.09 0.0 0 $k-2 single layer

2 1 1 5 $K-1 elastic regions

2 0.09 0.0 0 $k-2 single layer

C

C Unit 1 - top part of panel

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

0.0 6.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

0 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

110 000 $P-2 X=0 EDGE

1 0 0 $Q-1 LOADING (base load with Area=1.08 sq. in. gives

1 1 0 $Q-2 LOAD SET far field stress of 10 ksi)

-0.02 -1 1 1 1 0 $Q-3 applied displ. at point plus constraints

C-10800.0 1 1 1 1 0 $Q-3 applied load at point plus constraints

0 0 0 0 0 0 1 0 $R-1 OUTPUT FLAGS

1 0 $ output displacements across top of panel

C

C Unit 2 - segment 2

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

6.0 9.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 3 - segment 3

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

9.0 11.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 4 - segment 4

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.0 11.75 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 5 - center section with center crack - can be elasto-plastic
208

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

11.75 12.25 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 Solid Fabribrication SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 6 - section 6 - can be elasto-plastic

C

2 0 0 0 0 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

12.25 13.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+2 0 0.0 0.0 0 1 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 0 0 0 0 $R-1 OUTPUT FLAGS

C

C Unit 7 - segment 7

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

13.0 15.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 8

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

15.0 18.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 6 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 $R-1 OUTPUT FLAGS

C

C Unit 9 Bottom section

C

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

18.0 24.0 0.0 6.0 $M-2 24-IN BY 12-IN. PLATE (half width model)

+1 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

6 3 2 4 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

0 0 0 $Q-1 NO LOADING

0 0 0 0 $R-1 OUTPUT FLAGS

crack5.bin (for S2 processor)

Middle crack tension panel $a-1

3 1 0 0 0 0 0 -1 $b-1 analysis type and options

1.0 0.50 6.0 $c-1

0 6000 10 -20 0 1.0e-4 $d-1

0 0 0 $et-1

crack5.pin (for STAPL processor)

Panel with center crack and MSD (5 cracks total)

6 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C contour plot of longitudinal stress component

2 0 7 20 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX
209

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 38 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 61 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 71 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 80 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 7 100 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -6000. 84000. $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

C contour plot of plastic strain Ep_xx in shell units 4,5,6

2 3 8 20 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot units = 4,5,6

0.0 3 0.0 0.0 0.16 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 3 8 38 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot units = 4,5,6

0.0 3 0.0 0.0 0.16 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 3 8 61 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot units = 4,5,6

0.0 3 0.0 0.0 0.16 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 3 8 71 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot units = 4,5,6

0.0 3 0.0 0.0 0.16 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 3 8 80 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot units = 4,5,6

0.0 3 0.0 0.0 0.16 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 3 8 100 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6 $PL-4 plot units = 4,5,6

0.0 3 0.0 0.0 0.16 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

C contour plot of u-displ component

2 0 1 20 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -0.08 1.0e-6 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 38 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -0.08 1.0e-6 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 61 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -0.08 1.0e-6 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 71 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -0.08 1.0e-6 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 80 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -0.08 1.0e-6 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations

2 0 1 100 0 0 1 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 -1. -0.08 1.0e-6 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 -90.0 $PL-6 rotations
210

Problem References

Rankin, C. C., Loden, W. A., and Swenson, L. W., STAGS Element Manual – Version 5.0 Preliminary,

Lockheed Martin Advanced Technology Center, Palo Alto, CA, September 2001.

Rankin, C. C., Brogan, F. A., Loden, W., and Cabiness, H., Structural Analysis of General Shells –

STAGS User Manual, Version 4.0, Lockheed Martin Advanced Technology Center, Palo Alto, CA, June

2000.

Riks, E., Rankin, C. C., and Brogan, F. A., “The Buckling Behavior of a Central Crack in a Plate under 

Tension,” Engineering Fracture Mechanics, Vol. 143, No. 4, 1992, pp. 529-548.

Rankin, C. C., Brogan, F. A., and Riks, E., “Some Computational Tools for the Analysis of Through

Cracks in Stiffened Fuselage Shells,” Computational Mechanics, Vol. 13, 1993, pp. 143-156.

Dawicke, D. S., Newman, J. C., Jr., Sutton, M. A., and Amstutz, B. E., Stable Tearing Behavior of a

Thin-Sheet Material with Multiple Cracks, NASA TM-109131, July 1994.

Viz, M. J., Potyondy, D. O., Zehnder, A. T., Rankin, C. C., and Riks, E., “Computation of Membrane and

Bending Stress Intensity Factors for Thin, Cracked Plates,” International Journal of Fracture, Vol. 72,

No. 1, 1995, pp. 21-38.

Dawicke, D. S., Fracture Tests on 0.09 Inch Thick 2024-T3 Aluminum Alloy, NASA TM-112869, 1997.

Unofficial draft document.

Seshadri, B. R. and Newman, J. C., Jr., Analyses of Buckling and Stable Tearing in Thin-Sheet Materials,

NASA TM-1998-208428, May 1998.

Seshadri, B. R., Newman, J. C., Jr., Dawicke, D. S., and Young, R. D., Fracture Analysis of the

FAA/NASA Wide Stiffened Panels, NASA TM-1998-208976, December 1998.

Gullerud, A. S., Dodds, R. H., Jr., Hampton, R. W., and Dawicke, D. S., “Three-Dimensional Modeling

of Ductile Crack Growth in Thin Sheet Metals: Computational Aspects and Validation,” Engineering

Fracture Mechanics, Vol. 63, No. 4, July 1999, pp. 347-374.

Rankin, C. C. and Riks, E., “On the Simulation of Crack-Propagation in Pressurized Fuselages,” AIAA

Paper No. 2000-1594, April 2000.

Rankin, C. C. and Riks, E., “Tools for the Evaluation of the Residual Strength of Cracked Pressurized

Fuselage Shells,” AIAA Paper No. 2001-1325, April 2001.

Rankin, C. C., “Riks Path Parameter Solution Control During Crack Node Release,” unpublished notes,

June 9, 1998.
211

Hybrid Quasi-Static/Transient Solution Procedures Application

Background

Thin-walled plates and shells often can carry loads well in excess of its buckling load determined from a 

linear bifurcation buckling analysis. The structural response for load levels below the buckling load is

referred to as the primary solution or pre-buckling solution. It may be linear or nonlinear. Beyond the

buckling load, the response is referred to as postbuckling behavior when the response is stable and

collapse when the response is unstable. For these structures, the analyst needs to examine the role initial

geometry imperfections and “generalized” imperfections if possible. Generalized imperfections refer to

surface imperfections, thickness variations, variations in lamination, fabrication inconsistencies,

eccentricities in loading, and other aspects that cause the structure, its boundary conditions, and its

loading to be less than ideal (e.g., see Hilburger and Starnes, 2002).

Complex nonlinear response often involves changes in structural behavior that may develop gradually or 

may suddenly occur. Transition from a pre-buckled state to a post-buckled state for plates can be a

gradual process depending on the imperfections. Shell structures, on the other hand, often exhibit

collapse behavior. In some cases, the structural response involves changes in the buckle pattern in the

post-buckled state. Stein (1961) explored this behavior and also presented test results illustrating the 

phenomenon of buckle pattern changes. Supple (1967, 1968, 1970) has studied this phenomena as well

and provides insight into the structural response for simple configurations. Tiwari and Hyer (1996, 2000) 

also explored secondary buckling response predictions. However, Riks et al. (1993, 1996, 1997) 

provided the first computational procedure for nonlinear finite element analysis codes. Their approach

involves the use of a nonlinear static solution procedure for a period and then switching to a nonlinear

transient dynamics solution procedure. After the dynamic behavior has “settled” then the nonlinear static 

solution procedure is resumed after equilibrium is re-established. The term “load relaxation” is used for 

the procedure to re-establish equilibrium at a fixed load level. The procedure has been implemented in

QSTAGS (early 1990’s version) and improved on each version since then (currently at STAGS Version

4.0, Rankin, et al., 2001).

For structures exhibiting changes in their deformation pattern as part of the nonlinear response, the 

analysis effort can exhibit convergence difficulties and even non-convergence may result. In some cases,

there is a mode change (or a mode jump), and equilibrium paths that are not statically connected may be

involved. These difficulties may be signaled by the nonlinear analysis in several forms depending on the

solution control procedure (load control, displacement control, or arc-length control) being used. One

signal indicating convergence problems regardless of the solution control procedure is a large number of

iterations and repeated step size reductions. Another signal is when the determinant of the stiffness

matrix tends to zero indicating a limit point in the nonlinear response. Another signal is the occurrence of 

more than one negative roots in the tangent stiffness matrix due to the nonlinear response (i.e., not

including negative roots due to Lagrangian constraints). In the past such problems have been called “drop

dead” problems because the solution procedure essentially “died” and further predictions were not

possible. However, Riks, Rankin and Brogan (1993, 1996) proposed a hybrid static-transient solution

procedure including load relaxation as a method to overcome these non-convergence issues.

The basic steps of the computational procedure are described as followed:

1. After defining the finite element model (geometry, discretization, material definitions, boundary

conditions, and loading), perform a basic linear elastic stress analysis to check out the overall response of 

the model.

2. Perform a linear buckling analysis for the loading system considered. This step helps the analyst

define the initial load level and starting load step size for the nonlinear analysis. The buckling mode 
212

shapes may be used individually or in a linear combination to form an initial geometric surface 

imperfection.

3. Perform a linear free vibration analysis of the structure to determine the lowest natural frequency of 

vibration. This value is used in the transient dynamic analysis to define the coefficients associated with

structural damping.

4. Perform a nonlinear static analysis. Examine the results to determine whether non-convergence 

occurred, whether convergence difficulties were encountered, or whether multiple negative roots from

decomposition of the “tangent” stiffness matrix.

5. If no difficulties encountered, then perform a restart of the nonlinear solution process and continue the 

nonlinear static analysis until difficulties are encountered or until the desired load level is reached.

6. If difficulties or multiple negative roots are encountered, then perform a nonlinear transient dynamic 

analysis with either a slight increase in load or with a slight initial velocity. The analyst needs to have

some insight into the nonlinear response in choosing this amplitude – too little and the solution will return

to a neighboring static equilibrium solution instead of “passing through” or “jumping to” a new

deformation mode.

7. Perform the nonlinear transient dynamic analysis using direct time integration methods for a given

time period. The length of this time period is somewhat arbitrary – in essence, until the inertial forces

become negligible. However, the definition of negligible is analyst dependent. The initial time step using

the implicit Park’s method of STAGS can be chosen using the vibration frequencies from the linear

vibration analysis. An initial time step size can be defined using

!

" = 2 t where ω is the frequency

associated with the highest anticipated vibration mode (i.e., perhaps the third or fourth value assuming the 

lowest four are global mode shapes).

8. Perform a load relaxation step for each of one or more steps from the transient dynamic solution

process. The load relaxation process computes a new right-hand-side “load” vector using the transient

solution for that step. This “load” vector represents the inertial forces due to accelerations and velocities.

In this case, these forces are the d’Alembert required to put the system in static equilibrium given the

displacements from the transient solution at the specified load step; these forces are applied so long as the

load factor PX on this new “load” vector is nonzero. Holding the applied external loads fixed, the load

factor PX is decremented from a value of unity, and nonlinear solutions for each decrement are obtained

until PX is zero. When PX is zero, static equilibrium is now re-established in a consistent, rigorous basis.

9. Once equilibrium is re-established, a restart of the nonlinear solution process is performed again until

another problem is encountered.

The postbuckling response of a curved cylindrical composite panel with a central cutout shown in Figure

69 and loaded by in-plane compression is studied. This configuration corresponds to Panel CP8 in Knight

and Starnes (1985). The curved panel is 14-inch-square projected-planform with a 15-inch radius. The 

curved panel is clamped along the curved edges and the straight edges are restrained using knife-edge

supports that simulate a near simple support condition. The cutout is a 2-inch-diameter circular cutout in

the panel center. Constraints are imposed along the top curved edge to enforce a uniform end-shortening

condition similar to the test conditions. The material is T300/5208 graphite-epoxy, and nominal material

data and geometry are defined on Figure 69 using U.S. customary units.
213

Figure 69. Compression-loaded curved panel: geometry and material properties.

Modeling and Analysis Process

The finite element model represents the entire panel with twelve shell units as shown in Figure 70. Eight

shell units are used to model a six-inch-square region surrounding the central circular cutout using the 

LAME user-written subroutine – this region will be referred to as the cutout region (see Knight, October

1999). Two shell units are used to model the full width of the panel across the top and bottom. Two

additional shell units are then used to complete the left and right sides of the panel adjacent to the cutout

region. The finite element mesh in the cutout region is more refined than the other regions using the E510

transition elements (automatic).

Figure 70. Finite element model of the curved panel with central circular cutout.

Panel Geometry:

L = 14.0 in.

S = 14.0 in.

R = 15.0 in.

a = 2.0 in.

Panel Material:

E11 = 19.6 Msi, E22 = 1.89 Msi

G12 = G13 = 0.93 Msi , G23 = 0.31 Msi

ν12 = 0.38

ρ = 2.59×10-5 slugs/in.

3

Panel Quasi-Isotropic Laminate:

[±45/90/02/90/m45]s

hply=0.0056 in.

R

L

t

a

X, u

Z, w

Y, v

S
214

Material properties and shell wall construction are defined using the GCP approach. Material modeling

using the current GCP approach requires data on the I-5a and I-6a records to define the material

properties and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the shell fabrication. The 16-ply

quasi-isotropic laminate has a [±45/90/02/90/ 45]s stacking sequence and an average ply thickness of 

0.0056 inches (based on measurements of the panel thickness). The value of the elastic modulus in the

fiber direction E11 is modified for the nonlinear postbuckling analysis in order to better correlate the initial

slope of the load-shortening curve (EA) with the value obtained from the test (EA=8,620,000 pounds).

As a result, a value of 18.4 Msi is used instead of 19.0 Msi.

Boundary condition on the displacements are specified using the P-1 and P-2 records. An applied end

displacement is specified across top curved edge (edge 3 on shell unit 12). The opposite curved end of

the panel (edge 1 of shell unit 10) is clamped. The right and left straight edges of the finite element

model (i.e., edge 2 of shell unit 9 and edge 4 of shell unit 11, respectively) have knife-edge boundary

conditions imposed (i.e., w=θy=0).

Numerical Results and Discussion

The panel was observed during the test to buckle into a local mode shape around the cutout. This local

mode shape was observed to be embedded within a more global deformation pattern at buckling. After

buckling two regions of local deformation were noted. Panel failure occurred at a load nearly six times the

buckling load in the test.

Linear buckling analysis is performed with four eigenvalues requested. The lowest buckling load is used

to establish the initial load level and initial solution step size for the nonlinear analysis. In addition, these 

four mode shapes are then used to form an initial geometric surface imperfection for the nonlinear 

analysis. Contour plots of the out-of-plane displacement component of the first four buckling mode 

shapes are shown in Figure 71. The buckling modes are scaled (5%, 1%, 0.5% and 0.5% times the panel

thickness) and then combined as a linear combination to form the initial geometric surface imperfection

as shown in Figure 72. Note that STAGS normalizes the buckling modes by the largest component in the

eigenvector (i.e., the largest components will correspond to ±1; typically an out-of-plane displacement

degree of freedom has the maximum value in many applications).

Nonlinear elastic analysis results and test results are shown on Figure 73. The end-shortening

displacement as a function of the applied compressive load is shown in Figure 73. The test results are 

indicated by the open square symbols, and the elastic postbuckling analysis results obtained using arclength control are shown by the open circles. Good correlation is shown for the assumed initial

imperfection shape and nominal elastic properties up to buckling. The static solution predicted using the 

arc-length control procedure proceeded through the unstable regions of the response with no more than

one negative root.

Nonlinear elastic results were also predicted using displacement control wherein the amplitude of the endshortening displacement is controlled. In this case, the unstable branches of the nonlinear response are 

not predicted. Instead, one or more negative roots are detected once the collapse load had been reached.

Hence, following an initial nonlinear static analysis, the results are reviewed and the analyst may chose to

start the transient response from any of the archived nonlinear static solutions. Examination of the 

archived solutions indicate that the sixth solution step had no negative roots and the seventh step had just

one negative root; however, there was a significant increase in load level between these solution steps.

Therefore, the analyst needs to either restart the nonlinear solution and perform a few more static steps to

more closely approach the collapse point, initiate the transient at step 6 with a high enough amplitude to

cause the collapse to occur, or to initiate the transient at step 7 with a small increase in amplitude to
215

trigger the collapse. The results shown in Figure 73 are obtained using step 7 to initiate the transient with

Δt=0.0001 sec. The values used for the damping parameters are based on the first fundamental frequency

from a linear free vibration analysis. The fundamental frequency π is 1434 hertz. The damping

parameters, assuming 0.1% critical damping, are: 5 1.11 10

2

2 901.3 and != = = = "

#$

% ' #$% &

Following the transient, a load relaxation step is performed automatically on a nonlinear restart to reestablish equilibrium and subsequent increase in loading to advance the nonlinear solution.
216

(a) Mode 1. (b) Mode 2.

(c) Mode 3. (d) Mode 4.

Figure 71. Contour plots of the out-of-plane displacement component

of the buckling mode shapes.
217

Figure 72. Contour plot of out-of-plane component of the initial geometric surface imperfection based on

a linear combination of the lowest four buckling mode shapes.

Figure 73. Load versus end-shortening results.

6% t

-1% t

0
218

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Advanced-Testcases/Type-D-Hybrid

The 2-D shell analysis model is defined using entirely shell units in combination with the LAME userwritten subroutine to model the circular cutout as a sequence of eight shell units (45-degrees each) around

the hole.

Typical Shell Element Model

cp8.inp (for S1 processor)

Curved panel with a central cutout - using LAME.F

$ R=15" R_hole=1", Total length=14", 16-ply laminate

$ local 3" region around cutout

$ 2-to-1 transition for other shell units

$ top and bottom units span 3 middle shell units

$ first 8 shell units model local region around cutout

$

$ Panel is 53.5-degrees in arc, R=15 in. and L=14 in.

$ with the origin of the coord sys at the cylinder

$ mid-length on its axis

$

$ 8 segments around hole (+/- 45 degrees) plus

$ additional segments on top and bottom and

$ on left and right (uniform spacing of mesh)

$

0 0 1 0 0 3 $B-1

1 20.0 / 2 30.0 / 3 90.0 $b-1b model rotations

12 0 0 8 12 0 4 $B-2 MODEL SUMMARY

0 0 0 0 0 1 $B-3 DATA TABLE SUMMARY - use GCP

C

C Define imperfections using buckling mode shapes

C

0.0044800 0 1 0 $b-5 5%*t for Mode 1

0.0008960 0 2 0 $b-5 1%*t for Mode 2

0.0000896 0 3 0 $b-5 0.1%*t for Mode 3

0.0000896 0 4 0 $b-5 0.1%*t for Mode 4

C

C define shell unit discretization (rows and columns)

C

21 11 11 21 11 21 21 11,

21 11 11 21 11 21 21 11,

11 6,

6 21,

11 6,

6 21

$ G-1--Please see documentation in LAME routine

1 2 2 3

2 1 3 3

3 1 4 4

4 2 5 4

5 2 6 3

6 1 7 3

7 1 8 4

1 4 8 2
219

$g-2 combine segments with hole to other cylinder units

$ do the left side

2 0 21 0 9 0 1 0 1 11 2 6 11 1 $g-2

3 0 21 0 9 0 1 0 1 11 2 1 6 1 $g-2

$ do the bottom

4 21 0 0 10 6 0 0 1 11 2 16 11 -1 $g-2

5 21 0 0 10 6 0 0 1 11 2 11 6 -1 $g-2

$ do the right side

6 0 21 0 11 0 6 0 1 11 2 6 1 -1 $g-2

7 0 21 0 11 0 6 0 1 11 2 11 6 -1 $g-2

$ do the top

8 21 0 0 12 1 0 0 1 11 2 6 11 1 $g-2

1 21 0 0 12 1 0 0 1 11 2 11 16 1 $g-2

$

$ now connect outer shell units together

$ left side

9 1 0 0 10 6 0 0 1 6 1 16 21 1 $g-2

9 11 0 0 12 1 0 0 1 6 1 16 21 1 $g-2

$ right side

10 6 0 0 11 1 0 0 1 6 1 1 6 1 $g-2

11 11 0 0 12 1 0 0 1 6 1 1 6 1 $g-2

$

C ----------------------------------------------------------------

C

C 16-PLY QUASI-ISOTROPIC LAMINATE [pm45/90/0/0/90/mp45]_s

C

ORTHOELAST_MATERIAL 1 1 1 $I-5A GCP COMMAND RECORD

18.4E+6 1.89E+6 1.89e+6, $I-7A E1, E2, E3=E2

0.93E6 0.93E6 0.93E6, $I-7A G12,G13=G12, G23=G12

0.38 0.38 0.38, $I-7A NU12, NU13=NU12, NU23=NU12

2.59E-5, $I-7A MASS DENSITY

0.0 0.0 0.0 , $I-7A CTE'S

0.0 0.0 0.0 , $I-7A CME'S

0.0 0.0 $I-7A REF. TEMP AND REF. MOISTURE CONTENT

C

C 16-PLY QUASI-ISOTROPIC LAMINATE

C

ORT_EL_BR 2 1 1 $I-5A GCP COMMAND RECORD

18.4E+6 1.89E+6 1.89e+6, $I-7A E1, E2, E3=E2

0.93E6 0.93E6 0.93E6, $I-7A G12,G13=G12, G23=G12

0.38 0.38 0.38, $I-7A NU12, NU13=NU12, NU23=NU12

2.59E-5, $I-7A MASS DENSITY

0.0 0.0 0.0 , $I-7A CTE'S

0.0 0.0 0.0 , $I-7A CME'S

0.0 0.0 , $I-7A REF. TEMP AND REF. MOISTURE CONTENT

0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0, $i-7a allowable strains

165.e+3 200.e+3 27.41e+3 11.74e+3 27.41e+3 11.74e+3, $i-7a allowable

9.0e+3 9.0e+3 10.0e+3, $i-7a allowable shears

0.8e-14 0.0 -1.0e-3 1 1, $i-7a alpha, F12, beta, ifail idgrd

3*0.0 $i-7a visf0, visf1, visff

C

SHELL_FABRICATION 1 16 0 1 0 $I-5A 24-PLY LAMINATE

16*1 $I-21A T300/5208 MATID

16*0.0056 $I-21C LAYER THICKNESSES

+45.0 -45.0 90.0 0.0 0.0 90.0 -45.0 +45.0 , $i-21d

+45.0 -45.0 90.0 0.0 0.0 90.0 -45.0 +45.0 $i-21d

1.0 1.0 $I-21E SHEAR CORRECTION FACTORS

C

SHELL_FABRICATION 2 16 1 1 0 $I-5A 16-PLY LAMINATE

16*2 $I-21A T300/5208 MATID

16*1 $I-21B SHELL INTEGRATION POINTS PER LAYER

16*0.0056 $I-21C LAYER THICKNESSES

+45.0 -45.0 90.0 0.0 0.0 90.0 -45.0 +45.0 , $i-21d
220

+45.0 -45.0 90.0 0.0 0.0 90.0 -45.0 +45.0 $i-21d

1.0 1.0 $I-21E SHEAR CORRECTION FACTORS

END $I-5A END GCP INPUT

C --------------------------------------------------------------

C

C generate 45-degree wedges around the hole in a

C counter-clockwise manner starting at "Noon"

C

C --------------------------------------------------------------

$ UNIT 1

C --------------------------------------------------------------

1 0/1. 3.0 +11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 0 1 0

3 6 6 6

0 $q-1 no loads - interior unit

0 0 0 0 $r-1

C --------------------------------------------------------------

$ UNIT 2

C --------------------------------------------------------------

1 0/-1. 3.0 +11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 1 0 0

6 6 6 3

0 $q-1 no loads - interior unit

0 0 0 0 $r-1

C --------------------------------------------------------------

$ UNIT 3

C --------------------------------------------------------------

1 0/-1. -3.0 +11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 1 0 0

6 6 6 3

0 $q-1 no loads - interior unit

0 0 0 0 $R-1

C --------------------------------------------------------------

$ UNIT 4

C --------------------------------------------------------------

1 0/1. -3.0 -11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 0 1 0

3 6 6 6

0 $q-1 no loads - interior unit

0 0 0 0 $r-1

C --------------------------------------------------------------

$ UNIT 5

C --------------------------------------------------------------

1 0/1. -3.0 +11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 0 1 0

3 6 6 6

0 $q-1 no loads - interior unit

0 0 0 0 $r-1

C --------------------------------------------------------------

$ UNIT 6

C --------------------------------------------------------------

1 0/-1. 3.0 -11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 1 0 0

6 6 6 3

0 $q-1 no loads - interior unit

0 0 0 0 $r-1

C --------------------------------------------------------------
221

$ UNIT 7

C --------------------------------------------------------------

1 0/-1. -3.0 -11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 1 0 0

6 6 6 3

0 $q-1 no loads - interior unit

0 0 0 0 $r-1

C --------------------------------------------------------------

$ UNIT 8

C --------------------------------------------------------------

1 0/1. 3.0 -11.46 1.0 15.0

-1

410 0 0 0 1 0 0 0 0 1 0

3 6 6 6

0 $q-1 no loads - interior unit

0 0 0 0 $r-1

C --------------------------------------------------------------

$ unit 9 left side of shell

C --------------------------------------------------------------

5 0 $M-1

-3.0 3.0 11.46 26.74 15.0 $m-2

-1 $m-5 shell wall fabrication

410 0 0 $n-1

6 0 6 6 $p-1

110 101 $p-2 knife edge BC at theta=+60 deg

0 $q-1 no load

0 0 $r-1

C --------------------------------------------------------------

$ unit 10 bottom of shell

C --------------------------------------------------------------

5 0 $M-1

-7.0 -3.0 -26.74 26.74 15.0 $m-2

-1 $m-5 shell wall fabrication

410 0 3 $n-1

15.28 22.92 15.28 $n-5 y-segment lengths

5 10 5 $n-6 y-segment spacing

2 0 6 0 $p-1 clamped at x=-6

110 101 $p-2 knife edge BC at theta=+60 deg

110 101 $p-2 knife edge BC at theta=-60 deg

0 $q-1 no load

0 0 $r-1

C --------------------------------------------------------------

$ unit 11 right side of shell

C --------------------------------------------------------------

5 0 $M-1

-3.0 3.0 -26.74 -11.46 15.0 $m-2

-1 $m-5 shell wall fabrication

410 0 0 $n-1

6 6 6 0 $p-1

110 101 $p-2 knife edge BC at theta=-60 deg

0 $q-1 no load

0 0 $r-1

C --------------------------------------------------------------

$ unit 12 top of shell

C --------------------------------------------------------------

5 0 $M-1

3.0 7.0 -26.74 26.74 15.0 $m-2

-1 $m-5 shell wall fabrication

410 0 3 $n-1

15.28 22.92 15.28 $n-5 y-segment lengths

5 10 5 $n-6 y-segment spacing

6 0 0 0 $p-1
222

110 101 $p-2 knife edge BC at theta=+60 deg

100 000 $p-2 clamped except for applied u_0 at x=+6

110 101 $p-2 knife edge BC at theta=+60 deg

1 $q-1 applied end shortening

1 1 $q-2

-0.01 -1 1 6 0 $ q-3 applied u_0 across top at x=+6

0 0 0 0 0 0 1 $r-1

6 0 $r-2 selective displacements across the top

cp8.bin (for S2 processor)

This file contains the S2 input records for all the analyses performed on the panel (buckling, vibration,

nonlinear static, transient dynamics, and nonlinear restart with load relaxation). Only the first set of 

commands is executed even though all records are read and echoed on input. In this manner, a record of

all the analyses performed can be maintained in a single file.

Curved panel with central cutout - applied end shortening $a-1

C

C Nonlinear static restart after transient

C with load relaxation as a first step

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

4.2 0.1 8.0 $C-1 LOAD MULTIPLIERS

422 4000 5 -20 1 1.0e-4 1.0 $d-1 strategy parameters

5 0 1 $et-1 do load relaxation and use previous solution as estimate

C

C Nonlinear transient dynamic solution control from static solution

C

6 1 0 0 0 0 0 -1 $b-1

4.14375 0.0 4.14375 $c-1

7 4000 10 -20 0 1.0e-4 $d-1

0.0 20.0 1.0e-4 100.0 901.335 1.11e-5 $e-1

0 4 1 0 0 1 0 $e-2

4.20 0.0 0.0 1000.0 1000.0 0.0 $e-3

C

C Nonlinear analysis - displ control

C

3 1 0 0 0 0 0 -1

1.0 0.2 8.0 $c-1

0 8000 10 -20 1 1.0e-4 $d-1

0 0 3 $et-1

C

C Nonlinear analysis - arc length control

C

3 1 0 0 0 0 0 -1

1.0 0.2 8.0 $c-1

0 8000 10 -20 0 1.0e-4 $d-1

0 0 3 $et-1

C

C Linear buckling analysis

C

1 1 1 0 0 0 0 -1 $b-1

1. 0. 1. $c-1

1000 1.0e-4 $d-2

4 $d-3

C

C Nonlinear static restart after transient

C with load relaxation as a first step

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

4.50 0.1 8.0 $C-1 LOAD MULTIPLIERS

420 1000 5 20 1 1.0e-4 1.0 $d-1 strategy parameters

5 0 1 $et-1 do load relaxation and use previous solution as estimate
223

C

C Restart nonlinear analysis

C

3 1 0 0 0 0 0 -1

4.0 1.0 8.0 $c-1

28 8000 10 -20 0 1.0e-4 $d-1

0 0 3 $et-1

C

C Free vibration analysis

C

2 1 0 0 0 0 0 -1

1. 0. 1.

1000 1.0e-4 $d-2

4 $d-3

cp8.pin (for STAPL processor)

Curved panel with central cutout $A-1

10 0 1 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C

C displacement plots for linear solution

C

2 0 1 0 0 0 0 1 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

2 0 1 0 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

2 0 1 0 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

C

C stress resultant plots for linear solution

C

2 0 5 0 0 0 0 1 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

2 0 5 0 0 0 0 2 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

2 0 5 0 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

C

C buckling modes

C

2 0 4 0 1 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

2 0 4 0 2 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP
224

0.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

2 0 4 0 4 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0

2 30.0

3 90.0

C

C Nonlinear solution displacement plots

C

2 0 1 6 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 9 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 50 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 100 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 200 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 300 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 400 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 424 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

2 0 1 428 0 0 0 3 $PL-3 KPLOT,NUNIT,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 $PL-5 DSCALE,NROTS,LWSCALE

1 20.0 / 2 30.0 / 3 90.0

Problem References

Hilburger, M. W. and Starnes, J. H., Jr., “Effects of Imperfections on the Buckling Response of 

Compression-Loaded Composite Shells,” International Journal of Non-Linear Mechanics, Vol. 37, Nos.

4-5, June-July 2002, pp. 623-643.

Stein, M., The Phenomenon of Change in Buckle Pattern in Elastic Structures, NASA Technical Report

R-39, 1959.

Supple, W. J., “Couple Branching Configurations in the Elastic Buckling of Symmetric Structural

Systems,” International Journal of Mechanical Sciences, Vol. 9, No. 2, 1967, pp. 97-112.

Supple, W. J., “On the Change in Buckle Pattern of Elastic Structures,” International Journal of

Mechanical Sciences, Vol. 10, 1968, pp. 737-745.
225

Supple, W. J., “Changes of Wave-Form of Plates in the Post-Buckling Range,” International Journal of

Solid and Structures, Vol. 6, No. 9, 1970, pp. 1243-1258.

Riks, E, Rankin, C. C., and Brogan, F. A., The Numerical Simulation of the Collapse Process of Axially 

Compressed Cylindrical Shells with Measured Imperfections, Delft University of Technology, Faculty of 

Aerospace Engineering, Report No. LR-705, 1993.

Riks, E, Rankin, C. C., and Brogan, F. A., “On the Solution of Mode Jumping Phenomena in Thin-Walled

Shell Structures,” Computer Methods in Applied Mechanics and Engineering, Vol. 136, Nos. 1-2,

September 1996, pp. 59-92.

Riks, E. and Rankin, C. C., “Computer Simulation of the Buckling Behavior of Thin Shells Under QuasiStatic Loads,” Archives of Computational Methods in Engineering, Vol. 4, No. 4, 1997, pp. 325-351.

Tiwari, N. and Hyer, M. W., “Secondary Buckling of Compression-Loaded Composite Plates,” AIAA

Paper No. 96-1626-CP, April 1996.

Tiwari, N. and Hyer, M. W., “Secondary Buckling of Laminated Composite Plates,” AIAA Paper No.

2000-1457, April 2000.

Fujii, F., Noguchi, H., and Ramm, E., “Static Path Jumping to Attain Postbuckling Equilibria of a 

Compressed Circular Cylinder,” Computational Mechanics, Vol. 26, No. 3, September 2000, pp. 259-

266.

Everall, P. R. and Hunt, G. W., “Mode Jumping in the Buckling of Struts and Plates: A Comparative

Study,” International Journal of Non-Linear Mechanics, Vol. 35, No. 6, November 2000, pp. 1067-1079.

Godoy, Luis A., Theory of Elastic Stability – Analysis and Sensitivity, Taylor and Francis, Philadelphia,

PA, 2000, Chapter 14.

Knight, N. F., Jr. and Starnes, J. H., Jr., “Postbuckling Behavior of Axially Compressed Graphite-Epoxy

Panels with Circular Holes,” ASME Journal of Pressure Vessel Technology, Vol. 107, No. 4, November 

1985, pp. 394-402.

Hilburger, M. W., Numerical and Experimental Study of the Compression Response of Composite 

Cylindrical Shells with Cutouts, Ph.D. Dissertation, Department of Aerospace Engineering, Univeristy of 

Michigan, Ann Arbor, MI, 1998.

Hilliburger, M. W., Britt, V. O., and Nemeth, M. P., “Buckling Behavior of Compression-Loaded QuasiIsotropic Curved Panels with a Circular Cutout,” International Journal of Solids and Structures, Vol. 38,

2001, pp. 1495-1522.

Ambur, D. R., Jaunky, N., Davila, C. G., and Hilburger, M. W., “Progressive Failure Studies of 

Composite Panels with and without Cutouts,” AIAA Paper No. 2001-1182, April 2001.

Knight, Norman F., Jr., Enhancement of STAGS Progressive Failure Capability, Contract No. GS-35F4503G, Final Report for MRJ Task 1410, October 1999.
226

Progressive Failure Analysis of Postbuckled Shear Panel

Background

Thin-walled plates and shells often can carry loads well in excess of its buckling load determined from a 

linear bifurcation buckling analysis. The structural response for load levels below the buckling load is

referred to as the primary solution or pre-buckling solution. It may be linear or nonlinear. Above the 

buckling load, the response is referred to as postbuckling behavior when the response is stable and

collapse when the response is unstable. For these structures, the analyst needs to examine the role initial

geometry imperfections and “generalized” imperfections if possible. Generalized imperfections include 

to surface imperfections, thickness variations, variations in lamination, fabrication inconsistencies,

eccentricities in loading, and other aspects that cause the structure, its boundary conditions, and its

loading to be less than ideal (e.g., see Hilburger and Starnes, 2002).

In addition local material failures may initiate and then propagate – progressive failure. Nonlinear finite 

element analyses accounting for such behavior are quire computationally intense due to the large number 

of material points that need to be examined for one or more failure modes. Recent works on postbuckled

panels exhibiting a progressive failure response include Knight, Rankin, and Brogan (2000, 2001, 2002),

Ambur, Jaunky, Davila, and Hilburger (2001), Ambur, Jaunky, and Hilburger (2002), Engelstad, Reddy

and Knight (1992), Sleight, Knight and Wang (1997), and Baranski and Biggers (1999).

The postbuckling response of a flat composite panel loaded by in-plane shear shown in Figure 74 is

studied. This configuration corresponds to Panel B2 tested by Rouse (1985a,b). The panel is 12-inches

square and is clamped along all edges in a picture-frame test fixture. The corners are pinned so that a 

uniform diagonal-tension field develops prior to buckling. Constraints are imposed on the edges to keep

the edges straight and yet allow the edges to rotate about a normal to the plane. The material is AS4/3502

graphite-epoxy, and the nominal material data and geometry are defined on Figure 74 using U.S.

customary units and SI units.
227

Figure 74. In-plane-shear-loaded flat panel: geometry and material properties.

Modeling and Analysis Process

The finite element model represents the entire panel with fifty 4-node E410 shell elements along each

coordinate direction resulting in a total of 2500 4-node shell elements to model the entire panel. This

finite element model is shown in Figure 75. The test fixture is not explicitly modeled; however, a series of 

constraints enforce a picture-frame-type in-plane loading. The behavior predicted by the finite element

model is consistent with the test results.

Material properties and shell wall construction are defined using the GCP approach.. Material modeling

using the current GCP approach requires data on the I-5a and I-6a records to define the material

properties and records I-5a, I-21a, I-21b, I-21c, I-21d, and I-21e to define the shell fabrication. The 16-ply

quasi-isotropic laminate has a [±45/0/90]2s stacking sequence and an average ply thickness of 0.005702

inches (based on measurements of the panel thickness). The progressive failure analysis will consider 

each layer to be represented individually with only a single integration point per layer. The E410 element

has four surface-integration point and hence the number of material points to be examined for damage is

given by the product of the number of elements which may experience damage (i.e., those elements with

an ORT_EL_BR GCP material type), the number of surface-integration points per element (i.e., INTEG

parameter on the N-1 record), the number of layers in the laminate (i.e., NLAYERS on the I-21a record),

and the number of through-the-thickness integration points per layer (i.e., INTSHL on the I-21b record).

For this finite element model of the square flat shear panel, the resulting multiplication corresponds to

2500×4×1×16 for a total of 160,000 material points.

Panel Geometry:

L = 12.0 in.

Panel Material:

E11 = 18.53 Msi, E22 = 1.60 Msi

G12 = G13 = 0.87 Msi , G23 = 0.258 Msi

ν12 = 0.3

XT=232.75 ksi, XC=210.0 ksi

YT=14.7 ksi, YC=28.7 ksi

S=29.75 ksi

Panel Quasi-isotropic Laminate:

[±45/0/90]2s

hply=0.005702 in.

L L

T

Rigid rails with pin

connections simulating

a picture-frame fixture
228

Figure 75. Finite element model of a shear panel using a 50×50 mesh of 4-node shell elements.

Boundary condition on the displacements are specified using the P-1 and P-2 records. An applied end

displacement is specified across edge 1 on shell unit 1. The opposite end of the panel is clamped, the

right edge of the finite element model is free, and the left edge has symmetric conditions imposed.

The edges of the panel are constrained to remain straight. Lagrangian constraints are written across the 

edge 1 (x=0) such that a linear variation in both in-plane displacement components results. Along row 1,

the displacements vary linearly from zero at column 1 up to their values at column 51 (i.e., assuming a

model with 51 rows and 51 columns of nodes). Similar constraints are written along row 51 or edge 3.

Partial compatibility constraints are defined along edge 2 that define uniform u and v displacements

across that edge.

Numerical Results and Discussion

The panel was observed during the test to buckle into three halfwaves transverse to the diagonal-loading

direction and one halfwave in the diagonal-loading direction. The diagonal-tension load at buckling Tcr

and the diagonal load at failure are reported by Rouse (1985) to be 9,642 lbs. and 54,808 lbs. (5.68 Tcr),

respectively. Rouse (1985) reported failure initiation along the fixture edges and then along the main

diagonal of the panel where a severe displacement gradient developed. Panel failure occurred at a load

nearly six times the buckling load in the test.

The analytical buckling load for this STAGS finite element model corresponds to a diagonal-tension load

of 8,319 lbs. using nominal mechanical properties and NLIP equal to three (a value of 8,284 lbs is

obtained for NLIP=1). Contour plots of the out-of-plane displacement component of the buckling mode 

shapes corresponding to the lowest two eigenvalues in shown in Figure 76. To initial the nonlinear

postbuckling response for the flat panel, an initial geometric surface imperfection was generated using the
229

first buckling mode shape with a maximum amplitude equal to five percent of the panel thickness as

shown in Figure 77. Note that STAGS normalizes the buckling modes by the largest component in the

eigenvector (i.e., the largest components will correspond to ±1; typically an out-of-plane displacement

degree of freedom has the maximum value in many applications).

Nonlinear elastic analysis results and test results are shown on Figure 78. The out-of-plane displacement

near the panel center normalized by the panel thickness as a function of the diagonal tension load is

shown in Figure 78. The solid curve represents the test results and the elastic postbuckling analysis

results are shown as a dashed curve. Good correlation is shown for the assumed initial imperfection

shape and nominal elastic properties.

Nonlinear PFA analysis results were obtained using the maximum strain criteria and a small amount of

artificial viscous damping. The out-of-plane displacement near the panel center normalized by the panel

thickness as a function of the diagonal tension load is shown in Figure 78. Buckling occurs very early,

and as the diagonal-tension load continues to increase, the buckles deep and the panel stiffens. Damage 

initiation (matrix tension failures) occurs at a diagonal-tension load of 44,324 lbs. (Step 21) in the 

corners. Damage progresses in the loaded diagonal corners first as shown in Figure 79. The plateau in

load shown in Figure 78 is due to a rapid growth in damage along the edges near the corners. After some

load redistribution, the load reaches a plateau at a value of 53,976 lbs. (Step 35). Along this plateau,

damage propagates along the center buckle crest (Step 44). As the solution process continues, the extent

of damage increases (i.e., more damage through the thickness) and grows toward the opposite corners.

This process is a slow process numerically as the material nonlinearity develops due to local discrete

changes in material stiffness. Increasing the amount of artificial viscous damping may accelerate the

process without changing the overall panel response.

A sequence of deformed geometry plots showing the percent ply damage by element is given in Figure 

79. As mentioned previously, damage initiates in the loaded corners of the panel and first progresses

along the edges before damage initiates along the crest of the center buckle. Damage grows along the 

center buckle crest and then transverse to the buckle crest until the computations are stopped.
230

(a) Mode 1 at 8,319 lbs.

(b) Mode 2 at 9,529 lbs.

Figure 76. Contour plots of the out-of-plane displacement component of the buckling mode shapes.

+1.0

-1.0
231

Figure 77. Contour plot of the initial surface imperfection formed from the first buckling mode shape 

with a maximum amplitude of 5% of the panel thickness.

Figure 78. Diagonal-tension load versus out-of-plane deflection near panel center.

5.0% t

-0.5% t

0
232

Figure 79. Percent ply points with damage for selected solution steps obtained using the maximum strain

criteria. Total number of material points is 160,000.

(a) Step 35 (52,976 lbs.) has 110

elements with damage (1,158

ply points)

c) Step 112 (55,358 lbs.) has

444 elements with damage

(5,329 ply points)

d) Step 395 (57,387 lbs.) has

687 elements with damage

(9,060 ply points)

(b) Step 44 (53,916 lbs.) has

324 elements with damage

(2,945 ply points)

Percent Ply 

Points with 

Damage

100%

0%
233

Figure 80. Contour plot of the out-of-plane deflection pattern for a solution step at the end of the 

simulation.

The deformation pattern of the postbuckled panel due to the in-plane shear loading is shown in Figure 80.

The pattern has three halfwaves transverse to the diagonal tension loading and one halfwave along the

diagonal tension loading direction.

STAGS Input Files

These STAGS input files are located under the following subdirectory:

$STAGSHOME/Advanced-Testcases/Type-D-PFA

Typical Shell Element Model

b2.inp (for S1 processor)

Rouse B2 Panel with picture frame fixture and in-plane shear $a-1

C

C Rouse, M., "Postbuckling of flat unstiffened graphite-epoxy

C plates in shear,", AIAA Paper No. 85-0771-CP, 1985.

C

0 0 1 0 0 0 0 $B-1 ANALYSIS TYPE

CC 3 45.0 $b-1b

1 1 0 0 5 -98 1 $B-2 MODEL SUMMARY

1 0 0 0 0 1 $B-3 DATA TABLE SUMMARY -> use gcp

0.45616E-2 0 1 0 $B-5 buckling mode imperfection 5% * thick * Mode 1

$ h=0.09123=16*0.005702

51 51 $F-1 GRID SUMMARY

1 1 51 1 1 0 51 1 $G-2 Keep Top edge straight--all U's the same

1 1 51 2 1 0 51 2 $G-2 Keep Top edge straight -- all V's the same

1 1 51 1 2 2 0 1 $G-2 At pin, force local node translations to be

$ equal, use rigid link to simulate beam

1 1 51 2 2 2 0 2 $G-2 --V

1 1 51 3 2 2 0 3 $ -- W

$ Keep left edge straight (x = 0, boundary line 1), but allow line

$ to rotate -- U and V handled simultaneously

2 2 0 0 0 1

3.2 t

0

- t
2

34

11511.02e50

1121-1.e50

220001

11511.04e50

1131-1.e50

220001

11511.06e50

1141-1.e50

220001

11511.08e50

1151-1.e50

220001

11511.1e50

1161-1.e50

220001

11511.12e50

1171-1.e50

220001

11511.14e50

1181-1.e50

220001

11511.16e50

1191-1.e50

220001

11511.18e50

11101-1.e50

220001

11511.2e50

11111-1.e50

220001

11511.22e50

11121-1.e50

220001

11511.24e50

11131-1.e50

220001

11511.26e50

11141-1.e50

220001

11511.28e50

11151-1.e50

220001

11511.3e50

11161-1.e50

220001

11511.32e50

11171-1.e50

220001

11511.34e50

11181-1.e50

220001

11511.36e50

11191-1.e50

220001

11511.38e50

11201-1.e50

220001

11511.4e50

11211-1.e50

220001

11511.42e50

11221-1.e50

220001
2

35

11511.44e50

11231-1.e50

220001

11511.46e50

11241-1.e50

220001

11511.48e50

11251-1.e50

220001

11511.5e50

11261-1.e50

220001

11511.52e50

11271-1.e50

220001

11511.54e50

11281-1.e50

220001

11511.56e50

11291-1.e50

220001

11511.58e50

11301-1.e50

220001

11511.6e50

11311-1.e50

220001

11511.62e50

11321-1.e50

220001

11511.64e50

11331-1.e50

220001

11511.66e50

11341-1.e50

220001

11511.68e50

11351-1.e50

220001

11511.7e50

11361-1.e50

220001

11511.72e50

11371-1.e50

220001

11511.74e50

11381-1.e50

220001

11511.76e50

11391-1.e50

220001

11511.78e50

11401-1.e50

220001

11511.8e50

11411-1.e50

220001

11511.82e50

11421-1.e50

220001

11511.84e50

11431-1.e50

220001
236

1 1 51 1 .86e5 0

1 1 44 1 -1.e5 0

2 2 0 0 0 1

1 1 51 1 .88e5 0

1 1 45 1 -1.e5 0

2 2 0 0 0 1

1 1 51 1 .9e5 0

1 1 46 1 -1.e5 0

2 2 0 0 0 1

1 1 51 1 .92e5 0

1 1 47 1 -1.e5 0

2 2 0 0 0 1

1 1 51 1 .94e5 0

1 1 48 1 -1.e5 0

2 2 0 0 0 1

1 1 51 1 .96e5 0

1 1 49 1 -1.e5 0

2 2 0 0 0 1

1 1 51 1 .98e5 0

1 1 50 1 -1.e5 0

$ Keep right edge straight, same as above except for face #3

2 2 0 0 0 1

1 51 51 1 .02e5 0

1 51 2 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .04e5 0

1 51 3 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .06e5 0

1 51 4 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .08e5 0

1 51 5 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .1e5 0

1 51 6 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .12e5 0

1 51 7 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .14e5 0

1 51 8 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .16e5 0

1 51 9 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .18e5 0

1 51 10 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .2e5 0

1 51 11 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .22e5 0

1 51 12 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .24e5 0

1 51 13 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .26e5 0

1 51 14 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .28e5 0

1 51 15 1 -1.e5 0
2

37

220001

151511.3e50

151161-1.e50

220001

151511.32e50

151171-1.e50

220001

151511.34e50

151181-1.e50

220001

151511.36e50

151191-1.e50

220001

151511.38e50

151201-1.e50

220001

151511.4e50

151211-1.e50

220001

151511.42e50

151221-1.e50

220001

151511.44e50

151231-1.e50

220001

151511.46e50

151241-1.e50

220001

151511.48e50

151251-1.e50

220001

151511.5e50

151261-1.e50

220001

151511.52e50

151271-1.e50

220001

151511.54e50

151281-1.e50

220001

151511.56e50

151291-1.e50

220001

151511.58e50

151301-1.e50

220001

151511.6e50

151311-1.e50

220001

151511.62e50

151321-1.e50

220001

151511.64e50

151331-1.e50

220001

151511.66e50

151341-1.e50

220001

151511.68e50

151351-1.e50

220001

151511.7e50

151361-1.e50
238

2 2 0 0 0 1

1 51 51 1 .72e5 0

1 51 37 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .74e5 0

1 51 38 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .76e5 0

1 51 39 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .78e5 0

1 51 40 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .8e5 0

1 51 41 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .82e5 0

1 51 42 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .84e5 0

1 51 43 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .86e5 0

1 51 44 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .88e5 0

1 51 45 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .9e5 0

1 51 46 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .92e5 0

1 51 47 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .94e5 0

1 51 48 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .96e5 0

1 51 49 1 -1.e5 0

2 2 0 0 0 1

1 51 51 1 .98e5 0

1 51 50 1 -1.e5 0

$

$ H - 1 Element unit for single rigid link

$

2 1

1 0 0 $i-1

1.0E+7 0.3 $i-2

C ----------------------------------------------------------------

C Material Data for AS4/3502 Graphite Epoxy

C

C Elastic data only

C

ORTHOELAST_MATERIAL 1 1 1 $ I-5A GCP COMMAND RECORD

1.853E7 1.6E6 1.67E6, $ I-10A E1, E2, E3

8.7E5 8.7E5 2.58E5, $ I-10A G12, G13, G23

0.30 0.30 0.30, $ I-10A NU12, NU13, NU23

1.54e-4, $ I-10A MASS DENSITY

0.0 0.0 0.0 , $ I-10A CTE'S

0.0 0.0 0.0 , $ I-10A CHE'S

0.0 0.0 $I-7A REF. TEMP AND REF. MOISTURE CONTENT

C

C Elastic data and PFA data for traditional failure criteria
239

C

ORT_EL_BR 2 1 1 $ I-5A GCP COMMAND RECORD

1.853E7 1.6E6 1.67E6, $ I-10A E1, E2, E3

8.7E5 8.7E5 2.58E5, $ I-10A G12, G13, G23

0.30 0.30 0.30, $ I-10A NU12, NU13, NU23

1.54e-4, $ I-10A MASS DENSITY

0. 0. 0. 0. 0. 0. 0. 0., $ I-10A CTEs, CHEs, RT, RM

0.0 0.0 0.0 0.0 0.0, $ I-10A E1C, E1T, E2C, E2T, GAMMAF

0.0 0.0 0.0 0.0, $ I-10A E3C, E3T, GAM23F, GAM13F

210000. 232750., $ I-10A Xc, Xt

28700. 14700, $ I-10A Yc, Yt

29750., $ I-10A Sxy

28700. 14700., $ I-10A Zc, Zt

29750. 29750., $ I-10A Syz, Sxz

0.0 0.0 -1.E-6 1 1, $ I-10A alpha, F12, beta, IFAIL, IDGRD

1.0 1.0e-9 1.0e-4 $ I-10a visf0, visf1, visff

C

C 8-PLY [(pm45)_2]_s LAMINATE (Panel A2)

C

SHELL_FABRICATION 1 8 0 1 0 $ I-5A 8-PLY SYMMETRIC LAMINATE

8*1 $ I-21A MATID

8*0.005123 $ I-21C Layer thickness

+45.0 -45.0 +45.0 -45.0 , $ I-21D FAB. ORIENTATION ANGLES

-45.0 +45.0 -45.0 +45.0 $ I-21D FAB. ORIENTATION ANGLES

1.0 1.0 $I-21E SHEAR CORRECTION FACTORS

C

C 16-PLY [(pm45/0/90)_2]_s LAMINATE (Panel B2)

C

SHELL_FABRICATION 2 16 1 1 0 $I-5A 16-PLY SYMMETRIC LAMINATE

16*2 $I-21A MATID

16*1 $I-21A Number of layer integration points

16*0.005702 $I-21C LAYER THICKNESSES

+45.0 -45.0 0.0 90.0 , $I-21D

+45.0 -45.0 0.0 90.0 , $I-21D

90.0 0.0 -45.0 +45.0, $i-21d

90.0 0.0 -45.0 +45.0 $i-21d

1.0 1.0 $I-21E SHEAR CORRECTION FACTORS

SHELL_FABRICATION 3 16 0 1 0 $I-5A 16-PLY SYMMETRIC LAMINATE

16*1 $I-21A MATID

16*0.005702 $I-21C LAYER THICKNESSES

+45.0 -45.0 0.0 90.0 , $I-21D

+45.0 -45.0 0.0 90.0 , $I-21D

90.0 0.0 -45.0 +45.0, $i-21d

90.0 0.0 -45.0 +45.0 $i-21d

1.0 1.0 $I-21E SHEAR CORRECTION FACTORS

C

C 24-PLY [(pm45/0/90)_3]_s LAMINATE (Panel C4)

C

SHELL_FABRICATION 4 24 0 1 0 $I-5A 24-PLY SYMMETRIC LAMINATE

24*1 $I-21A MATID

24*0.005376 $I-21C LAYER THICKNESSES

+45.0 -45.0 0.0 90.0 , $I-21D

+45.0 -45.0 0.0 90.0 , $I-21D

+45.0 -45.0 0.0 90.0 , $I-21D

90.0 0.0 -45.0 +45.0, $i-21d

90.0 0.0 -45.0 +45.0, $i-21d

90.0 0.0 -45.0 +45.0 $i-21d

1.0 1.0 $I-21E SHEAR CORRECTION FACTORS

C

END $I-5A END GCP INPUT

C --------------------------------------------------------------

2 0 $M-1 SHELL SURFACE DEFINITION - RECTANGULAR PLATE

0.0 12.0 0.0 12.0 $M-2 12-IN BY 12-IN. PLATE
240

-2 0 $M-5 SHELL WALL SELECTION -> USE GCP

410 0 0 $N-1 ELEMENT SELECTION, UNIFORM MESH

0 0 0 0 $P-1 BOUNDARY CONDITIONS GIVEN (0=FIXED; 1=FREE)

110 000 $P-2 X=0 EDGE

110 000 $P-2 Y=12 EDGE

110 000 $P-2 X=12 EDGE

000 000 $P-2 Y=0 EDGE

1 0 0 $Q-1 LOADING

1 1 0 $Q-2 LOAD SET

+5882.5094 1 1 1 51 0 $Q-3 Force component along +X axis

CC +0.0226239 -1 1 1 51 0 $Q-3 Displ component along +X axis

0 0 0 0 0 0 1 $R-1 OUTPUT FLAGS

0 51 $R-2 SELECTED OUTPUT ACROSS COLUMN 51

C

C One Rigid Link:

1 3*0 3*0. 000 001 $S-1

2 3*0 0. 12. 0. 110 001 $S-1

1 2 1 120 0

1.e3

0

0 0 0 0 0 0

b2.bin (for S2 processor)

Rouse shear panels with picture frame - Panel B2 $A-1

C nonlinear analysis options

3 1 0 4*0 -1 $b-1

0.50 .1 8.0 $c-1

0 8000 10 -20 0 1.e-4 $d-1

0 0 3 $et-1

c buckling analysis options

1 1 0 4*0 -1 $b-1

1.0 1.0 1.0 $c-1

1000 1.0e-4 1 $d-2

4 $d-3
241

b2.pin (for STAPL processor)

Rouse shear panels - Panel B2

5 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C deformed shape

2 0 1 181 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

C percent ply damage for different load steps

2 0 8 34 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 8 40 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 8 112 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 8 181 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

C buckling modes

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 -1.0 +1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 -1.0 +1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 -1.0 +1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 -1.0 +1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

C Nxy distributions

2 0 5 30 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 4.5e3 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

2 0 5 40 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 0 0.0 0.0 4.5e3 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX
242

Problem References

Hilburger, M. W. and Starnes, J. H., Jr., “Effects of Imperfections on the Buckling Response of 

Compression-Loaded Composite Shells,” International Journal of Non-Linear Mechanics, Vol. 37, Nos.

4-5, June-July 2002, pp. 623-643.

Rouse, M., “Postbuckling of Flat Unstiffened Graphite-Epoxy Plates in Shear,” AIAA Paper No. 85-

0771-CP, 1985.

Rouse, M., Postbuckling of Flat Unstiffened Graphite-Epoxy Plates in Shear, Master’s Thesis, School of

Engineering and Applied Science, The George Washington University, Joint Institute for the

Advancement of Flight Sciences, Hampton, VA, October 29, 1985.

Knight, Norman F., Jr., Rankin, Charles C., and Brogan, Frank A., “Controlling a Nonlinear Solution

Procedure During a Progressive Failure Analysis,” AIAA Paper No. 2000-1460, April 2000.

Knight, Norman F., Jr., Rankin, Charles C., and Brogan, Frank A., “Controlling a Progressive Failure 

Analysis using Artificial Viscous Damping,” AIAA Paper No. 2001-1180, April 2001.

Knight, Norman F., Jr., Rankin, Charles C., and Brogan, Frank A., “STAGS Computational Procedure for

Progressive Failure Analysis of Laminated Composite Structures,” International Journal of Non-Linear

Mechanics, Vol. 37, Nos. 4-5, June-July 2002, pp. 833-849.

Ambur, D. R., Jaunky, N., Davila, C. G., and Hilburger, M. W., “Progressive Failure Studies of 

Composite Panels with and without Cutouts,” AIAA Paper No. 2001-1182, April 2001.

Ambur, D. R., Jaunky, N., and Hilburger, M. W., “Progressive Failure Studies of Stiffened Panels

Subjected to Shear Loading,” AIAA Paper No. 2002-1404, April 2002

Baranski, A. T. and Biggers, S. B., “Postbuckling Analysis of Tailored Composite Plates with Progressive 

Failure,” Composite Structures, Vol. 46, 1999, pp. 245-255.

Sleight, D. W., Knight, N. F., Jr., and Wang, J. T., “Evaluation of a Progressive Failure Analysis

Methodology for Laminated Composite Structures,” AIAA Paper No. 97-1187, April 1997.

Engelstad, S. P., Reddy, J. N., and Knight, N. F., Jr., “Postbuckling Response and Failure Prediction of

Graphite Epoxy Plates Loaded in Compression,” AIAA Journal, Vol. 30, No. 8, August 1992, pp. 2106-

2113.
243

Membrane Wrinkling Problems

Background

Research on ultra-thin membrane structures for space applications such as solar sails and sun shields is

motivated by the need for advanced space propulsion concepts (see Leifer et al. (1997), Frisbee and

Leifer (1998), and Garner et al. (2000, 2001). On of the leading concepts is the solar sail concept using

ultra-thin membrane films. The square solar sail architecture with separate triangular quadrants (Greschik

and Mikulas (2001) is being developed and ground tests at NASA Langley are planned (Garner et al.

(2001). State-of-the-art literature reviews for membrane structures have been published (Jenkins and

Leonard (1991) and Jenkins(1996)) as well as a review of deployment simulations for inflatable structures

(Jenkins (2001) and Fang (1999)). In addition, a recent monograph by Jenkins (2001) on gossamer 

structures has been published by AIAA covering mission, materials, structural mechanics, deployment

and inflation, structural dynamics, and controls. Examples of NASA efforts in inflatable structures and

ultra-thin membranes include antenna structures such as the IAE, NMP solar sail propulsion concepts, and

NGST sunshields (e.g., Salma et al. (2000), Freeland (2001), Smalley et al. (2001a, 2001b), Johnston

(2002), Johnston and Lienard (2001), and Slade et al. (2001)). These efforts highlight the need for more 

advanced structural analysis tools for this class of structures.

Research topics in solar sail structures include efforts to predict and understand the influence of wrinkles

on the performance of these structures (e.g., Murphey et al. (1999, 2002), Talley et al. (2002)). While the

formation of wrinkles in thin membrane structures is well known, only recently have researchers

measured wrinkle amplitudes and wavelengths (e.g., Jenkins et al. (1998), Blandino et al. (2001, 2002),

Dharamsi et al. (2002)). Specialized experimental measurement procedures using non-contacting

instrumentation such as photogrammetry are needed (Pappa et al. (2002)). Additional ground tests are

either planned or underway and new data are anticipated (Garner et al. (2001)).

Analysis methods have generally fallen into one of two categories. The first category analyzes the 

structure as a membrane using a modified the constitutive matrix so that no compression stresses are 

supported. Methods in this category generally predict the regions where wrinkling is anticipated to

developed and average strains and displacements but give no information regarding the wrinkle amplitude 

or wavelength. The second category analyzes the structure as a very thin shell structure that exhibits

general and local instability characteristics. Methods in this category typically apply finite element

analysis methods to these thin structures and may need to adjust the nonlinear solution procedure in order 

to obtain converged solutions for wrinkled membranes.

Very early work on wrinkled membrane structures is tied to tension field theory. Stein and Hedgepeth

(1961) presented an analytical approach for partly wrinkled membranes and demonstrated its capability

on three basic configurations. The basic approach is to examine the principal stresses and determine 

whether or not a local region of the membrane is taut or slack. Mikulas (1964) extended this approach for 

pre-tensioned circular membranes with a central hub being twisted. Both examined global response 

functions and overall structural behavior for the partly wrinkled membranes rather than detailed

examination of the wrinkles.

Moriya and Uemura (1971) extended the Stein-Hedgepeth approach (1961) using the finite element

method to determine the boundary between wrinkled and unwrinkled regions. They applied the method

to square panels in a picture-frame shear test fixture rather than ultra-thin membranes.

Haug and Powell (1971) developed a nonlinear finite element formulation for membrane structures with

applications to fabric roof structures. They developed a complete finite element formulation for large
244

deformations. With regards to wrinkling, the principal stresses are examined. In addition, prestress

elements are defined that exhibit an isotropic state of stress and are of constant thickness and thin. As a 

result these elements have geometric stiffness but no elastic stiffness. Limited applications were

presented.

Miller et al. (1982, 1985) formulated an algorithm for partly wrinkled membrane from a finite element

analysis perspective using Stein and Hedgepeth’s approach. This model is often referred to as the MillerHedgepeth model; however, this approach is herein referred to as the Stein-Hedgepeth-Miller (or SHM)

model to reflect contributions by each main contributor.

Tabarrok and Qin (1992) applied this wrinkling model to tension structures that were essentially tent

structures for civil engineering applications. The emphasis of their work is on form finding, loads

analysis and cutting patterns. Typically the civil engineering tension structure is not ultra-thin and hence

the nonlinear analysis issue associated with non-convergence and singularities observed for solar sail

applications were not detected.

Adler et al. (2000a, 2000b, 2001) incorporated the SHM model within the Iterative Membrane Properties

(IMP) method and MSC/NASTRAN. Difficulties in controlling the nonlinear solution procedure and

being limited to examining only an element centroid for wrinkling led to a subsequent implementation of

the SHM model as a user-defined material or UMAT for HKS/ABAQUS. This UMAT implementation is

commonly used by other investigators working on gossamer structures. However, this approach still only

provides general information regarding the wrinkled region.

Roddeman et al. (1987a, 1987b, 1991) formulated a large deformation finite element for planar

membrane wrinkling analysis. This formulation is based on the use of a modified deformation tensor.

The principal stresses determine whether a region is wrinkled, slack, or taut. A new membrane finite 

element was developed and tested on a membrane in shear.

Chiu et al. (1994) extended this formulation to account for thermal effects being motivated by the thermal

printing process. Muttin (1996) further extended the Roddeman model to curved membranes. The

applications were then focused on sailboat sails, tension fabric structures, and airbags.

Contri and Schrefler (1988) used a total Lagrangian formulation for a geometrically nonlinear finite 

element analysis with a no-compression material model. The process involves a two-step procedure. The 

first step involves determining the equilibrium state of the membrane with both tensile and compressive 

stresses active. Once determined, the principal stresses are evaluated and compressive stresses

eliminated. New tensile stresses are defined that maintain the same absolute value and direction of the 

principal tensile stress. These new trial stresses are then used in the nonlinear equilibrium iteration

process. The method was demonstrated for an airbag inflation problem.

Kang and Im (1997) also start with the basic nonlinear finite element formulation for a membrane and

incorporate the wrinkling criterion based on a combination of principal stresses and principal strains.

Additional a reconstruction of the stress update procedure during the nonlinear iteration process is

presented which has an impact on the internal force vector and tangent stiffness matrix. Results are 

presented for a flat membrane and an airbag application. Wrinkled regions are identified; however,

wrinkle amplitudes and wrinkle pattern wavelengths are not determined.

Yang and his colleagues (2001, 2002) have proposed an approach using a two-field variational statement

for wrinkling predictions using first a bar-network approach and then for a two-dimensional membrane 

approach. He refers to it as a parameter variation principle or PVP. The total potential energy
245

formulation is augmented with a term having two parameters related to the wrinkle state. Results are

shown to be in good correlation with test data for wrinkle pattern and wrinkle distribution.

Lee and Lee (2002) applied solid shell formulations to gossamer structures. Their approach dealt with

near singularities stemming from these ultra-thin membranes. Two techniques were considered. The first

technique scaled the material moduli by a factor related to the ratio of overall planar membrane size to

membrane thickness (i.e., L/t). The second technique involved performing the computations in

“quadruple” precision. Both techniques essential have the same effect in that the accuracy of their

elements was extended to extremely thin structures. The implication may be that a judicial choice of units

for the membrane geometry and material properties may alleviate some of the numerical issues.

Haseganu and Steigmann (1994) applied a dynamic relaxation solution procedure to partly wrinkled

membranes and thereby avoided some of the quasi-static solution procedure problems associated with

non-convergence and near singularities. Their formulation is based on the relaxed strain energy concept

(Pipkin (1988, 1994). Epstein and Forcinito (2001) have completed the formulation for anisotropic 

membrane wrinkling.

Liu, Jenkins, and Schur (2000) describe two levels of analysis for wrinkled membranes. The coarse-scale

analysis uses a penalty parameter to degrade material stiffness if local wrinkling is detected. The 

wrinkling criterion associated with the SHM model is used for this step in combination with a UMAT and

HKS/ABAQUS. Only general wrinkling behavior (regions and distributions) is obtained. The second

level is the fine-scale analysis that provides details about the wrinkles. The fine-scale analysis extracts

information from the coarse-scale analysis and assumes a uniform wrinkled zone (based on coarse-scale 

analysis). Within this zone wrinkle parameters are calculated in a global/local approach.

Wong (2000) and Wong and Pellegrino (2002a, 2002b) employed HKS/ABAQUS shell elements to

simulate the membrane wrinkling response of the ultra-thin structures. Their approach differs from others

using HKS/ABAQUS in that no UMAT involved. Since the simulation is based on the use of shell

elements rather than membrane elements, wrinkling details may be predicted including wrinkle amplitude 

and wavelength. A membrane with in-plane shear loading was analyzed by first performing the pre-stress

calculation followed by a nonlinear equilibrium check, then a linear buckling analysis that provide the

basis for initial geometric surface imperfections, and finally a nonlinear analysis of an imperfect

(“wrinkled”) membrane. Convergence difficulties encountered in the nonlinear solution process were 

addressed using the automatic stabilization function available in HKS/ABAQUS. In addition, Wong and

Pellegrino (2002a, 2002b) observed and predicted the changes in mode shape (mode jumping) as the inplane shear loading increased. Loading and unloading of the membrane was also examined. Excellent

correlation between test (Jenkins et al. (1998)) and analysis is shown for wrinkle details (number of

wrinkles, amplitude, wavelength and angle).

Stanuszek (2002) membrane wrinkling is treated using a cable analogy – which is not clearly described.

The finite element formulation is based on the natural approach of Argyris using a total Lagrangian

formulation. Nonlinear continuum mechanics approach is used within membrane theory. Stanuszek

(2002) comments that stochastic considerations are necessary for determining the number and distribution

of folds and wrinkles.

The key developments related to finite element prediction for wrinkled membrane structures are 

represented by the works of Adler et al. (2000a, 2000b, 2001), Kang and Im (1997), Wong (2000), and

Wong and Pellegrino (2002a, 2002b). The approach implemented in STAGS under this effort is to first

study the Stein-Hedgepeth-Miller (SHM) membrane model since it is now widely used in the finite 

element analysis of gossamer structures. This model is applied to membrane structures to determine
246

overall behavior and regions susceptible to wrinkling rather than details of the wrinkles (e.g., wrinkle 

wavelength, wrinkle height).

Modeling and Analysis Process

The basic concept behind the Stein-Hedgepeth-Miller model is to examine points within the thin

membrane structure and determine the current stress state. Since the structure is ultra-thin, bending is

often neglected and the stress state is assumed constant through the thickness at a given planar coordinate.

Denoting the planar deformation field as the xy-plane and given the state of strain (

!

"xx ," yy ,# xy

) at a

material point in that plane, the principal strains (

1 2 ! , !

) are determined from:

2 2

1 2 2 2 2 , !

!

"

#

$

$

%

& + !

!

"

#

$

$

%

& '

±

+

=

xx yy xx yy xy ) ) ) ) (

) )

where the subscript 1 denotes major principal value and subscript 2 denotes the minor principal value.

The orientation of the principal axes relative to x-axis is obtained from:

xx yy

xy

! !

"

#

$

tan 2 =

The stress state at that material point can be determined using the strain state and the generalized Hooke’s

law for an isotropic linear elastic material:

!

"

!

#

$

!

%

!

&

'

(

(

(

)

*

+

+

+

,

-

=

!

"

!

#

$

!

%

!

&

'

xy

yy

xx

xy

yy

xx

Q Q Q

Q Q Q

Q Q Q

.

/

/

0

0

0

16 26 66

12 22 26

11 12 16

where 0

2(1 )

1

1

16 26

66

12 2

11 22 2

= =

+

= =

!

=

!

= =

Q Q

E Q G

E Q

E Q Q

"

"

"

"

and E is the elastic or Young’s modulus and ν is Poisson’s ratio. Given this plane stress state, the 

principal stresses can be calculated according to:

"1," 2 = " xx +" yy

2

±

" xx #" yy

2

$

%

&&

'

(

))

2

+ (" xy )

2
247

where the subscript 1 denotes major principal value and subscript 2 denotes the minor principal value.

The orientation of the principal axes relative to x-axis is obtained from:

xx yy

xy

! !

!

"

#

=

2

tan 2

The Stein-Hedgepeth-Miller model then examines these principal stress values and modifies the local

constitutive relations for the membrane. Kang and Im (1997), Wong (2000), and Adler (2000) consider 

three criteria to define the membrane state: stress criteria; strain criteria; and a combined or mixed stressstrain criteria. While similar in concept, the actual criteria are slightly different and six different ones are 

implemented. The first three follow Wong (2000) and the next three follow Adler (2000). These criteria

are:

• Wong (2000) stress criteria based on principal stresses (IWRINK=1)

• Taut state:

"2 > 0

• Slack state:

0 and 0 " 1 ! " 2 !

• Wrinkled state:

"1 > 0 and " 2 # 0

• Wong (2000) strain criteria based on principal strains (IWRINK=2)

• Taut state: ! 2 > 0

• Slack state:

0 and 0 " 1 ! " 2 !

• Wrinkled state:

0 and 0 " 1 > " 2 !

• Wong (2000) mixed stress-strain criteria based on both principal stresses and principal strains

(IWRINK=3)

• Taut state:

"2 > 0

• Slack state: 0 and 0 # 1 ! " 1 !

• Wrinkled state:

"1 > 0 and # 2 $ 0

• Adler (2000) stress criteria based on principal stresses (IWRINK=4)

• Taut state:

"2 > 0

• Slack state:

"1 # 0

• Wrinkled state:

"1 > 0 and " 2 # 0

• Adler (2000) strain criteria based on principal strains (IWRINK=5)

• Taut state:

"1 > 0 and " 2 > #$"1

• Slack state:

"1 # 0

• Wrinkled state:

"1 > 0 and " 2 # $%"1

• Adler (2000) mixed stress-strain criteria based on both principal stresses and principal strains

(IWRINK=6)

• Taut state:

"2 > 0

• Slack state:

"1 # 0

• Wrinkled state:

"1 > 0 and # 2 $ 0

Of these criteria, the mixed stress-strain criteria appear to be the more commonly accepted criteria. Once 

the membrane state is determined at a material point, the constitutive model for the material point is set

accordingly:
248

!

"

!

#

$

=

 taut state

wrinkled state

 slack state

L

L

L

 taut

ij

wrinkle

ij

slack

ij

ij

Q

Q

Q

Q

For the slack behavior, the constitutive coefficients are set to a penalty factor κ (input parameter 

PENLTY) that is typically a very small number approaching zero and are given by:

[ ]

!

!

!

"

#

$

$

$

%

&

=

1 1 1

1 1 1

1 1 1

' slack Q

For the taut behavior, the constitutive coefficients are the original plane stress values for a linear elastic,

isotropic material given by:

[ ]

!

!

!

!

"

#

$

$

$

$

%

&

'

'

=

2

1 0 0

1 0

1 0

1 2

(

(

(

(

E Qtaut

For the wrinkled behavior, the constitutive coefficients are changed and are given by:

[ ]

1 2 1 2

where P cos2 = and sin 2

1

0 2(1 )

2(1 ) 0

4

! !

"

#

! !

! !

#

$

= =

$

$

=

%

%

%

&

'

(

(

(

)

*

$

+

=

xx yy xy

wrinkle

Q

Q Q

P Q

P Q

E Q

The wrinkling process is considered to be an elastic process where wrinkles may form and then disappear 

if the local stress state at a material point would permit it.

This material model can be used with membrane elements (constraint all bending degrees of freedom to

zero using the Q-records) and also with plate/shell elements. Within STAGS, membrane behavior is

modeled by constraining all out-of-plane deformation degrees of freedom (transverse displacement and

two bending rotations) using the loading records (Q-records). The E410 shell element uses the “drilling

degree of freedom” to increase the order of the in-plane displacement field approximations; the E480 and

E330 shell elements do not have this freedom and so it must also be constrained. Using this material

model with plate/shell elements means that the local material stiffness terms are modified in the same way

based on the wrinkling criteria and in addition, the bending stiffness terms are computed and used in the

stiffness matrix evaluation.

The basic computation process for each iteration of a nonlinear solution step starts with a given estimate 

of the displacement solution for the current iteration. Then within the loop over the number of elements

in the finite element model, the local element strain resultants are computed at each element surface 

integration point. Then point strains through the thickness are computed – even though the membrane is
249

very thin. The membrane strains are examined and principal values computed. Stresses are computed

either using the original plane stress values that assumes the membrane is taut or using the values

extracted from the historical material database. The principal values are used to determine the state of the

membrane (taut, slack, or wrinkled). The default criteria will be the stress-strain or mixed criteria.

However, the stress criteria and the strain criteria will also be implemented as options to be used for

comparisons.

Once the membrane state is determined, then the constitutive coefficients are evaluated and new trial

stresses are computed. The constitutive coefficients (Q11, Q12, Q16, Q22, Q26, Q66), principal strains (ε1, ε2),

principal angle for strains (α), principal stressess (σ1, σ2), principal angle for stresses (β), and the

membrane state variable (Mstate) are archived, upon convergence for this solution step, to the historical

material database for this material point – thirteen words per material point. This record is written for 

every material that has changed from an initially taut state to any other state – even when it possibly

returns to a taut state. As long as the membrane state remains in its initially taut state, no data are written

to historical material database for that material point. Once all elements are evaluated, the iteration

process is continued until no compressive regions are found and convergence is achieved.

Numerical Results and Discussion

Pellegino Rectangular Membrane:

The first problem is the rectangular membrane loaded by in-plane shearing displacement studied by Wong

(2000) and Wong and Pellegrino (2002a, 2002b). Finite element results are available for comparison. The 

basic geometry and initial finite element model are shown in Figure 81. The finite element mesh is

uniform having 3960 (99×40) 4-node elements. The STAGS input files are also listed.

Figure 81. Initial finite element of rectangular membrane loaded by in-plane shear.

The rectangular membrane has dimensioned of 128 mm by 380 mm and an assumed uniform thickness of

0.025 mm. The material is a Kapton foil with an elastic modulus of 3530 N/mm

2

, a Poisson’s ratio of 0.3,

and a mass density of 1.5×10-6 kg/mm3. The bottom edge is completely restrained, the side edges are 

free, and the top edge is loaded. The loading has two stages. First, a pre-tensioned stretching of the

membrane is done by imposing an edge displacement (normal to the top edge) of 0.5 mm. Then from this

pre-tensioned state, a shearing displacement (parallel to the top edge) is imposed and increased to a

maximum value of 3.0 mm.

The simulation is performed in two stages. First, a pre-tensioning vertical displacement is imposed in two

solution steps (Load Set B). Then a shearing horizontal displacement is imposed over several solution

steps (Load Set A). Contour plots of the wrinkle indicator are shown in Figures 82 and 83. Results for 

the pre-tensioning state are given in Figure 82 and indicate only minor edge wrinkling. Then the shearing
250

displacement is superimposed with the pre-tensioning displacement and the results are shown in Figure 

83. The wrinkle region extends from the free vertical edges very quickly until the entire membrane is

wrinkled – quantitatively consistent with the available results.

Figure 82. Contour plot of wrinkling indicator for the pre-tensioning step

(Step 2, PA=0.0, PB=1.0, 112 affected elements).

Regions

Changed

From Taut

Membrane

State, %

100%

0
251

(a) Step 3, PA=0.20, PB=1.0, 826 affected elements.

(b) Step 4, PA=0.24, PB=1.0, 1465 affected elements.

(c) Step 5, PA=0.28, PB=1.0, 3730 affected elements.

Figure 83. Contour plot of wrinkling indicator for the pre-tensioning step

Regions

Changed

From Taut

Membrane

State, %

100%

0
252

(d) Step 8, PA=0.40, PB=1.0, 3886 affected elements.

(e) Step 10, PA=1.0, PB=1.0, 3900 affected elements.

Figure 83. Concluded.

Regions

Changed

From Taut

Membrane

State, %

100%

0
253

Square Solar Sail

The second problem is related to the NASA effort in solar sail propulsion concepts. One of the square 

sail architectures defined by Greschik and Mikulas (2001) has four separate triangular quadrants. Ground

testing at NASA Langley is underway for a 10-m solar sail testbed (Slade et al. (2002)) (a two quadrant

model including a center boom). The basic geometry and initial finite element model of a scaled 200-mm 

model are shown in Figure 84.

Figure 84. Initial finite element model of two quadrants of the 200-mm solar sail.

The hypotenuse of each triangular segment of the membrane is 200 mm and an assumed uniform

thickness of 0.0254 mm. The material is a Kapton foil with an elastic modulus of 2964.8 N/mm

2

, a 

Poisson’s ratio of 0.34, and a mass density of 1.4172×10-6 kg/mm3. Along the lower horizontal edge,

three points are fully restrained (the end points and the center point). Between the two triangular regions

is a single beam element to model a center boom structure. The membrane structure is only attached to

the center boom at the end points and not along its length. At the upper vertex, the center boom is loaded

by an applied vertical force with a base magnitude of 1 N.

Nonlinear static solutions are obtained using the SHM membrane wrinkling model with a relaxed

tolerance on the convergence criterion. Contour plots of the wrinkling indicator for several solution steps

are shown in Figure 85. These results indicate that wrinkling develops from the membrane edges and

does evolve as the loading increases. The center region of each quadrant apparently stays taut.
254

(a) Step 1, PA=0.020, 2110 affected elements.

(b) Step 2, PA=0.040, 2200 affected elements.

Figure 85. Contour plots of the wrinkling indicator for several solution steps.

Regions

Changed

From Taut

Membrane

State, %

100%

0
255

(c) Step 3, PA=0.0597, 2074 affected elements.

(d) Step 5, PA=0.1479, 2040 affected elements.

Figure 85. Continued.
256

(e) Step 6, PA=0.2132, 1978 affected elements.

(f) Step 8, PA=0.5115, 2281 affected elements.

Figure 85. Continued.
257

(g) Step 10, PA=1.0, 2073 affected elements.

Figure 85. Concluded.

STAGS Input Files

These input files are located under the following subdirectory:

$STAGSHOME/Advanced-Testcases/Type-E-wrinkling

with the first case under the subdirectory pellegrino and the second case under the subdirectory sail2m.

pellegrino.inp

Rectangular Kapton membrane with in-plane shear loading $a-1

C

C Membrane wrinkling test case studied by Wong & Pellegrino

C

C Ref.: Wong & Pellegrino, "Computation of Wrinkle

C Amplitudes in Thin Membranes," AIAA Paper

C No. 2002-1369, April 2002, SDM in Denver.

C

C MODEL INPUT CONTROLS

1 0 1 0 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 0.0 $B-1b model rotations

1 0 0 0 0 0 0 1 $B-2 include inertial loads

1 0 1 0 0 1 $B-3 INCLUDE GCP INPUT

9814.56 $b-4 acceleration due to gravity mm/s/s (=386.4 in/s/s)

1 1 0 0 0 $B-6 gravity load in y-direction

0.0 0.0 0.0 $b-6a neg y-global to center of earth

C 0.0 9814.56 0.0 $b-6a neg y-global to center of earth

100 41 $f-1 row and columns in each unit (3960 4-node elements)

C

C HISTORICAL STAGS MATERIAL DEFINITION

C
258

C Kapton Type H film

C E=430 ksi = 2964.8 N/mm^2; nu=0.34

C rho(mass) = 0.0512 lbm/in^3 = 1.4172E-6 kg/mm^3 = 0.013909 N/mm^3

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)

3530.0 0.30 0.0 1.4722E-2 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

3530.0, $I-6A YOUNG'S MODULUS, N/mm^2

0.30, $I-6A POISSON'S RATIO

1.5000E-6, $I-6A MASS DENSITY, kg/mm^3

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

C Membrane wrinkling model

SHM_MEMB 2 1 1 0 0 $I-5A MATERIAL NO. 2 (GCP APPROACH)

3530.0, $I-6A YOUNG'S MODULUS, N/mm^2

0.30, $I-6A POISSON'S RATIO

1.5000E-6, $I-6A MASS DENSITY, kg/mm^3

4*0.0, $I-6A UNUSED MATERIAL PARAMETERS

1.0e-3, $I-6a Penalty factor for slack state

3, $I-6a Wrinkling criteria

1 $I-6a Initial membrane state for each iteration

SHELL_FABRICATION 1 1 1 0 0 $I-5A GCP SHELL FABRICATION RECORD

2 $I-21A GCP LAYER MATERIAL ID

1 $I-21A GCP LAYER INTEGRATION POINTS

25.0e-3 $I-21C GCP LAYER THICKNESS, mm (= 25 micro-meters)

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 25.0e-3 0.0 0 $K-2 LAYERED WALL, mm (= 25 micro-meters)

C

C SHELL UNIT 1 MODEL DEFINITION (right side)

C

2 0 0 0 0 0 $M-1 RECTANGULAR PLATE GEOMETRY

0.0 380.0 0.0 128.0 $M-2 rectangle dimensions, mm

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 ELEMENT SELECTION

C

C Boundary conditions

C (horizontal edges in rigid blocks at fixed distance apart

C and the vertical edges are free)

C

0 0 0 2 $P-1 EDGE 4 IS CLAMPED

110 000

110 000

110 000

C

C Load definition

C

2 0 0 0 $Q-1 LOADING SUMMARY

C load system A - horizontal edge displacement - shears membrane

1 1 0 $Q-2 LOAD SET A SUMMARY

3.0 -1 1 0 41 0 0 0 0 0 $Q-3 uniform horizontal displ.

C load system B - vertical edge displacement - tensions membrane

2 4 0 $Q-2 LOAD SET B SUMMARY

0.5 -1 2 0 41 0 0 0 0 0 $Q-3 uniform vertical displ.

0.0 -1 3 0 0 0 0 0 0 0 $Q-3 w=0

0.0 -1 4 0 0 0 0 0 0 0 $Q-3 ru=0

0.0 -1 5 0 0 0 0 0 0 0 $Q-3 rv=0
259

C

C Output Control

C

0 0 0 0 0 0 0 0 $r-1

pellegrino.bin

Wong & Pellegrino rectangular membrane under shear loading $a-1

C

C Nonlinear restart adding in shearing with tensioning

C ( Increment Load Set A with constant Load Set B)

C

3 1 5*0 -1 $B-1 ANALYSIS Type

0.1 0.1 1.0 1.0 0.0 1.0 $C-1 LOAD MULTIPLIERS

2 2000 5 -20 0 1.0e-4 $d-1 Solution controls

0 0 1 $et-1

C

C Nonlinear solution for tensioning first (Load Set B)

C

3 1 5*0 -1 $B-1 ANALYSIS Type

0.0 0.0 0.0 0.5 0.5 1.0 $C-1 LOAD MULTIPLIERS

0 2000 5 -20 0 1.0e-4 $d-1 Solution controls

0 0 1 $et-1

C

C Linear solution

C

0 1 5*0 -1 $B-1 ANALYSIS CONTROL

0.0 0.0 0.0 1.0 1.0 1.0 $C-1 Pre-tensioning

C

C linear buckling analysis

C

1 1 0 4*0 -1 $b-1

1.0 0.0 1.0 1.0 0.0 1.0 $c-1 load factor

6000 1.0e-4 0 $d-2

10 0.0215 $d-3

C

C Nonlinear solution

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

0.0 0.1 0.2 1.0 1.0 1.0 $C-1 LOAD MULTIPLIERS

0 2000 5 -20 0 1.0e-4 $d-1

0 0 1 $et-1

C

C Nonlinear solution

C

3 1 5*0 -1 $B-1 ANALYSIS CONTROL

1.0 1.0 5.0 $C-1 LOAD MULTIPLIERS

0 200 5 -20 0 1.0e-4 $d-1

0 0 0 $et-1

C

C linear vibration with gravity prestress

C

5 1 5*0 -1 $b-1

1.0 $c-1 load factor

1 4 $c-3 number of modes

1.0 $c-4

0 200 5 -20 1 1.0e-4 $d-1

0 0 0 $et-1

C

C free vibration analysis

C

2 1 5*0 -1 $b-1

1.0 $c-1 load factor

200 1.0e-4 0 $d-2

4 $d-3
260

pellegrino.pin

Wong & Pellegrino rectangular Kapton membrane in shear $a-1

10 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C plot membrane state - state variable

2 0 14 1 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 2 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 3 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 4 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 5 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 6 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 8 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 10 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

C plot wrinkling flag

2 0 8 2 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 3 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 4 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 5 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 6 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 7 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 8 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 10 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 12 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 14 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 16 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0
261

2 0 8 18 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

C plot state variable term

2 0 14 18 0 0 1 7 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 .0 .0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 18 0 0 1 10 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 .0 .0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 12 0 0 1 13 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 14 18 0 0 1 13 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

C plot displacements

2 0 1 2 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 1 3 0 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

C plot mode shapes

2 0 4 0 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -5.0 / 2 -5.0 / 3 1.0

2 0 4 0 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -5.0 / 2 -5.0 / 3 1.0

2 0 4 0 3 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -5.0 / 2 -5.0 / 3 1.0

2 0 4 0 4 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 -5.0 / 2 -5.0 / 3 1.0

C plot principal stresses

2 0 7 2 0 0 0 7 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 7 2 0 0 0 8 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 8 2 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

C

2 0 1 6 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

2 0 1 6 0 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 1.0 / 2 1.0 / 3 1.0

C plot stress resultants

2 0 5 0 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 5 0 0 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 5 0 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

C plot strains

2 0 6 0 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP
262

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 6 0 0 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

C plot principal stresses

2 0 7 0 0 0 0 7 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 7 0 0 0 0 8 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

C plot displacements

2 0 1 0 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 1 1 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

sail2m.inp

Two quadrants of square solar sail including center boom $A-1

C

C Tension load applied at tip of center boom then

C shearing displacement

C

C MODEL INPUT CONTROLS

1 0 1 0 0 3 0 $B-1

1 0.0 / 2 0.0 / 3 0.0 $B-1b model rotations

6 1 0 6 2 0 0 0 $B-2 include inertial loads

1 1 1 0 0 1 $B-3 INCLUDE GCP INPUT

9814.56 $b-4 acceleration due to gravity mm/s/s (=386.4 in/s/s)

C1 1 0 0 0 $B-6 gravity load in y-direction

C0.0 9814.56 0.0 $b-6a neg y-global to center of earth

21 21 21 21 21 21, $f-1 row and columns in each unit on right

21 21 21 21 21 21 $f-1 row and columns in each unit on left

C

C Shell unit connections

C

1 3 2 1

1 2 3 4

2 2 3 3

4 1 5 3

4 2 6 4

5 2 6 -1

C

C Partial compatibility at two end points along center

C

4 21 1 0 1 1 1 0

6 21 21 0 3 1 21 0

C

C Element unit specifics

C

3 0 1 0 0 $h-1 element unit (3 nodes and 1 beam element)

C

C HISTORICAL STAGS MATERIAL DEFINITION

C

C Kapton Type H film

C E=430 ksi = 2964.8 N/mm^2; nu=0.34

C rho(mass) = 0.0512 lbm/in^3 = 1.4172E-6 kg/mm^3 = 0.013909 N/mm^3

C

1 $I-1 MATERIAL NO. 1 (HISTORICAL STAGS APPROACH)
263

2964.8 0.34 0.0 1.3909E-2 $I-2 ISOTROPIC ELASTIC MATERIAL

C ============================================

C BEGIN GCP INPUT FOR MATERIAL AND FABRICATION

C

ISOELASTIC_MATERIAL 1 1 1 0 0 $I-5A MATERIAL NO. 1 (GCP APPROACH)

2964.8, $I-6A YOUNG'S MODULUS, N/mm^2

0.34, $I-6A POISSON'S RATIO

1.4172E-6, $I-6A MASS DENSITY, kg/mm^3

4*0.0 $I-6A UNUSED MATERIAL PARAMETERS

C Membrane Wrinkling Model

SHM_MEMB 2 1 1 0 0 $I-5A MATERIAL NO. 2 (GCP APPROACH)

2964.8, $I-6A YOUNG'S MODULUS, N/mm^2

0.34, $I-6A POISSON'S RATIO

1.4172E-6, $I-6A MASS DENSITY, kg/mm^3

4*0.0, $I-6A UNUSED MATERIAL PARAMETERS

1.0e-6, $I-6a Penalty factor for slack state

3 0 $I-6a Wrinkling criteria

SHELL_FABRICATION 1 1 1 0 0 $I-5A GCP SHELL FABRICATION RECORD

2 $I-21A GCP LAYER MATERIAL ID

1 $I-21B GCP Layer integration points

25.4e-3 $I-21C GCP LAYER THICKNESS, mm (= 1 mil)

0.0 $I-21D GCP LAYER ORIENTATION, DEGREES

END $I-5A END GCP INPUT

C END GCP INPUT FOR MATERIAL AND FABRICATION

C ============================================

C

C define center boom stiffnesses

C

1 1 1 0 0.0 $j-1

10.0 1000. 1000. 0.0 $j-2a A, Iyy, Izz, Iyz

C

C HISTORICAL STAGS SHELL FABRICATION DEFINITION

C

1 1 1 0 $K-1 SHELL WALL RECORD

1 25.4e-3 0.0 0 $K-2 LAYERED WALL, mm (= 1 mil)

C

C SHELL UNIT 1 MODEL DEFINITION (right side)

C

3 0 0 0 0 0 $M-1 QUADRILATERAL PLATE GEOMETRY

0.0000 0.0000 , $M-2 coordinates

0.0000 70.7107 , $M-2 coordinates

47.1405 47.1405 , $M-2 coordinates

70.7107 0.0000 $M-2 coordinates

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 ELEMENT SELECTION

C

C Boundary conditions

C

6 6 6 3 $P-1

C

C Load definition

C

1 0 0 0 $Q-1 LOADING SUMMARY

1 4 0 $Q-2 LOAD SET SUMMARY

0.0 -1 3 0 0 0 0 0 0 0 $Q-3 w=0

0.0 -1 4 0 0 0 0 0 0 0 $Q-3 ru=0

0.0 -1 5 0 0 0 0 0 0 0 $Q-3 rv=0

0.0 -1 1 1 1 0 6 1 0 0 $Q-3 Fix one point

C

C Output Control

C

0 $r-1

C
264

C SHELL UNIT 2 MODEL DEFINITION (right side)

C

3 0 0 0 0 0 $M-1 QUADRILATERAL PLATE GEOMETRY

70.7107 0.0000 , $M-2 coordinates

47.1405 47.1405 , $M-2 coordinates

70.7107 70.7107 , $M-2 coordinates

141.4214 0.0000 $M-2 coordinates

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 ELEMENT SELECTION

C

C Boundary conditions

C

6 6 3 3 $P-1

C

C Load definition

C

1 0 0 0 $Q-1 LOADING SUMMARY

1 4 0 $Q-2 LOAD SET SUMMARY

0.0 -1 3 0 0 0 0 0 0 0 $Q-3 w=0

0.0 -1 4 0 0 0 0 0 0 0 $Q-3 ru=0

0.0 -1 5 0 0 0 0 0 0 0 $Q-3 rv=0

0.0 -1 1 21 1 0 6 1 0 0 $Q-3 Fix one point

C

C Output Control

C

0 $r-1

C

C SHELL UNIT 3 MODEL DEFINITION (right side)

C

3 0 0 0 0 0 $M-1 QUADRILATERAL PLATE GEOMETRY

0.0000 70.7107 , $M-2 coordinates

0.0000 141.4214 , $M-2 coordinates

70.7107 70.7107 , $M-2 coordinates

47.1405 47.1405 $M-2 coordinates

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 ELEMENT SELECTION

C

C Boundary conditions

C

6 3 6 6 $P-1

C

C Load definition

C

1 0 0 0 $Q-1 LOADING SUMMARY

1 4 0 $Q-2 LOAD SET SUMMARY

0.0 -1 3 0 0 0 0 0 0 0 $Q-3 w=0

0.0 -1 4 0 0 0 0 0 0 0 $Q-3 ru=0

0.0 -1 5 0 0 0 0 0 0 0 $Q-3 rv=0

0.0 -1 3 1 21 0 4 1 0 0 $Q-3 Fix one point

C

C Output Control

C

0 $r-1

C

C SHELL UNIT 4 MODEL DEFINITION (left side)

C

3 0 0 0 0 0 $M-1 QUADRILATERAL PLATE GEOMETRY

-70.7107 0.0000 , $M-2 coordinates

-47.1405 47.1405 , $M-2 coordinates

0.0000 70.7107 , $M-2 coordinates

0.0000 0.0000 $M-2 coordinates

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 ELEMENT SELECTION
265

C

C Boundary conditions

C

6 6 6 3 $P-1

C

C Load definition

C

1 0 0 0 $Q-1 LOADING SUMMARY

1 3

0.0 -1 3 0 0 0 0 0 0 0 $Q-3 w=0

0.0 -1 4 0 0 0 0 0 0 0 $Q-3 ru=0

0.0 -1 5 0 0 0 0 0 0 0 $Q-3 rv=0

C

C Output Control

C

0 $r-1

C

C SHELL UNIT 5 MODEL DEFINITION (left side)

C

3 0 0 0 0 0 $M-1 QUADRILATERAL PLATE GEOMETRY

-141.4214 0.0000 , $M-2 coordinates

-70.7107 70.7107 , $M-2 coordinates

-47.1405 47.1405 , $M-2 coordinates

-70.7107 0.0000 $M-2 coordinates

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 ELEMENT SELECTION

C

C Boundary conditions

C

3 6 6 3 $P-1

C

C Load definition

C

1 0 0 0 $Q-1 LOADING SUMMARY

1 4 0 $Q-2 LOAD SET SUMMARY

0.0 -1 3 0 0 0 0 0 0 0 $Q-3 w=0

0.0 -1 4 0 0 0 0 0 0 0 $Q-3 ru=0

0.0 -1 5 0 0 0 0 0 0 0 $Q-3 rv=0

0.0 -1 1 1 1 0 6 1 0 0 $Q-3 Fix one point

C

C Output Control

C

0 $r-1

C

C SHELL UNIT 6 MODEL DEFINITION (left side)

C

3 0 0 0 0 0 $M-1 QUADRILATERAL PLATE GEOMETRY

-47.1405 47.1405 , $M-2 coordinates

-70.7107 70.7107 , $M-2 coordinates

0.0000 141.4214 , $M-2 coordinates

0.0000 70.7107 $M-2 coordinates

-1 0 0.0 0.0 0 0 0 $M-5 SHELL WALL RECORD, USE GCP FAB. # 1

410 0 0 $N-1 ELEMENT SELECTION

C

C Boundary conditions

C

6 3 6 6 $P-1

C

C Load definition

C

1 0 0 0 $Q-1 LOADING SUMMARY

1 3

0.0 -1 3 0 0 0 0 0 0 0 $Q-3 w=0
266

0.0 -1 4 0 0 0 0 0 0 0 $Q-3 ru=0

0.0 -1 5 0 0 0 0 0 0 0 $Q-3 rv=0

C

C Output Control

C

0 $r-1

C

C Define 3 nodes for the center vertical boom between the

C two triangular quadrants

C

1 1 1 1 3*0.0 110 000 0 $S-1 base point

2 3 1 21 3*0.0 110 000 0 $s-1 end of strut where load is applied

3 2 21 1 3*0.0 000 000 0 $s-1 reference point defining xy plane

C

C define the beam element - only one required

C

1 2 3 210 1 0.0 0.0 0.0 0 0 $T-2 beam element

C

C tip load on center boom

C

1 0 0 0 $u-1

1 1 $u-2

1.0 1 2 2 0 1 $u-3 tip load in y-direction at node 2 Fy=100 N

1 0 0 0 0 1 $v-1

sail2m.bin

Two quadrants of the square solar sail with gravity loading $a-1

C

C Nonlinear solution

C

3 1 5*0 -1 $B-1 ANALYSIS Type

0.02 0.02 1.0 $C-1 LOAD MULTIPLIERS

0 2000 8 -20 0 1.0e-1 $d-1 Solution Controls

0 0 0 $et-1

C

C Linear solution

C

0 1 5*0 -1 $B-1 ANALYSIS CONTROL

1.0 1.0 1.0 $C-1 LOAD MULTIPLIERS

C

C linear vibration with gravity prestress

C

5 1 5*0 -1 $b-1

1.0 $c-1 load factor

1 4 $c-3 number of modes

1.0 $c-4

0 200 5 -20 1 1.0e-4 $d-1

0 0 0 $et-1

C

C free vibration analysis

C

2 1 5*0 -1 $b-1

1.0 $c-1 load factor

200 1.0e-4 0 $d-2

4 $d-3

C

C linear vibration with gravity prestress

C

5 1 5*0 -1 $b-1

1.0 $c-1 load factor

1 4 $c-3 number of modes

1.0 $c-4
267

0 200 5 -20 1 1.0e-4 $d-1

0 0 0 $et-1

sail2m.pin

Two quadrants of square solar sail

10 0 0 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C plot wrinkling indicator

2 0 8 1 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 8 2 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 8 3 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 8 4 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 8 5 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 8 6 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 8 8 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 8 10 0 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

C plot membrane state - state variable

2 0 14 1 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 14 2 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 14 3 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 14 4 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 14 5 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 14 6 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 14 8 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 14 10 0 0 1 13 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

-1.0 3 0.0 -1.0 1.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

C plot displacements

2 0 1 2 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 1 2 0 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX
268

1 0.0 / 2 -45.0 / 3 15.0

C plot strains

2 0 7 2 0 0 0 11 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 7 2 0 0 0 12 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

C plot principal stresses

2 0 7 2 0 0 0 7 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 7 2 0 0 0 8 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

C plot stress resultants

2 0 5 0 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 2 5 0 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 3 5 0 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

4 5 6

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 1 5 0 0 0 0 1 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

6

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 5 0 0 0 0 2 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 5 0 0 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

C plot vibration mode shapes

2 0 4 1 1 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 -45.0 / 3 15.0

2 0 4 1 2 0 0 3 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 1.0 / 3 0.0

2 0 4 0 3 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0

2 0 4 0 4 0 0 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE,IFRNG,COLOR,ICOMP

0.0 3 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0.0 / 2 0.0 / 3 0.0
269

Problem References

Leifer, S. D., Frisbee, R. H., and Brophy, J. R., “The NASA Advanced Propulsion Concepts Program at

the Jet Propulsion Laboratory,” AIAA Paper No. 97-2792, 1997.

Frisbee, R. H. and Leifer, S. D., “Evaluation of Propulsion Options for Interstellar Missions,” AIAA

Paper No. 98-3403, 1998.

Garner, C. and Leipold, M., “Developments and Activities in Solar Sail Propulsion,” AIAA Paper No.

2000-3858, July 2000.

Garner, C., Price, H., Edwards, D., and Baggett, R., “Developments and Activities in Solar Sail

Propulsion,” AIAA Paper No. 2001-3234, July 2001.

Greschik, G. and Mikulas, M. M., “Design Study of a Square Solar Sail Architecture,” AIAA Paper No.

2001-1259, April 2001.

Jenkins, C. H. and Leonard, J. W., “Nonlinear Dynamic Response of Membranes: State of the Art,”

Applied Mechanics Reviews, Vol. 44, No. 7, July 1991, pp. 319-328.

Jenkins, C. H., “Nonlinear Dynamic Response of Membranes: State of the Art – Update,” Applied

Mechanics Reviews, Vol. 49, No. 10, Part 2, October 1996, pp. S41-S48.

Jenkins, C. H. M. (editor), Gossamer Spacecraft: Membrane and Inflatable Structures Technology for

Space Applications, AIAA Progress in Astronautics and Aeronautics Series, Vol. 191, Paul Zarchan

(editor-in-chief), Reston, Virginia, 2001.

Fang, H. and Lou, M. “Analytical Characterization of Space Inflatable Structures – An Overview,” AIAA

Paper No. 99-1272, April 1999.

Salama, M., Lou, M., and Fang, H., “Deployment of Inflatable Space Structures: A Review of Recent

Developments,” AIAA Paper No. 2000-1730, April 2000.

Freeland, R. F., “History of Relevant Inflatable High-Precision Space Structures Technology

Development,” Gossamer Spacecraft: Membrane and Inflatable Structures Technology for Space 

Applications, C. H. M. Jenkins (editor), AIAA Progress in Astronautics and Aeronautics Series, Vol. 191,

2001, pp. 35-47.

Smalley, K. B., Tinker, M. L., and Fischer, R. T., “Investigation of Nonlinear Pressurization and Modal

Restart in MSC/NASTRAN for Modeling Thin Film Inflatable Structures,” AIAA Paper No. 2001-1409,

April 2001.

Smalley, K. B., Tinker, M. L., and Taylor, W. S., “Structural Modeling of a Five-Meter Thin Film

Inflatable Antenna/Concentrator with Rigidized Support Struts,” AIAA Paper No. 2001-1412, April 2001.

Johnston, John D., “Finite Element Analysis of Wrinkled Membrane Structures for Sunshield

Applications,” AIAA Paper No. 2002-1456, April 2002.

Johnston, J. and Lienard, S., “Modeling and Analysis of Structural Dynamics for a One-Tenth Scale

Model NGST Sunshield,” AIAA Paper No. 2001-1407, April 2001.
270

Slade, K. N., Tinker, M. L., Lassiter, J. O., and Engberg, R., “Dynamics of an Inflatable Structure in

Vacuum and Ambient Conditions,” AIAA Journal, Vol. 39, No. 6, June 2001, pp. 1-8.

Murphey, T. W. and Mikulas, M. M., “Nonlinear Effects of Material Wrinkles on the Stiffness of Thin

Polymer Films,” AIAA Paper No. 99-1341, April 1999.

Murphey, T. W., Murphy D. M., Mikulas, M. M., Jr., and Adler, A. L., “A Method to Quantify the Thrust

Degradation Effects of Structural Wrinkles in Solar Sails,” AIAA Paper No. 2002-1560, April 2002.

Talley, C., Clayton, W., Gierow, P., McGee, J., and Moore, J., “Advanced Membrane Materials for

Improved Solar Sail Capabilities,” AIAA Paper No. 2002-1561, April 2002.

Jenkins, C. H., Haugen, F., and Spicher, W. H., “Experimental Measurement of Wrinkling in Membranes

Undergoing Planar Deformation,” Experimental Mechanics, Vol. 38, No. 2, June 1998, pp. 147-152.

Blandino, J. R., Johnston, J. D., Miles, J. J., and Soplop, J. S., “Thin Film Membrane Wrinkling due to

Mechanical and Thermal Loads,” AIAA Paper No. 2001-1345, April 2001.

Blandino, J. R., Johnston, J. D., Miles, J. J., and Dharamsi, U. K., “The Effect of Asymmetric Mechanical

and Thermal Loading on Membrane Wrinkling,” AIAA Paper No. 2002-1371, April 2002.

Dharamsi, U. K., Evanchik, D. M., and Blandino, J. R., “Comparing Photogrammetry with a

Conventional Displacement Measurement Technique on a 0.5m Square Kapton Membrane,” AIAA Paper 

No. 2002-1258, April 2002.

Pappa, R. S., Jones, T. W., Black, J. T., Walford, A., Robson, S., and Shortis, M. R., “Photogrammetry

Methodology Development for Gossamer Spacecraft Structures,” AIAA Paper No. 2002-1375, April

2002.

Stein, Manuel and Hedgepeth, John M., Analysis of Partly Wrinkled Membranes, NASA TN D-813, July

1961.

Mikulas, Martin M., Jr., Behavior of a Flat Stretched Membrane Wrinkled by the Rotation of an Attached

Hub, NASA TN D-2456, September 1964.

Moriya, K. and Uemura, M., “An Analysis of the Tension Field after Wrinkling in Flat Membrane 

Structures,” IASS Pacific Symposium – Part II on Tension Structures and Space Frames, October 17-23,

1971, Tokyo and Kyoto, International Association for Shell and Spatial Structures, pp. 2-5-1 to 2-5-12.

Haug, E. and Powell, G. H., “Finite Element Analysis of Nonlinear Membrane Structures,” IASS Pacific 

Symposium – Part II on Tension Structures and Space Frames, October 17-23, 1971, Tokyo and Kyoto,

International Association for Shell and Spatial Structures, pp. 2-3-1 to 2-3-13.

Miller, Richard K. and Hedgepeth, John M., “An Algorithm for Finite Element Analysis of Partly

Wrinkled Membranes,” AIAA Journal, Vol. 20, No. 12, December 1982, pp. 1761-1763.

Miller, Richard K., Hedgepeth, John M., Weingarten, Victor I., Das, Prasanta, and Kahyai, Shahrzad,

“Finite Element Analysis of Partly Wrinkled Membranes,” Computers and Structures, Vol. 20, Nos. 1-3,

1985, pp. 631-639.
271

Tabarrok, B. and Qin, Z., “Nonlinear Analysis of Tension Structures,” Computers and Structures, Vol.

45, Nos. 5-6, 1992, pp. 973-984.

Adler, A. L., Mikulas, M. M., and Hedgepeth, J. M., “Static and Dynamic Analysis of Partially Wrinkled

Membrane Structures,” AIAA Paper No. 2000-1810, April 2000.

Adler, A. L., Finite Element Approaches for Static and Dynamic Analysis of Partially Wrinkled

Membrane Structures, PhD Dissertation, Department of Aerospace Engineering, University of Colorado,

Boulder, CO, December 2000.

Adler, A. L. and Mikulas, M. M., “Application of a Wrinkled Membrane Finite Element Approach to

Advanced Membrane Structures,” AIAA Paper No. 2001-4646, August 2001.

Roddeman, D. G., Drukker, J., Oomens, C. W. J., and Janssen, J. D., “The Wrinkling of Thin Membranes:

Part 1 – Theory,” ASME Journal of Applied Mechanics, Vol. 54, No. 4, December 1987, pp. 884-887.

Roddeman, D. G., Drukker, J., Oomens, C. W. J., and Janssen, J. D., “The Wrinkling of Thin Membranes:

Part 2 – Numerical Analysis,” ASME Journal of Applied Mechanics, Vol. 54, No. 4, December 1987, pp.

888-892.

Roddeman, D. G., “Finite Element Analysis of Wrinkling Membranes,” Communications in Applied

Numerical Methods, Vol. 7, 1991, pp. 299-307.

Chiu, H. C., Benson, R. C., Fiscella, M. D., and Burns, S. J., “Mechanical and Thermal Wrinkling of 

Polymer Membranes,” ASME Journal of Applied Mechanics, Vol. 61, No. 1, March 1994, pp. 67-70.

Muttin, F., “A Finite Element for Wrinkled Curved Elastic Membranes, and Its Applications to Sails,” 

Communications in Numerical Methods in Engineering, Vol. 12, No. 11, November 1996, pp. 775-785.

Contri, P. and Schrefler, B. A., “A Geometrically Nonlinear Finite Element Analysis of Wrinkled

Membrane Surfaces by a No-Compression Material Model,” Communications in Applied Numerical

Methods, Vol. 4, No. 1, January-February 1988, pp. 5-15.

Kang, S. and Im, S., “Finite Element Analysis of Wrinkling Membranes,” ASME Journal of Applied

Mechanics, Vol. 64, No. 2, June 1997, pp. 263-269.

Yang, B, Ding, H., Lou, M., and Fang, H., “A New Approach to Wrinkling Prediction for Space

Membrane Structures,” AIAA Paper No. 2001-1348, April 2001.

Ding, H., Yang, B., and Lou, M., “A Two-Viable Parameter Membrane Model for Wrinkling Analysis of 

Membrane Structures,” AIAA Paper No. 2002-1460, April 2002.

Lee, Keejoo and Lee, S. W., “Analysis of Gossamer Space Structures using Assumed Strain Formulation

Solid Shell Elements,” AIAA Paper No. 2002-1559, April 2002.

Haseganu, E. M. and Steigmann, D. J., “Analysis of Partly Wrinkled Membranes by the Method of

Dynamic Relaxation,” Computational Mechanics, Vol. 14, No. 6, September 1994, pp. 596-614.

Pipkin, A. C., “Relaxed Energy Densities for Isotropic Membranes,” Journal of Applied Mathematics,

Vol. 36, 1988, pp. 85-99.
272

Pipkin, A. C., “Relaxed Energy Densities for Large Deformations of Membranes,” Journal of Applied

Mathematics, Vol. 52, 1994, pp. 297-308.

Epstein, Marcelo and Forcinito, Mario A., “Anisotropic Membrane Wrinkling: Theory and Analysis,” 

International Journal of Solids and Structures, Vol. 38, No. 30-31, June 2001, pp. 5253-5272.

Liu, X., Jenkins, C. H., and Schur, W. W., “Fine Scale Analysis of Wrinkled Membranes,” International

Journal of Computational Engineering Science, Vol. 1, No. 2, 2000, pp. 281-298.

Wong, Yew Wei, Analysis of Wrinkle Patterns in Prestressed Membrane Structures, Master of 

Philosophy Dissertation, Department of Engineering, University of Cambridge, U.K., August 2000.

Wong, Y. W. and Pellegrino, S., “Computation of Wrinkle Amplitudes in Thin Membranes,” AIAA Paper 

No. 2002-1369, April 2002.

Wong, Y. W. and Pellegrino, S., “Amplitude of Wrinkles in Thin Membranes,” in New Approaches to

Structural Mechanics, Shells and Biological Structures, H. Drew and S. Pellegrino (editors), Kluwer

Academic Publishers, 2002

Stanuszek, M., “FE Analysis of Large Deformations of Membranes with Wrinkling,” Finite Elements in

Analysis and Design, in press, 2002.

Slade, K. N., Belvin, W. K., and Behun, V., “Solar Sail Loads, Dynamics, and Membrane Studies,”

AIAA Paper No. 2002-1265, April 2002.
273

Actuator Problems

Background

A very simple actuator element can be based on enforcing the relative distance between the two endpoints

to be a function of the applied load factor. Output from this element would in this case be the force 

required in the actuator mechanism to maintain the specified distance. Conversely, a specified force 

directed along the line between the two endpoints can be applied, resulting in a modified distance

between the two points. The geometry of the actuator element is shown in Figure 86.

Modeling and Analysis Process

This sample case involves two flat strips separated initially by a distance of 0.1 inches. Each strip is

clamped at one end and has an actuator element at the corners of the other end. The actuator elements

then drive the two ends apart through specified stroke (ub910.inp) and through specified force 

(ubl910.inp). Note that while STAPL plotting of user-written elements is still pending, STAPL plots can

be generated for those parts of the finite element that use intrinsic STAGS features.

Numerical Results and Discussion

The deformed geometry plots for the two-strip test case with tip actuator elements is shown in Figure 87.

These results indicate that the present actuator element functions properly for large-displacements and

large-rotation applications.

2 2 n x

2 2 n x

1 1 n x

F

d = x2! x1

Figure 86. Illustration of a simple actuator
274

Figure 87. Selected deformed geometry plots for the Charles Rankin two actuator test case.

Step 10

Step 20

Step 37

Actuators

applied

at tip.
275

Sample output from the actuator elements is shown next. The displacements and rotations of each node

on any actuator are printed using the frequency specified for the STAGS Element Unit input. In addition,

actuator specific results (force and stroke) are available as shown:

Force in actuator Uel Type: 910

Element Force

1 -6.29449E-03

2 -6.29449E-03

Length change in actuator Uel Type: 910

Element Delta Length

1 8.25516E+00

2 8.25516E+00

XYTRANS is fully capable of producing a history plot of actuator stroke or resultant (reaction or loading) 

force. No “remaking” of software is necessary since the actuator is a permanent STAGS element. To

obtain the stroke, the user should choose option 14 “total strain and reference surface” and choose option

1 (labeled “xx”), when the request “Enter component for total strain & reference surface:” comes up. The

element number to be input is the actual STAGS global element number (not the actuator number). The

user can input 0 for the element number, and then answer the next request with unit and local element

number, as is done for all other elements. The next prompt requests the user to enter “C” for centroid and

“I” for integration point data: enter C.

For the resultant (reaction or loading force) choose option 13 “integrated stresses.” Follow that with

component 1 (Nx), and the global element number (as described above). Then choose the C option (as

above). Other questions in the interview are exactly the same as for other elements.

The results of these operations go into a {casename}.plt file exactly as in other XYTRANS executions.

This file can be processed with PLOTPS or imported into an EXCEL spreadsheet for display.

An example of an XYTRANS execution followed by PLOTPS processing yields the plot in Figure 88 for 

the test case described above:
276

Figure 88. Representative actuator stroke versus force plot.
277

STAGS Input Files

These input files are located under the following subdirectory:

$STAGSHOME/Advanced-Testcases/Type-F-actuator

STAGS S1 Input:

Two strips clamped at one end and actuators at another

0 0 0 0 0 0 0 $ b1

2 1 0 0 0 0 0 0 0 0 $ b2

1 0 1 0 0 0 $ b3

11 2 11 2 $ f1

-1 -1 0 0 0 0 $ h1

$ Material for plates

1 /1.e7 .03 $I1/I2

$ Wall for plates

1 1 1 $K1

1 .01 $K2

$ Unit 1

2 0 $M1

0. 10. 0. 1. $M2

1 $M5

410 $N1

2 3 3 3 $P1

0 $Q1

1 0 0 0 0 1 $R1

$ Unit 2

2 4

0. 10. 0. 1.

0. 0. .1

0. 0. 0.

1

410

2 3 3 3

1/1 1

0. 5 3 0 0

1 0 0 0 0 1

$====================================================

$--User Element Definitions--------------------------

$====================================================

$

*userElement name="Actuator Element" type=910 nodes=3

*dofOrdering

$ Node DOF...

$ -----------------

1 1 2 3

2 1 2 3

3 1

*nodeSequence

$ Nodes...

$ --------

1 2 3

*floatVariables
278

$ Name Size

$ -------------------

FactA 1

FactB 1

Length 1

*integervariables

$ Name Size

$ -------------------

spec_disp 1

*end userElement

*userProperty name="Standard Data -- Actuator Element" id=910

*integerProps

$ Required Standard Data

$ ----------------------

ActiveNodes 2

SamplingCount 1

StrainCount 1

StressCount 1

*end userProperty

$

$====================================================

$--Element Unit--------------------------------------

$====================================================

0 1 11 1 0.0 0.0 0.0 111 111 0 2 0 $ s3

1 0 0 1 .0 0.0 0.0 $ s3a

0 2 11 1 0.0 0.0 0.0 111 111 0 2 0 $ s3

1 0 0 1 .0 0.0 0.0 $ s3a

0 3*0 5.0 1.0 0.0 000 000 0 1 0 $ s3

END $ s3

$

$ ---------------------------------------------------

E9XX_elements 1 $ t100

910 1 0 0 0 0 2 1 1 $ ----

1 3 5 $ nodes

1 1 0 1 $ {nodes} & elt x-incs

.3 0. 0. $ FactA, FactB, length

1 $ Spec_disp

END $ t100

$====================================================

$--Specified displacements & forces------------------

$====================================================

0

$----------------------------------------------------

1 1 1 0 0 1 0 0 0 0 0 $ v1

STAGS S2 Input:

Two plates with actuator (specifed stroke)

3 1 1 0 0 0 0 -1

.1 .1 60.

0 0 5 -20 -1 1.e-7

0

STAGS STAPL Input:
279

Two plates with actuators

4 0 1 0 $PL-2 NPLOT,IPREP,IPRS,KDEV

C Plot deformed shapes

1 0 1 10 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE

-1.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 1 20 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE

-1.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 1 30 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE

-1.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

1 0 1 37 0 $PL-3 KPLOT,VIEW,ITEM,STEP,MODE

-1.0 0 0.0 0.0 0.0 $PL-5 DSCALE,NROTS,LWSCALE,RNGMIN,RGMAX

Problem References

None.
280

Summary

This document summarizes the STAGS development effort, STAGS performance for selected

demonstration problems, and STAGS application problems illustrating selected advanced features

available in the STAGS Version 5.0. Each problem is discussed including selected background

information and reference solutions when available. The modeling and solution approach for each

problem is described and illustrated. Numerical results are presented and compared with reference 

solutions, test data, and/or results obtained from mesh refinement studies. These solutions provide an

indication of the overall capabilities of the STAGS nonlinear finite element analysis tool and provide 

users with representative cases, including input files, to explore these capabilities that may then be

tailored to other applications.

References

1. Almroth, B. O., Brogan, F. A., and Pittner, E. V., Buckling Analysis of Segmented Orthotropic

Cylinders Under Nonuniform Stress Distribution, Lockheed Missiles & Space Company, Report No. M77-65-4, July 1965.

2. Bushnell, D., Amroth, B. O., and Sobel, L. H., Buckling of Shells of Revolution with Various Wall

Constructions - Volume 2: Basic Equations and Method of Solution, NASA CR-1050, May 1968.

3. Bushnell David, Numerical Methods for the Analysis of Shells, Lockheed Missiles & Space Company,

Report No. 6-77-67-36, October 1968.

4. Brogan, F. A. and Stern, P., Analysis of Stiffened Shells with Cutouts, Lockheed Missiles & Space

Company, Report No. N-3M-69-1, 1969.

5. Almroth, B. O. and Holmes, A. M. C., “Buckling of Shells with Cutouts: Experiment and Analysis,”

International Journal of Solids and Structures, Vol. 8, 1972, pp. 1057-1071.

6. Besseling, J. F., A Theory of Elastic, Plastic, and Creep Deformations of an Initially Isotropic Material,

Stanford University, Department of Aeronautical Engineering, SUDAER Report No. 78, 1958.

7. Marlowe , M. B. and Flugge, W., Some New Developments in the Foundations of Shell Theory,

Lockheed Missiles & Space Company, Report No. LMSC-6-78-68-13, May 1968

8. Almroth, B. O., Brogan, F. A., and Marlowe, M. B., Computer Analysis of Shells of General Shape -

Volume I: Analysis, AFFDL-TR-71-8, August 1972.

9. Almroth, B. O., Brogan, F. A., Meller, E., Zele, F., and Petersen, H. T., Collapse Analysis for Shells of

General Shape - Volume II: User’s Manual for the STAGS-A Computer Code, AFFDL TR-71-8, March

1973.

10. Anon., Collected Papers on Instability of Shell Structures -1962, NASA TN-D-1510, December 1962.

11. Hartung, R. F. (editor), Computer Oriented Analysis of Shell Structures, proceedings of a conference

held in Palo Alto, CA, August 10-14, 1970, AFFDL Report No. TR-71-79, 1971.

12. Hartung, R. F. and Ball, R. E., A Comparison of Several Computer Solutions to Three Structural Shell

Problems, AFFDL, Report No. TR-73-15, 1973.
281

13. Almroth, B. O., Meller, E., and Brogan, F. A., “Computer Solutions for Static and Dynamic Buckling of

Shells,” in Buckling of Structures, B. Budiansky (editor). Proceedings of the IUTAM Symposium, June

17-21, 1974, Springer-Verlag, Berlin, 1976, pp. 52-66.

14. Almroth, B. O., Brogan, F. A., Meller, E., and Petersen, H. T., User’s Manual for the STAGS: Volume 3

- User’s Instructions, LMSC Report LMSC-D351897, January 1974. (STAGSB users manual)

15. Almroth, B. O., Brogan, F. A., and Stanley, G. M., User’s Manual for STAGS - Volume I: Theory,

NASA CR-165670, March 1978. (mainly for STAGSC)

16. Almroth, B. O. and Brogan, F. A., The STAGS Computer Code, NASA CR-2950, February 1978.

(STAGSC overview)

17. Melosh, R. J., “Basis of Derivation of Matrices for the Direct Stiffness Method,” AIAA Journal, Vol. 1,

No. 7, 1963, pp. 1631-1637.

18. Willam, K. J., Finite Element Analysis of Cellular Structures, PhD Thesis, University of California at

Berkeley, Department of Civil Engineering, 1969.

19. Rankin, Charles and Brogan, Frank, The Computational Structural Mechanics Testbed Structural

Element Processor ES5: STAGS Shell Element, NASA CR-4358, May 1991.

20. Ahmad, S., Irons, B. M., and Zienkiewicz, O. C., “Analysis of Thick and Thin Shell Structures by

Curved Elements,” International Journal for Numerical Methods in Engineering, Vol. 2, 1970, pp. 419-

451.

21. Giles, Gary L., Digital Computer Programs for Generating Oblique Orthographic Projections and

Contour Plots, NASA TN D-7797, January 1975.

22. Almroth, B. O., Brogan, F. A., and Stanley, G. M., Structural Analysis of General Shells - Volume II:

User Instructions for STAGSC-1, Lockheed Missiles & Space Company, Report No. LMSC-D633873,

December 1982.

23. Almroth, B. O. and Brogan, F. A., “Computational Efficiency of Shell Elements,” in Nonlinear Finite

Element Analysis of Plates and Shells, T. J. R. Hughes, A. Pifko, and A. Jay (editors), ASME AMDVol. 48, 1981, pp. 147-165.

24. Thomas, K. and Sobel, L. H., Evaluation of the STAGSC-1 Shell Analysis Computer Program,

Westinghouse Electric Corporation, Advanced Reactor Division, Report No. WARD-10881, August

1981.

25. Woytowitz, Peter J., Sample Problems for STAGSC-1, Air Force Wright Aeronautical Laboratories,

Report No. AFWAL-TR-84-3088, February 1985.

26. L. H. Sobel and K. Thomas (editors), Collapse Analysis of Structures, ASME PVP- Vol. 84, June 1984.

27. Riks, E., On the Numerical Solution of Snapping Problems in the Theory of Elastic Stability, Stanford

University, Report SUDAAR No. 401, 1970. Also available as AFOSR 70-2258TR.

28. Riks, E., Brogan, F. A., and Rankin, C. C., “Numerical Aspects of Shell Stability Analysis,”

Computational Mechanics of Nonlinear Response of Shells, W. B. Kratzig and E. Onate (editors),

Springer-Verlag, Berlin, 1990, pp. 125-151.
282

29. Riks, E., “On Formulations of Path-Following Techniques for Structural Stability Analysis,” New

Advances in Computational Structural Mechanics, P. Ladeveze and O. C. Zienkiewicz (editors),

Elsevier Science Publishers, 1992, pp. 65-79.

30. Knight, N. F., Jr. and Starnes, J. H., Jr., “Postbuckling Behavior of Axially Compressed Graphite-Epoxy

Panels with Circular Holes,” ASME Journal of Pressure Vessel Technology, Vol. 107, No. 4, November

1985, pp. 394-402.

31. Rankin, C. C., Stehlin, P., and Brogan, F. A., Enhancements to the STAGS Computer Code, NASA CR4000, November 1986.

32. Rankin, C. C. and Brogan, F. A., “An Element-Independent Corotational Procedure for the Treatment of

Large Rotations,” ASME Journal of Pressure Vessel Technology, Vol. 108, 1986, pp. 165-174. Also

available in Collapse Analysis of Structures, L. H. Sobel and K. Thomas (editors), ASME PVP- Vol. 84,

June 1984, pp. 85-100.

33. Rankin, C. C., Consistent Linearization of the Element-Independent Corotational Formulation for the

STructural Analysis of General Shells, Lockheed Missiles & Space Company, Report No. LMSCF202439, March 1987.

34. Rankin, C. C. and Nour-Omid, B., “The Use of Projectors to Improve Finite Element Performance,”

Computers and Structures, Vol. 30, Nos. 1-2, 1988, pp. 257-267.

35. Nour-Omid, B and Rankin, C. C., “Finite Rotation Analysis and Consistent Linearization Using

Projectors,” Computer Methods in Applied Mechanics and Engineering, Vol. 93, 1991, pp. 353-384.

36. Thurston, G. A., Brogan, F. A., and Stehlin, P., “Postbuckling Analysis Using a General-Purpose

Code,” AIAA Journal, Vol. 24, No. 6, June 1986, pp. 1013-1020.

37. Rankin, C. C. and Brogan, F. A., “Application of the Thurston Bifurcation Solution Strategy to

Problems with Modal Interaction,” AIAA Paper No. 88-2286, April 1988.

38. Davila, Carlos, “Pad Elements for Gaps, Contact Problems and Crack Closure in Fracture Mechanics,”

unpublished NRC Progress Report, August 18, 1992.

39. Rankin, C. C., Chien, L. S., Loden, W. A., and Swenson, L. W., Jr., “Line-to-Line Contact Behavior of

Shell Structures,” AIAA Paper No. AIAA-99-1237, April 1999.

40. Almroth, B. O., Stern, P., and Brogan, F. A., “Automatic Choice of Global Shape Functions in

Structural Analysis,” AIAA Journal, Vol. 16, No. 5, May 1978, pp. 525-528.

41. Almroth, B. O., Stehlin, P. , and Brogan, F. A., “Use of Global Functions for Improvement in Efficiency

of Nonlinear Analysis,” AIAA Paper No. 81-0575, April 1981.

42. Almroth, B. O., Stehlin, P. , and Brogan, F. A., Global Function Approach in Structural Analysis:

Basic Approach, Numerical Results, NASA CR-165669, April 1981.

43. Stehlin, P., Brogan, F. A., and Almroth, B. O., RRSYS Integrated Modular Program System for the

Static and Dynamic Analysis of Elastic Structures by Means of the Rayleigh-Ritz Method - User’s

Manual, Lockheed Missiles & Space Company, December 1981.

44. Stehlin, P., Brogan, F. A., and Almroth, B. O., RRSYS - System Reference Manual (second revision),

NASA CR-178096, July 1986.
283

45. Knight, N. F., Jr. and Stroud, W. J., Computational Structural Mechanics: A New Activity at the NASA

Langley Research Center, NASA TM-87612, 1985.

46. Rankin, C., Stanley, G., and DeRuntz, J., Formulation of Improved Plasticity Calculations in the

STAGSC-1 and NICE-SPAR Computer Codes, Lockheed Missiles & Space Company, Report No.

LMSC-F183026, 1987.

47. Rankin, C. and Brogan, F., STAGS/Testbed Interface, Lockheed Missiles & Space Company, Report

No. LMSC-255539, April 1988.

48. Rankin, C. and Brogan, F., Improved Plasticity and Imperfections in the STAGSC-1 Computer Code -

Phase 2: Implementation, Lockheed Missiles & Space Company, Report No. LMSC-F386402, July

1990.

49. Young, Richard D., “STAGS Sample Problems,” presentation notes dated May 17, 1993.

50. Young, Richard D. “Introduction to STAGS,” presentation charts from STAGS short course at NASA

Langley, June 30 - July 1, 1993. (based on QSTAGS)

51. Brogan, F. A., Rankin, C. C., and Cabiness, H. D., STAGS User Manual - Version 2.0, Lockheed

Missiles & Space Company, Report No. LMSC-P032594, June 1994.

52. Brogan, F. A., Rankin, C. C., and Cabiness, H. D., STAR Reference Manual - Version 2.0, Lockheed

Martin Missiles & Space Company, Inc., Report No. LMMS-P032595, July 1996.

53. Rankin, C. C., Brogan, F. A., Loden, W., and Cabiness, H. D., Structural Analysis of General Shells

(STAGS) User Manual - Version 2.4, Lockheed Martin Missiles & Space Company, Report No. LMMSP032594, June 1997.

54. Hurlbut, B. J. and Stehlin, B. P., Computational Mechanics Testbed (COMET) Generic Constitutive

Processor, Lockheed Missiles & Space Company, Report No. LMSC-F318484, May 1991.

55. Stanley, Gary M., The Computational Structural Mechanics Testbed Structural Element Processor ES1:

Basic SRI and ANS Shell Elements, NASA CR-4357, May 1991.

56. Rankin, C. C., Brogan, F. A., and Riks, E., “Some Computational Tools for the Analysis of Through

Cracks in Stiffened Fuselage Shells,” Computational Mechanics, Vol. 13, 1993, pp. 143-156.

57. Riks, E., Rankin, C. C., and Brogan, F. A., “On the Solution of Mode Jumping Phenomena in ThinWalled Shell Structures,” Computer Methods in Applied Mechanics and Engineering, Vol. 136, Nos. 1-

2, September 1996, pp. 59-92.

58. Riks, E. and Rankin, C. C., “Computer Simulation of the Buckling Behavior of Thin Shells Under

Quasi-Static Loads,” Archives of Computational Methods in Engineering, Vol. 4, No. 4, 1997, pp. 325-

351.

59. Rankin, C. C., Brogan, F. A., Loden, W., and Cabiness, H. D., Structural Analysis of General Shells

(STAGS) User Manual - Version 3.0, Lockheed Martin Missiles & Space Company, Report No. LMMSP032594, June 1998.

60. Rankin, C. C., Brogan, F. A., Loden, W. A., and Cabiness, H. D., STAGS Users Manual - Version 4.0,

Lockheed Martin Missiles & Space Co., Inc., Report No. LMSC P032594, June 2000.
284

61. Knight, N. F., Jr., Rankin, C. C., and Brogan, F. A., “STAGS Computational Procedure for Progressive

Failure Analysis of Laminated Composite Structures,” International Journal of Non-Linear Mechanics,

Vol. 37, Nos. 4-5, June-July 2002, pp. 833-849.

62. Riks, E. and Rankin, C. C., “Sandwich Modeling with an Application to the Residual Strength Analysis

of a Damaged Composite Compression Panel,” AIAA Paper No. 2001-1323, April 2001.

63. Riks, E. and Rankin, C. C., “Sandwich Modeling with an Application to the Residual Strength Analysis

of a Damaged Compression Panel,” International Journal of Non-Linear Mechanics, Vol. 37, Nos. 4-5,

2002, pp. 897-908.

64. Rose, C. A., Moore, D. F., Knight, N. F., Jr., and Rankin, C. C., “Finite Element Modeling of the

Buckling Response of Sandwich Panels,” AIAA Paper No. 2002-1517, April 2002.

65. Rankin, C. C., Brogan, F. A., Loden, W. A., Cabiness, H. D., “STAGS User Manual – Version 5.0,”

Rhombus Consultants Group, Inc., Palo Alto, CA, revised January 2005 (on-line). Previously Report

No. LMSC P032594, Lockheed Martin Missiles and Space Company, Palo Alto, CA.

66. Hurlbut, B. J. and Stehlin, B. P., “Computational Mechanics Testbed (COMET) Generic Constitutive

Processor Manual,” Lockheed Palo Alto Research Laboratory, Palo Alto, CA, Contract Report No.

F318484, May 1991.

67. Rankin, C. C., Loden, W. A., and Swenson, L. W., “STAGS Elements Manual – Version 5.0,

Preliminary,” Rhombus Consultants Group, Inc., Palo Alto, CA, revised January 2005.

68. Brogan, F. A., Rankin, C. C., and Cabiness, H. D., STAR Reference Manual – Version 2.0,” Lockheed

Martin Missiles and Space Company, Palo Alto, CA, July 1996.

69. Loden, W. A., Rankin, C. C., and Young, R. W., “STAGS Test Cases Manual – Preliminary,” Lockheed

Martin Missiles and Space Company, Palo Alto, CA, February 2001.

70. Rankin, C., “STAGS UEL Post-processing and GCP Interface: UEL Developer Requirements

and Interface Enhancements,” January 2005.

71. Rankin, C., “Characterization of STAGS Thermal Capabilities,” January 2005.

72. Rankin, C., “STAGS UEL Post-processing and GCP Interface: UEL Developer Requirements

and Interface Enhancements,” January 2005.

73. Jacoby, M., “STAGS Viewer and Mesher,” December 2004.

74. Rankin, C. “An Actuator Element for STAGS V5,” revised January, 2005.
REPORT DOCUMENTATION PAGE Form Approved

OMB No. 0704-0188

2. REPORT TYPE 

Contractor Report

 4. TITLE AND SUBTITLE

STAGS Example Problems Manual

5a. CONTRACT NUMBER

 6. AUTHOR(S)

Knight, Norman F., Jr.; and Rankin, Charles

 7. PERFORMING ORGANIZATION NAME(S) AND ADDRESS(ES)

NASA Langley Research Center General Dynamics

Hampton, VA 23681-2199 Advanced Information Systems, Inc.

 14700 Lee Road

 Chantilly, VA 20151

 9. SPONSORING/MONITORING AGENCY NAME(S) AND ADDRESS(ES)

National Aeronautics and Space Administration

Washington, DC 20546-0001

 8. PERFORMING ORGANIZATION

 REPORT NUMBER

10. SPONSOR/MONITOR'S ACRONYM(S)

NASA

13. SUPPLEMENTARY NOTES

Prepared for Langley Research Center under GSA Task Order GS-00F-0067M, NASA Order No. NNL05AC09T.

Langley Technical Monitor: Richard D. Young

An electronic version can be found at http://ntrs.nasa.gov

12. DISTRIBUTION/AVAILABILITY STATEMENT

Unclassified - Unlimited

Subject Category 39

Availability: NASA CASI (301) 621-0390

19a. NAME OF RESPONSIBLE PERSON

STI Help Desk (email: help@sti.nasa.gov)

14. ABSTRACT

This document summarizes the STructural Analysis of General Shells (STAGS) development effort, STAGS performance for

selected demonstration problems, and STAGS application problems illustrating selected advanced features available in the

STAGS Version 5.0. Each problem is discussed including selected background information and reference solutions when

available. The modeling and solution approach for each problem is described and illustrated. Numerical results are presented

and compared with reference solutions, test data, and/or results obtained from mesh refinement studies. These solutions

provide an indication of the overall capabilities of the STAGS nonlinear finite element analysis tool and provide users with

representative cases, including input files, to explore these capabilities that may then be tailored to other applications.

15. SUBJECT TERMS

Finite elements; STAGS; Plates; Shells

18. NUMBER

 OF 

 PAGES

289

19b. TELEPHONE NUMBER (Include area code)

(301) 621-0390

a. REPORT

U

c. THIS PAGE

U

b. ABSTRACT

U

17. LIMITATION OF 

 ABSTRACT

UU

Prescribed by ANSI Std. Z39.18

Standard Form 298 (Rev. 8-98)

3. DATES COVERED (From - To)

5b. GRANT NUMBER

5c. PROGRAM ELEMENT NUMBER

5d. PROJECT NUMBER

NNL05AC09T

5e. TASK NUMBER

Task 8

5f. WORK UNIT NUMBER

732759.07.11

11. SPONSOR/MONITOR'S REPORT

 NUMBER(S)

NASA/CR-2006-214281

16. SECURITY CLASSIFICATION OF:

The public reporting burden for this collection of information is estimated to average 1 hour per response, including the time for reviewing instructions, searching existing data sources, 

gathering and maintaining the data needed, and completing and reviewing the collection of information. Send comments regarding this burden estimate or any other aspect of this 

collection of information, including suggestions for reducing this burden, to Department of Defense, Washington Headquarters Services, Directorate for Information Operations and 

Reports (0704-0188), 1215 Jefferson Davis Highway, Suite 1204, Arlington, VA 22202-4302. Respondents should be aware that notwithstanding any other provision of law, no person 

shall be subject to any penalty for failing to comply with a collection of information if it does not display a currently valid OMB control number.

PLEASE DO NOT RETURN YOUR FORM TO THE ABOVE ADDRESS.

1. REPORT DATE (DD-MM-YYYY)

01- 03 - 2006