Source: https://fr.scribd.com/document/162150071/aircraft-crash-analysis
Timestamp: 2019-06-16 00:34:36
Document Index: 146685623

Matched Legal Cases: ['ART 572', 'ART 572', 'ART 572', 'art 23', 'art 23', 'art 21', 'art 23', 'art 23', 'art 572', 'art 572', 'art 23', 'art 23', 'art 23', 'art 23', 'art 23', 'art 572', 'art 572', 'ART 572', 'art 572', 'art 572', 'ART 572', 'art 572', 'ART 572', 'art 572', 'art 572', 'arts 23', 'arts 27', 'art 23', 'art 23']

aircraft crash analysis | Computer Simulation (95 views)
Transféré par Srinivas Rallabandi
ls-dyna crash
enregistrerEnregistrer aircraft crash analysis pour plus tard
CHAPTER 4-Brief Introduction to the Finite Element Method (F
AGATE (ADVANCED GENERAL AVIATION TRANSPORTATION EXPERIMENTS PROGRAM)
METHODOLOGY FOR SEAT DESIGN AND CERTIFICATION BY ANALYSIS (REVISION A) AGATE-WP3.4-034012-079-REPORT
SUBMITTED BY CESSNA AIRCRAFT COMPANY AUGUST 17, 2001
Date of general release: August 31, 2001
Prepared for Langley Research Center National Aeronautics and Space Administration Hampton, Virginia 23681-0001
LETTER N/C DATE 05/28/01 ITEM Original release of report. BY Terence Lim (Cessna Aircraft Company) A 08/01/01 1. Removed AGATE proprietary restriction statement from cover page. Document is released to the general public. 2. Revised Section 4.1.1.5. Head Injury Criteria (HIC) 3. Added section 4.5.5.1. Energy Balance 4. Moved and renumbered Section 3 Reference Publications to Section 2, and added references. 5. Section 2 Definitions was Section 3. 6. Revised Section 3.4 Stability of Codes. 7. Added Section 7 Acknowledgements Terence Lim (Cessna Aircraft Company
1. 2. 3. 3.1 3.2 3.3 3.4 4. 4.1 4.1.1 4.1.2 4.1.3 4.2 4.2.1 4.2.2 4.2.3 4.3 4.3.1 4.3.2 4.4 4.4.2 4.4.3 4.5 4.5.1 4.5.2 PURPOSE REFERENCE PUBLICATIONS DEFINITIONS SEATING CONFIGURATION SEATING SYSTEM COMPUTER MODELING STABILITY OF EXPLCIT CODES SEAT CERTIFICATION BY COMPUTER MODELING GENERAL VALIDATION ACCEPTANCE CRITERIA APPLICATION SPECIFIC VALIDATION CRITERIA DISCREPANCIES COMPUTER HARDWARE AND SOFTWARE APPLICATION OF COMPUTER MODEL IN SUPPORT OF DYNAMIC TESTING DETERMINATION OF WORST CASE FOR A SEAT DESIGN DETERMINATION OF WORST CASE SCENARIO FOR SEAT INSTALLATION DETERMINATION OF OCCUPANT STRIKE ENVELOPE APPLICATION OF COMPUTER MODELING IN-LIEU OF DYNAMIC TEST SEAT SYSTEM MODIFICATION SEAT INSTALLATION MODIFICATION SEAT CERTIFICATION PROCESS CERTIFICATION PLAN TECHNICAL MEETING COMPLIANCE METHODOLOGY AND DATA REQUIREMENTS PURPOSE OF COMPUTER MODEL OVERVIEW OF SEATING SYSTEM
1 2 3 3 3 3 4 6 6 7 11 11 12 12 13 13 14 14 14 14 15 16 17 17 17
4.5.3 4.5.4 4.5.5 4.5.6 4.5.7 4.5.8 5. 5.1 5.2 5.3 5.3.1 5.3.2 5.4 5.4.1 5.4.2 5.4.3 5.4.4 5.5 5.5.1 5.6 5.6.1 5.6.2 5.6.3 5.7 5.7.1 5.7.2 5.8
SOFTWARE AND HARDWARE OVERVIEW DESCRIPTION OF COMPUTER MODEL ANALTICAL RESULT INTERPRETATION MARGIN OF SAFETY MINIMUM DOCUMENTATION REQUIREMENTS RETENTION OF COMPUTER MODEL DATA DECK DYNAMIC SEAT COMPUTER MODELING GUIDELINE UNITS COORDINATE SYSTEM OCCUPANT MODELS ATB HYBRID II (PART 572 SUBPART B) OCCUPANT MODEL MADYMO HYBRID II (PART 572 SUBPART B) DUMMY MODELING STRUCTURAL ELEMENTS METHOD 1 - MULTI-BODY TECHNIQUES METHOD 2 - FINITE ELEMENT MODELING METHOD 3 - HYBRID MODELING METHOD MODELING FAILURE OF JOINTS OR FASTENERS RESTRAINT MODELING METHODS MATERIAL MODELS METALLIC MATERIAL MODELS COMPOSITE MODELS SEAT CUSHION FOAM MODELS APPLYING BOUNDARY CONDITIONS KINEMATIC CONSTRAINTS CONTACT DEFINITION LOAD APPLICATION
18 19 21 23 23 23 24 26 28 29 30 34 40 40 42 54 55 57 57 62 63 67 71 73 74 76 82
5.8.1 5.8.2 5.9 5.9.1 5.9.2 6. 7.
LOAD APPLICATION FOR 60 DEGREES PITCH TEST LOAD APPLICATION FOR 10 DEGREES YAW TEST FLOOR DEFORMATION EXAMPLE FLOOR DEFORMATION SIMULATION USING MADYMO EXAMPLE FLOOR DEFORMATION SIMULATION USING MSC/DYTRAN GENERAL DISCLAIMER ACKNOWLEDGEMENTS
82 84 87 87 88 90 91
PAGE 24 27 29 32 34 35 42 44 46 47 48 49 50 51 53 54 60 61 64 66 66 66 68 72 73
Figure 5-1 Computer Modeling in Seat Design Figure 5-2 Example Unit Specification Figure 5-3 Model Coordinate System Orientation Figure 5-4 ATB HII Occupant Model Figure 5-5 Finite Element MSC/DYTRAN ATB Model
Figure 5-6 MADYMO HYBRID II (PART 572 Subpart B) DUMMY Figure 5-7 Multi-body model Figure 5-8 FE Modeling Flowchart Figure 5-9 Spring Element Figure 5-10 Rod Element Figure 5-11 Beam Element Figure 5-12 Shell Element Figure 5-13 Solid Element Figure 5-14 MSC/DYTRAN FE Model Figure 5-15 Exploded View of FE Seat Figure 5-16 MADYMO Hybrid Modeling Model Figure 5-17 MADYMO 4-Point Restraint Before Pre-simulation Figure 5-18 MADYMO Hybrid Belt After Pre-simulation Figure 5-19 Elasto-Plastic Material Model Figure 5-20 Example MSC/DYTRAN Input for Strain Rate Material Figure 5-21 Example LS-DYNA3D Input for Strain Rate Material Figure 5-22 Example MADYMO Input for Strain Rate Material Figure 5-23 User Defined Shell Integration Points Figure 5-24 Foam Impact Test Figure 5-25 Stress-%Crush Foam Data
Figure 5-26 Example of FOAM1 material model Figure 5-27 Rigid Connections Figure 5-28 Example RCONN Input Deck Figure 5-29 Contact Applications Figure 5-30 MSC/DYTRAN Surface Contact Definition Figure 5-31 MADYMO Multi-Body Contact Figure 5-32 Multi-body Contact Definition Figure 5-33 ATB 1 G Load Application Pitch Test
73 75 76 78 79 81 81 83 84 84 85 86 88 89 90
Figure 5-34 MSC/DYTRAN Load Application Pitch Test Figure 5-35 Test 1 Applied Loads Figure 5-36 Test 2 Applied Loads Figure 5-37 MSC/DYTRAN Load Application Yaw Test Figure 5-38 Floor Deformation Using MADYMO Figure 5-39 Floor Deformation Using MSC/DYTRAN Figure 5-40 MSC/DYTRAN Pitch and Roll Simulation
FOREWORD A methodology for demonstrating compliance with FAR Part 23.562 by computer modeling analysis technique, validated by dynamic seat tests, was generated by the AGATE Advanced Crashworthiness Group. was performed in collaboration with the Federal Aviation Administration Small Airplane Directorate. Nothing in this document This document was This task
shall supersede applicable laws and regulations.
developed by The Cessna Aircraft Company under the AGATE crashworthiness program, and is approved by the principal members of the Integrated Design and Manufacturing Technical Council for public release under the terms of the Joint Sponsorship Research Agreement. This document may be reproduced and distributed without restrictions. Any improvements, beneficial comments or clarification needed regarding the contents of this document shall be forwarded to: Advanced Crashworthiness Group Intergrated Design and Manufactring Technical Council c/o AGATE Alliance Association Inc. 3217 N. Armistead, Ste. M Hampton, VA 23666-1379
1. PURPOSE The purpose of this document is to provide guidance for demonstrating compliance with FAR Part 23.562 by means of computer modeling analysis techniques. It defines the acceptable applications, limitations,
validation processes and minimum documentation requirements that are involved when substantiation by computer modeling is used to support a seat certification program. This document also provides guidance and lists specific examples on the methodologies associated with generating occupant crash simulation. The intent of this document is to provide an engineer
with background in transient finite element modeling with sufficient details to develop a seat/occupant computer model that may be successfully employed for design and certification. Since the practice of computer modeling is highly dependent on the state of hardware and software at the time of the release of this document, future enhancement may effect portions of the guideline, and appropriate update to this document will be required. It is recognized that there may be more than one possible approach in generating a seat/occupant computer model. Therefore, the
methodologies and examples presented in this document should not be construed as the only method of performing a computer analysis of the seat/occupant system. Other modeling techniques, subjected to reasonable validation, may be acceptable and should be coordinated with the FAA if the data is to be used for certification purposes.
2. REFERENCE PUBLICATIONS Code of Federal Regulations, Title 14 Part 21 Certification Procedures for Products and Parts. Code of Federal Regulations, Title 14 Part 23 Airworthiness Standards: Normal, Utility, and Acrobatic Category Airplanes
U.S. Department of Transportation FAA Order 8110.4A Type Certificate Process Advisory Circular 23.562-1 Dynamic Testing of Part 23 Airplane Seat Restraint/Systems and Occupant Protection, 1989. SAE 8049 Rev.A Performance Standard for Seats in Civil Rotorcraft, Transport Aircraft, and General Aviation Aircraft, 1997. SAE J211 Instrumentation for Impact Test, SAE Recommended Practice, March 1995. Articulated Total Body Version V.1 Users Manual, United States Air Force Research Laboratory 1998. MSC/DYTRAN Users Manual Version 4.7, The Mac-Neal Schwendler Corporation 1999. MADYMO Users Manual 3D Version 5.4, TNO-MADYMO 1999. MADYMO Database Manual 3D Version 5.4, TNO-MADYMO 1999. MADYMO Theory Manual 3D Version 5.4, TNO-MADYMO 1999. LS-DYNA Theoretical Manual, Livermore Software Technology Corporation 1998. LS-DYNA Users Manual Version 940, Livermore Software Technology Corporation 1997. Finite Element Procedures in Engineering Analysis, K.J. Bathe 1982. Solutions Method, T.Belytschko, W.K.Liu and B. Moran 1999.
3. DEFINITIONS 3.1 SEATING CONFIGURATION
The aircraft interior floor plan, which defines the seating positions available to passengers during take-off, landing and in-flight conditions. 3.2 SEATING SYSTEM A seating system is comprised of the seat structure, upholstery and restraint system. 3.3 COMPUTER MODELING The use of computer based finite element or multi-body transient analysis to simulate the physical crash event. These codes typically follow an explicit formulation. The following combination of computer
codes and occupant models have been tested for use in the design and certification of dynamic seats. 1. MADYMO transient finite element/multi-body software and the
MADYMO 50% Part 572 Subpart B (Hybrid II) occupant model. 2. MSC/DYTRAN transient finite element software and the ATB
(Hybrid II) occupant model 3. LS-DYNA3D transient finite element software and the MADYMO 50%
MADYMO is a registered trademark of TNO Road-Vehicles Research Institute MSC/DYTRAN is a registered trademark of the MacNeal-Schwendler Corporation LS-DYNA3D is a registered trademark of the Livermore Software Technology Corporation
ATB is a public domain code developed and maintained by Wright Patterson Air Force Base
Part 572 Subpart B (Hybrid II) occupant model. 3.4 STABILITY OF EXPLCIT CODES Most transient explicit finite element codes employ direct integration methods, and take advantage of the numerical effectiveness of integration schemes such as the central difference methods, Wilson- or Newmark -methods. These integration schemes attempt to satisfy
equilibrium only at discrete time intervals (t) rather than for the duration of the analysis. The accuracy and stability of the solution is highly path dependent, and relies heavily on the interpolated values of displacements, velocities and accelerations within each time step interval. The
inherent numerical instabilities encountered with explicit dynamic analysis codes are discussed in detail, most notably by Bathe and Belytschko in their respective publications (reference Section 2). The solutions are therefore conditionally stable, a trade-off for the simplicity and cost effectiveness of the methods. The stability of
the explicit methods is a function of the critical time step tcr defined as
tc r = mi n
where le is the effective length of the smallest element, and c is the wave speed (a function of material stiffness). In other words, the time step selected for the analysis must be smaller than the time for
the stress wave to cross the smallest element in the finite element mesh. Otherwise, the solution can grow without bound and deviate from stability, and thereby, producing erroneous results. In theory, the most accurate solution is obtained when an integrating time step equivalent to the stability limit is chosen. Commercial
codes, such a MADYMO or LS-DNA3D, attempt to offset the problems of numerical instability by automatically regulating and constantly updating the time interval used throughout the analysis. Although the
user may chose an initial time step to begin the analysis, the program will calculate the critical integration time step, and will either terminate or default to the critical time step if the user input time step is larger than the minimum.
4. SEAT CERTIFICATION BY COMPUTER MODELING Computer analysis may be used to substantiate a seat system design that is subjected to the certification requirements of FAR Part 23.562 after it has been correlated to the validation acceptance criteria specified in Section 4.1. The validation must be performed on a
baseline seat design that has demonstrated compliance, by test, to 14 CFR 23.562. Once validated, the model may then be utilized for certification purposes under the conditions specified in Section 4.2 and 4.3. Further utilization of computer analysis for demonstrating compliance beyond the conditions specified in Sections 4.2 and 4.3 will occur as the experience base of industry grows. 4.1 GENERAL VALIDATION ACCEPTANCE CRITERIA The model is considered validated and may be used as means of demonstrating compliance if the validation acceptance criteria specified in this section have been demonstrated. The criteria will
allow for some subjective interpretation as long as the basis of such interpretation is consistent with good engineering judgment. Such
interpretation shall also be commensurate with the basis of the regulation, and the level of correlation required of the applicant shall not be imposed to tolerances beyond that observed in a dynamic test. The validation acceptance criteria are as follows: 1. The model must be reasonably validated against a dynamic test.
2. The model can be utilized for substantiation under similar conditions that the model was validated against. 3. The general pre-impact occupant trajectory, verified by visual comparisons, should correlate against test data. In addition to the general validation criteria above, the model has to correlate to the following application specific criteria defined in Section 4.1.1. 4.1.1 APPLICATION SPECIFIC VALIDATION CRITERIA The intent is to have the applicant validate -in addition to the general validation criteria- parameters that are relevant to the application of the model. This will remove undue burden from the
applicant to perform validation for other parameters that may not be used in the certification. The relevant application specific
validation criteria should be established and agreed by the FAA ACO, and listed in the certification plan. Test data used to validate the The
model should be included as an appendix in the analysis report.
computer model is considered validated if reasonable agreement between analysis and test data can be shown. Acceptable correlation methods
related to each application specific validation criteria are defined in Section 4.1.1.1 to 4.1.1.6. 4.1.1.1 OCCUPANT TRAJECTORY
Occupant trajectory describes the overall motion of the occupant. The trajectory of the occupant (such as headpath) determined by analysis
may be compared to high-speed video obtained from dynamic tests. Validation may be established by visual comparison or by over-laying space (xy, yz or zx) time-history plots obtained from the analysis to calibrated photometric data obtained from dynamic tests. 4.1.1.2 STRUCTURAL RESPONSE
The computer model, used for structural certification, may be validated by correlating the following structural performance criteria to dynamic test. 4.1.1.2.1 INTERNAL LOADS
Internal loads such as floor reaction loads are a required means to show correlation. Reasonable agreement between the peak resultant
floor reaction load obtained in the analysis and test data should not exceed 10%. 4.1.1.2.2 STRUCTURAL DEFORMATION
Reasonable agreement should be obtained between the mode of structural deformation obtained by analysis and test data for members that are critical to the overall performance or structural integrity of the seat or seating system. Validation may be established by visual
comparisons or by over-laying space (xy, yz or zx) plots obtained from the analysis to photometric data obtained from dynamic tests. 4.1.1.3 RESTRAINT SYSTEM
Compliance with shoulder harness load is defined in FAR Part 23.562(c)(6). Validation of the restraint system may be obtained by correlating the analysis belt load force-time history to test data. The phase and maximum value force-time history profile should correlate within 10% of dynamic test data. This would ensure that in the analysis, the energy from the occupant as a result from inertia forces are transferred appropriately to the seat and vice versa. Additional parameters such as belt pay-out or permanent elongation may be correlated if similar measurements were recorded during dynamic test. 4.1.1.4 INJURY CRITERIA
Validation of the injury criteria may be obtained by correlating the analysis time history plots to test data. In general, the level of deviation in the injury criteria between analysis and test data should not exceed 10%. 4.1.1.5 HEAD INJURY CRITERIA (HIC)
Compliance with Head Injury Criteria is defined in FAR Part 23.562(c)(5). The regulation specifies HIC to be calculated during
the duration of the major head impact, and the maximum allowable HIC limit is 1,000 units. The selected time interval1 used in calculating HIC may not exceed 50 milliseconds. If the HIC evaluation involves head impact with airbags, FAA will determine the appropriate HIC limit and time interval criteria2. In either case, the time interval used to
evaluate HIC in the analysis should be selected to match the time interval size used to evaluate HIC in the test. Because HIC is a
maximizing function, the reported time duration3 that produces the maximum HIC need not match. The analysis is validated for HIC if the following correlations between analysis and test data are established. 1. The phase and profile of the acceleration time-history plot for resultant head accelerations. 2. The average resultant G loading as measured from the center of the head center of gravity. 3. The HIC calculation, using the same time interval.
The term time interval used in this section is defined as the duration between
the initial and end time which the user selects to calculate HIC, which should correspond to the duration when the ATD is exposed to head impact on airplane interior features.
Shorter HIC evaluation time intervals and lower HIC limits are used in the
automotive regulations (46 CFR 571.208) to account for head/airbag interactions, and may be appropriate in some airplane certification. The validation of computer models using a HIC limit other than that specified in 14 CFR 23.562 should be approved by the FAA.
The term reported time duration used in this section is defined as two points in This reported
time in the head acceleration profile that produces the maximum HIC.
time duration is not user defined, and is based on the outcome of the HIC algorithm.
4.1.1.6 SPINE LOAD
Compliance with spine load is defined in FAR Part 23.562(c)(7). The maximum allowable limit is 1,500 pounds. The phase and maximum value
force-time history profile for spine load obtained in the analysis should be correlated to the dynamic test. 4.1.2 DISCREPANCIES Failure to satisfy all validation criteria does not automatically preclude the model from being validated. The applicant and the FAA
ACO engineer should evaluate if the deviations will have a detrimental impact on the model to sufficiently predict the crash scenario, and to determine if deviations from the validation criteria are acceptable. In addition, the applicant may present evidence to show that the deviation is within the inherent reliability and statistical accuracy of the test results. Discrepancies between results obtained from analysis and test data should be quantified. 4.1.3 COMPUTER HARDWARE AND SOFTWARE The model should be used for certification on the same hardware and software platform that the validation was conducted. The model should Beta
be developed using the production version of the software. releases are not allowed.
If the computer model is transferred for
use on a different platform, the applicant must re-validate the model as necessary to ensure that the results do not reflect any significant differences.
4.2 APPLICATION OF COMPUTER MODEL IN SUPPORT OF DYNAMIC TESTING The purpose of this section is to encourage the use of analysis to reduce the number of full-scale dynamic test that are required to certify a seat design or installation. This is beneficial in
certifying seats that are based on the same design concept, but may differ structurally to accommodate a particular installation. A final certification test is normally required to certify the worst-case seat design or installation. When the intent of the computer model is to provide engineering analysis and rationale in support of dynamic testing, the results from the computer model may be used for, but are not limited to, the following conditions specified in Section 4.2.1 through 4.2.3. Additional conditions, which are currently not defined, shall be coordinated with the local FAA ACO and approved in the certification plan. 4.2.1 DETERMINATION OF WORST CASE FOR A SEAT DESIGN Upon completion of the computer analysis, the results from the simulation may be used to determine the worst case or critical loading scenario for a particular seating system. This includes
1. Identifying components of seat structures that are critically loaded. 2. Selection of critical seat tracking positions.
3. Determine the direction of floor deformation to produce worst case loading on seat frame. 4. Evaluation of restraint system. 5. Selection of worst-case seat cushion build-up. 6. Evaluation direction of yaw condition to address loading on seat frame and movement of occupant out of restraint system. 4.2.2 DETERMINATION OF WORST CASE SCENARIO FOR SEAT INSTALLATION For seats, which have been shown by analysis or test to be similar, computer analysis may be used to select the worst case seating system in the seating configuration for dynamic testing. Each seating system shall be analyzed in its production installation configuration. Examples where analysis may be used to determine a worst case seating system may include: 1. Seating system installed in an over-spar versus a non-over spar configuration. 2. Seating system installed at different positions in the fuselage, which results in varying restraint anchor positions relative to the occupant and seat structure. 4.2.3 DETERMINATION OF OCCUPANT STRIKE ENVELOPE The results of the computer analysis may be used to determine the occupant strike envelope with aircraft interior components. Each
seating system shall be analyzed in its production installation
configuration. The occupant strike envelope can then be used to determine if a potential for head strike exist, and if so, which items are required in the test setup during the HIC evaluation tests.
4.3 APPLICATION OF COMPUTER MODELING IN-LIEU OF DYNAMIC TEST The purpose of this section is to encourage the use of analysis to eliminate dynamic testing on certified seats. When the intent of the
computer model is to provide engineering data in-lieu of dynamic testing, the results from the computer model may be applied to the following conditions: 4.3.1 SEAT SYSTEM MODIFICATION Analysis based on computer simulation may be used to re-substantiate seat designs which have been modified from the TSOd or certified configuration. No additional testing is required.
4.3.2 SEAT INSTALLATION MODIFICATION Analysis based on computer simulation may be used to re-substantiate seat installations. The primary application is to show compliance for
HIC and occupant body-to-body contact as a result of changes in seat arrangements. 4.4 SEAT CERTIFICATION PROCESS This section contains certification guidelines when computer modeling is utilized as supporting engineering data to demonstrate compliance 14
with FAR Part 23.562.
It defines the procedures that are involved
with regards to FAA coordination, guidelines for the preparation and validation of the computer model, and the minimum documentation requirements for FAA data submittal. 4.4.1.1 FAA COORDINATION
The FAA coordination process used in this document has been extracted from FAA Order 8110.4A. FAA coordination is essential in ensuring the Specific
proper and timely execution of any certification program.
guidelines are presented to assist in the implementation of computer modeling as a means of compliance. 4.4.2 CERTIFICATION PLAN The use of computer modeling as technical data to support the establishment of dynamic test conditions or in-lieu of dynamic test shall be negotiated with the FAA during the preliminary and interim Type Certification Board (TCB) meeting. The applicants role is to:
1. Acquaint the FAA personnel with the project 2. Discuss and familiarize the FAA with the details of the design 3. Identify, with the FAA, applicable certification compliance paragraphs. 4. Negotiate with the FAA where the applicant will utilize computer modeling, specify its intent and purpose for the analysis.
5. Establish means of compliance, either by test, computer modeling or both with respect to the certification requirements. 6. Establish the validation criteria for the computer model relative to its application for certification. 7. Prepare and obtain FAA ACO approval of the certification plan. 4.4.3 TECHNICAL MEETING The details of the computer model are defined during scheduled technical meetings held with the FAA ACO. The applicant should
prepare a document for the FAA describing the purpose of the analysis, the validation methods and data submittal format. As a minimum, the
following items should be contained in the document: 1. Description of the seat system to be modeled. 2. Selection of software for the analysis. 3. A description of how compliance will be shown. 4. Validation method. 5. Interpretation of results. 6. Substantiation documentation and data submittal package. The document, hereby referred to as the analysis report, should be developed in conjunction with the seat design evaluation phase, and approved by the FAA as early in the certification program as possible.
4.5 COMPLIANCE METHODOLOGY AND DATA REQUIREMENTS The following sections define the methodology for showing compliance and minimum documentation requirements when computer modeling is submitted as engineering data. should contain the following: 4.5.1 PURPOSE OF COMPUTER MODEL The applicant should define the purpose of the computer model and a list of the FAR requirements relevant to the certification of the seating system. Emphasis should be given to describe how the computer As a minimum, the analysis report
model would be used to demonstrate compliance for each stated requirement. 4.5.2 OVERVIEW OF SEATING SYSTEM Provide an overview of the design of the seating system. Describe the seat layout in the aircraft, restraint type, and attachment to the airframe. If applicable, state the adjustment positions required during take off and landing. Discuss special occupant protection features included in the design. 4.5.2.1 SEAT STRUCTURE
Describe the critical components of the seat, the primary load paths and energy absorbing features. Provide a description on how the List the material properties of
seat(s) are attached to the airframe.
the primary structural and energy absorbing components, and specify the method of fabrication. 4.5.2.2 RESTRAINT SYSTEM
Provide a description of the restraint system and any other devices that are intended to restrain the occupant in the seat or reduce the occupants flail envelope under emergency landing conditions. This
may include the shoulder and lap belts, load limiting devices, belt locking devices and pretensioners. Describe how the restraint system and its devices are attached or secured in position. 4.5.2.3 UNIQUE ENERGY ABSORBING FEATURES
Unique energy absorbing features are components, other than the seat and restraint system, that are designed to limit the load into the seating system or occupant. Examples include energy absorbing sub-
floor structure and inflatables that are not mounted on the seat. 4.5.3 SOFTWARE AND HARDWARE OVERVIEW The analysis report should contain a brief description of the software and hardware used to perform the analysis, and should include the following information: 1. Type and platform of computer hardware 2. Software type and versions 3. Basic software formulation.
4.5.4 DESCRIPTION OF COMPUTER MODEL The analysis report should contain a detailed description of the computer model. This includes providing rational to the following:
4.5.4.1 ENGINEERING ASSUMPTIONS
Assumptions that are made in the analysis should be documented. Assumptions may include simplification of a physical structure, the use of a particular material model, methods used for applying boundary conditions, method of load application, etc. Discuss the validity of If
the assumptions and provide rational support for the assumptions.
required, demonstrate that the assumptions do not negatively affect the results. Components that are not critical to the performance of the seating system and do not influence the outcome of the analysis may be omitted from the model. A list of all components that are excluded from the
analysis shall be documented. Comments should be included to justify its exclusion. 4.5.4.2 DISCRETIZATION OF PHYSICAL STRUCTURE
A description of the finite element mesh of the structure should be provided in the analysis report. It should describe how the critical components of the structure were modeled and provide the rational for the selection of element types that were used to represent the structure.
4.5.4.3 MATERIAL MODELS
Data of material models in the analysis should be documented in the analysis report. List the materials used by the analysis software and provide a general description. Document the source of material data. Material data acquired through in-house tests must be supported by appropriate documentation that describes the basis of such test, test methods, and results. This includes proprietary data. 4.5.4.4 CONSTRAINTS
Constraints are boundary conditions applied in the model.
includes single and multi-point constraints, contact surfaces, rigid walls and tied connections. Document the boundary conditions applied in the model. Discuss how the model boundary conditions correspond to the test conditions. Provide a description on all contact definitions and nodal constraints. Document the values used to represent frictional constants and the validity of such values. 4.5.4.5 LOAD APPLICATION
Loads that are applied in the computer model include concentrated forces and moments, pressure, enforced motion and initial conditions. Describe how external loads are applied to the model. List the source
of the crash pulse and include a copy of the profile in the appendix.
4.5.4.6 OCCUPANT SIMULATION
The use of appropriate occupant models is dependent on the objective of the analysis. The use of the appropriate occupant model should be If the analysis is used to certify to the
negotiated with the FAA.
requirements of FAR 23.562(b)(1) and (b)(2) conditions, then a validated occupant model representing a 50th percentile male per 49 CFR Part 572 Subpart B or equivalent approved dummy should be used. Descriptions should be included in the analysis report on the development and validation of the occupant model. 4.5.4.7 GENERAL ANALYSIS CONTROL PARAMETERS
General analysis control parameters are features of a program that control, accelerate and terminate the analysis. It may also include
parameters that enhance the performance of the software for the purpose of reducing the computational time, and subroutines that are employed to facilitate post-processing of results. A summary of the control parameters used for a particular analysis should be documented. Parameters that may influence the outcome of For example, the analyst should
the analysis should be justified.
show that artificial scaling of mass for the purpose of reducing computational time is acceptable and does not negatively influence the results of the model. 4.5.5 ANALTICAL RESULT INTERPRETATION
This section contains guidance and recommendations for the output, filtering and the general methods of reporting analytical data. purpose is to achieve uniformity in the practice of reporting analytical results. The use of the following recommendations will The
provide a basis for meaningful comparison to test results from different sources. 4.5.5.1 ENERGY BALANCE
A summary of the ratio of initial energy to final energy, and a comparison of hourglass energy to total energy should be provided. The hourglass energy should not exceed 15% of total energy. In
addition, the deformation modes associated with the presence of hourglass energy should be evaluated to determine if they are located at critical components of the structure, upon which, and an assessment of the hourglass modes and its influence on the accuracy of the analysis be determined. The model should be corrected as required if
the appropriate energy balance is not attained. 4.5.5.2 DATA OUTPUT
Data from transient analysis should be generated at channel class 1000. The purpose is to maintain an equivalent practice with the
instrumentation requirement specified in SAE J211 so that a meaningful comparison to test data may be performed. If the output of the data channels is dependent on the integration time step of the analysis, and its sample rate is higher than channel
class 1000, the data should be reduced to be consistent with channel class 1000 prior to filtering. the analysis report. 4.5.5.3 DATA FILTERING A deviation should be documented in
The filtering practices of SAE J211 shall apply for all applications (reference in Section 5 of the SAE J211 document for the recommended channel class filtering). 4.5.6 MARGIN OF SAFETY Margin of safety applies only to structural substantiation and should show a positive margin of safety. Injury pass/fail criteria shall not
exceed the maximum value as specified in 14 CFR 23.562(c). 4.5.7 MINIMUM DOCUMENTATION REQUIREMENTS The FAA data submittal package to show compliance with FAR 23.562 by means of computer modeling should contain the following: 1. Report of the analysis. 2. Video of the computer model simulation. 4.5.8 RETENTION OF COMPUTER MODEL DATA DECK A copy of the computer model data deck used for substantiation should be archived for reference purposes. The archived copy of the data
deck should include the date and the final revision number of the model.
5. DYNAMIC SEAT COMPUTER MODELING GUIDELINE This section presents some of the methods used to develop a computer model of the occupant and seating system. The examples presented reflect the versions of the software used at the time of the release of this document (reference Section 3.0). When used effectively,
computer models can reduce the cost and certification schedule significantly. Figure 5-1 shows a flowchart on the use of computer
modeling in the dynamic seat design process. Figure 5-1 Computer Modeling in Seat Design
D esign & Param etric Study
P aram etric Study D esign
Seat/D ivider/U pholstery W eight reduction Increase confidence in design R estraint optim ization O ccupant trajectory O ccupant injury prediction E nergy absorbing concepts
D iagnostic Tool (pre-test)
C ertification T est
D iagnostic Tool (post-test)
In the preliminary design phase, computer modeling is used to perform numerous parametric studies to investigate different energy absorbing concepts and establish design parameters to meet the structural and occupant loads. Simple restraint models are generated to predict
occupant trajectory and determine, optimize restraint design and determine the approximate anchor mount positions. Information from the parametric analysis is used to produce the prototype seat design. The prototype seat is then evaluated for fit and function, and modifications made to refine the design. More details are added to the computer models as the seat design moves from the prototype to the first production concept design. The analysis is performed to obtain an accurate prediction of structural and occupant response, and in particular, occupant loads with respect to the dynamic pass/fail criteria. The objective is to reduce the
risk of failure and the need to re-test during the certification program. In this phase, detailed finite element models are used to
generate cross-section properties of beam structures that can withstand the dynamic load. Iterations in analysis are performed to obtain an optimal stiffnessto-weight ratio. Interior components such as glareshield, instrument panels and side-ledges are added to the model to predict the head injury criteria. Seat cushions, seat pans or energy absorbing devices Floor deformation analysis is
are modeled to predict spine load.
performed to determine if the seat structure is able to react the induced pre-stress and crash load without failure. The simple axial
belt model used in the parametric analysis is replaced with 2-D finite element belt model to provide better occupant trajectory predictions. An evaluation test is conducted on the seat design and appropriate changes are made based on the test results. The design and analysis
cycle is iterated until a satisfactory design is attained, and the seat program proceeds to the certification phase. Computer models can also be utilized as a post-test diagnostic tool. Well-prepared models can sometimes help identify anomalies that occurred during a test that are linked to bad instrumentation channels. The computer model helps establish the range or approximate
values that a measuring device may produce, such as shoulder harness load or head acceleration. The output from the computer model can be compared with actual test signals to determine if the test data are physically possible or if the signals are compromised by noise or faulty instrumentation. 5.1 UNITS Transient finite element modeling requires the use of a consistent set of engineering units for the fundamental measures of length (L), time (T), mass (M) and derivative units such as velocity (L/T) and force (ML/T2). Table 5-1 show an example of different sets of consistent units. It is good modeling practice to define a specific set of
units that will be used in the model by specifying them early in the data deck, as shown in an example MSC/DYTRAN file in Figure 5-2.
Table 5-1 Sets of Consistent Units
Length Mass Time Density Force Stress
Meter (m) Kilogram (kg) Second (s) kg/m3 kg m/s2 = Newton (N) N/m2 = Pa
Foot (ft) slug (lbf-s2/ft) Second (s) slug/ft3 slug ft/s2 = lbf (slug ft/s2)/ft2 =lbf/ft2 (slug ft/s2)ft =lbf-ft
mm/kg/ms
Millimeter (mm) Kilogram (kg) Millisecond (ms) kg/mm3 KN Gpa
Nm = Joule (J)
This would help the person generating the model, and users downstream that may be involved in editing, debugging or checking the analysis, to quickly recognize and apply the correct input to the model. Figure 5-2 Example Unit Specification $ SEAT CRASH TEST MODEL $ $ SI Units: kg - meter - seconds $ -----------------------------$ conversion factors $ lbm/in3 to kg/m3: multiply by 2.767990e+4 START ENDTIME=150.E-3 PARAM,INISTEP,1.E-6 TLOAD=1
In general, software such as MSC/DYTRAN, MADYMO or LS-DYNA3D do not require the model to be defined in a particular set of units as long they are consistent. However, careful consideration should be given
when the structural finite element model is coupled with an occupant
For MADYMO the use of SI units with the occupant model is
highly recommended due to built-in absolute convergence criteria. Using non-SI units with MADYMO occupants may introduce error in results. Other coupled models - such as MSC/DYTRAN/ATBwill execute
well either in English or SI units as long as both the structure and the occupant have consistent set of units. 5.2 COORDINATE SYSTEM The seat model should be aligned with the aircraft coordinate system. This will facilitate the results of the computer model to be correlated to the test data, where the coordinate and sign convention of the test instrumentation is also oriented in the aircraft coordinate system, as specified in SAE J211. For the seat and sled,
the X-axis should be along the fore-aft (fuselage) direction of the aircraft, the Y-axis along the inboard-outboard (buttline) direction, and the Z-axis along the direction of gravity (waterline). Figure 5-3
illustrates a MADYMO model of a forward facing seat aligned in the aircraft coordinate system. The engineer needs to note the specific orientation of the occupants axis system, since different occupant models have their own bodyattached axis system and may differ from the positive sign convention of the ATDs transducers as specified by the SAE J211 document.
Figure 5-3 Model Coordinate System Orientation
5.3 OCCUPANT MODELS Most occupant models have been validated for a particular application. For example, the NHTSA Hybrid III occupant model has been extensively validated and used in automotive applications. Cessna has correlated the response of the ATB Hybrid II and MADYMO Hybrid II for aircraft applications with full-scale test data (ref AGATE report C-GEN-3432-1 and C-GEN-3433-1). The ATB Hybrid II and MADYMO Hybrid II occupant models have a response similar to the 14 CFR Part 572 Subpart B Hybrid
II ATD, and therefore are suitable for use in design and certification. Other occupant models may be used for certification if sufficient data is available and the validation task is coordinated with the FAA. 5.3.1 ATB HYBRID II (PART 572 SUBPART B) OCCUPANT MODEL The ATB Hybrid II (Part 572 Subpart B) occupant model executes within the ATB crash simulation program. Although the ATB program by itself (with multi-body capabilities) can be used to perform crash simulation, the lack of a finite element solver makes it impractical for use in complex analysis and certification where stress results are required. The ATB occupant model is generally coupled with the
MSC/DYTRAN finite element codes, although there are current developments to integrate it with LS-DYNA3D within the automotive industry. For practical purposes, this document will provide a brief overview of the ATB HYBRID II model and how ATB is coupled with MSC/DYTRAN. Detailed information of the ATB program, theory or the
organization and control of the ATB input deck is available from the ATB Version V Users Manual. The input for the ATB program is contained in a FORTRAN formatted file with the *.ain extension (i.e. seatmodel.ain). The main output file
is identified by the *AOU extension and contains an annotated listing of the program input and summary of the kinetic energy, accelerations, etc for each requested time step. debugging. It is also the primary source for
Tabular time history of specific outputs, such as joint
forces, accelerations and displacements, are generated in the *THS file. Each ATB input file has the following structure as specified in
Table 5-2. Table 5-2 Program ATB Input Card Structure
CARD TYPE Card A.1-A.5 Card B.1-B.7 Card C.1-C.5 Card D.1-D.9 Card E.1-E.7 Card F.1-F.10 Card G.1-G.6 Card H.1-H.12
DESCRIPTION Run control parameters Physical characteristics of the body Prescribe motion Contact surface and other environmental definitions Function definitions Allowed contacts and associated functions Equilibrium constraint assignments Tabular time history output control parameters
Definition of each card entry is given in the ATB Model Input Manual. The ATB Hybrid II occupant is comprised of 17 rigid segments connected by 16 pin and spherical joints (Figure 5-4). The geometry, inertial
properties and bio-fidelity of the ATB model simulate the NHTSA 49 CFR Part 572 Subpart B ATD. and SI units. The parent body of the ATB occupant represents the lower torso (Segment 1 - LT). The head acceleration is obtained from Segment 5. Joint number 1 connects the middle torso (MT) to the lower torso (LT), and joint number 2 connects the middle torso (MT) to the upper torso 31 The occupant model is available in English
(UT) of the lumbar column.
Therefore, the resultant force in the Z-
direction for joint 1 or 2 represents the compressive force of the spinal column. Figure 5-4 ATB HII Occupant Model
Card G.2 defines the initial position and velocity of the occupant. Orientation of different segments of the body (such as rotating the arms or legs of the occupant) to obtain a desired occupant position is defined by manipulating the coordinate and orientation of each segment in Card G.3. The ATB model, when coupled with MSC/DYTRAN will appear in the MSC/PATRAN pre/post processor as shown in Figure 5-5. The ATB model was digitized with rigid shell finite elements (with negligible mass)
so that contact with other surrounding finite element structures can be defined. The ATB ellipsoid was coupled to MSC/DYTRAN by means of a
RELEX entry. The RELEX entry defines a rigid ellipsoid within the MSC/DYTRAN environment whose properties and motions are governed by ATB. The rigid shell finite elements are then attached to the MSC/DYTRAN ellipsoid through a RCONREL entry, thus completing the finite element definition of the ellipsoid ATB dummy.
Dummy positioning is performed using MSC/PATRAN by running a dummy positioning session file supplied by MSC. The session file enables
each individual segment (arms, legs,etc) to be positioned and a new set of nodes will be written out to select the final occupant position. The session file also generates an ATBSEG card, which overwrites the position and orientation of the ATB segments specified in the *ain file. Since ATB is internally coupled to MSC/DYTRAN, no major change is required to the *ain input file.
Finite Element MSC/DYTRAN ATB Model
5.3.2 MADYMO HYBRID II (PART 572 SUBPART B) DUMMY The Part 572 Subpart B dummy database available with MADYMO version 5.4 is made of 32 bodies connected with various kinematic joints (reference Figure 5-6). There are seated and standing versions included, but only the seated dummy will be discussed in this
document. See the MADYMO 5.4 Database Manual and Users Manual for detailed information. Figure 5-6 MADYMO HYBRID II (PART 572 Subpart B) DUMMY
Table 5-3 Standard MADYMO Part 572 Subpart B Dummy Definition
NUMBER 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 NAME LOWER TORSO ABDOMEN LOWER LUMBAR UPPER LUMBAR UPPER TORSO RIBS LOWER NECK BRACKET LOWER NECK SENSOR NECK NODDING PLATE HEAD CLAVICLE LEFT CLAVICLE RIGHT UPPER ARM LEFT UPPER ARM RIGHT LOWER ARM LEFT HAND LEFT HAND RIGHT HAND LEFT FEMUR LEFT FEMUR RIGHT KNEE LEFT KNEE RIGHT UPPER TIBIA LEFT UPPER TIBIA RIGHT MIDDLE TIBIA LEFT MIDDLE TIBIA RIGHT LOWER TIBIA LEFT LOWER TIBIA RIGHT FOOT LEFT FOOT RIGHT STERNUM COMPLIANT CENTRAL REGION OF RIB CAGE PROXIMAL OF FEMUR LOAD CELL PROXIMAL OF FEMUR LOAD CELL PERIPHERAL OF FEMUR LOAD CELL PERIPHERAL OF FEMUR LOAD CELL ABOVE UPPER LOAD CELL ABOVE UPPER LOAD CELL IN BETWEEN LOAD CELLS IN BETWEEN LOAD CELLS BELOW LOWER LOAD CELL BELOW LOWER LOAD CELL FOR LOAD SENSING ONLY SPINE BOX AND BACK OF THE RIBS FRONTAL AREA OF THE RIB CAGE FOR NECK ANGLE ADJUSTMENT ONLY FOR LOAD SENSING ONLY REMARKS REFERENCE BODY OF DUMMY SYSTEM
The lower torso body is the reference body in the dummy system and connects to inertial space with a free joint (joint number 1), meaning all rotation and translation degrees of freedom are unconstrained. Any other bodies in the dummy system can be traced back to the reference body along a single path (there are no closed loops). Therefore, the overall position and orientation of the dummy is specified by the reference joint degrees of freedom (DOF) entries following the JOINT DOF keyword. The relative orientations of the system child bodies can be adjusted in the input block following the JOINT DOF keyword. This allows adjusting the dummy posture from the nominal seated position. Do NOT position the dummy parts by modifying the joint coordinate system orientations in the dummy database following the JOINTS keyword, as this will disrupt the joint ranges of motion and stiffness characteristics. The default dummy database is structured as two trees of keyword/input blocks. The first part of the deck is the system specification enclosed between the keywords SYSTEM and END SYSTEM. The second part of the deck is the output requests enclosed between the keywords OUTPUT CONTROL PARAMETERS and END OUTPUT PARAMETERS. Note that keywords may be abbreviated as specified in the MADYMO Users Manual, for example SYS for SYSTEM or END for END SYSTEM etc. The following entries are in the SYSTEM block: CONFIGURATION table defines the body connectivity.
GEOMETRY defines the coordinates of each joint and joint CG in the parent body coordinate system. INERTIA table defines the inertial properties of each body and orientation. JOINTS table specifies each joint type, stiffness, and orientation. INCLUDE the lumbar spine characteristics are encrypted in the referenced h350lumb.v03 file. FLEXION-TORSION RESTRAINTS defines the force model for the neck and spine. CARDAN RESTRAINTS defines the force models for the hips and ribs. Orientations and stiffness functions are specified following this data block. ELLIPSOIDS table defines the ellipsoid dimensions, degree, and (optional) contact stiffness characteristics. Orientations and stiffness functions are specified following this data block. KELVIN defines a spring-damper element (Kelvin element) for the spine. CONTACT INTERACTIONS defines the dummy self-contact evaluations. POINT-RESTRAINTS the ribs and abdomen have compressive characteristics defined using point restraints. A point restraint is
equivalent to three mutually orthogonal Kelvin elements. See section 7.3 in MADYMO Theory Manual Version 5.4. JOINT DOF these values prescribe initial joint position and velocity degrees of freedom. The following entries are in the OUTPUT CONTROL PARAMETERS section of the dummy model. Additional parameters can be specified as stated in the MADYMO 5.4 Users Manual. TSKIN time interval for writing data to kinematic and FE results files. KIN3 results format version and options. TSOUT time interval for writing data to time history files. FILTER PARAMETERS configure signal filters for results data. LINACC output requests for linear acceleration vs. time for specified points on bodies, with options to correct for prescribed fictitious acceleration fields. CONSTRAINT LOADS output requests for joint constraint loads and filter parameters. INJURY PARAMETERS output requests for occupant injury criteria. Note: The default window size for HIC is set to 36 ms in the MADYMO Part 572 Subpart B dummy model file. The automotive industry uses the 36 ms window. Federal Aviation Regulations definition of HIC does not
specify a window size other than the full duration of the impact event. 14 CFR Parts 23 and 25 do not explicitly define a time window for HIC calculations, but a maximum window of 50 ms is defined in 14 CFR Parts 27 and 29 (Rotorcraft and Transport Rotorcraft, respectively). In practice, the FAA often imposes the 50 ms maximum window on Part 23 and 25 aircraft certification tests. Automotive
regulations (49 CFR 571.208) have recently adopted a 15 ms window with a maximum allowable HIC of 700 for airbag interactions. The modeler
should apply the appropriate maximum window based on the impact surface and the negotiated certification requirement. 5.4 MODELING STRUCTURAL ELEMENTS The modeling of structural elements may consists of the seat structure, cushions, restraint systems, floor structure, instrument panels, glareshields, side panels, crash sled and any other objects that can influence the response of the occupant. There is no ideal method to model structural elements. Generally, each method depends on the capabilities of the software, the information the analyst wants to extract from the model and the desired accuracy of the analysis. There are three basic methods to model structural elements, which are discussed in subsequent sections. 5.4.1 METHOD 1 - MULTI-BODY TECHNIQUES The easiest method to model structural objects is to use multi-body (a Madymo definition) or rigid elements. This includes using combinations of simple planes, cylinders, ellipsoids, and facet
surfaces. Multi-body elements are primarily used to simplify the representation of the structure and are utilized in applications where the kinematic response of the structure is desired but information on stresses and strains are not required. Parts of rigid bodies can be connected together by spring-damper or torsional spring elements to provide resistive force. Figure 5-7 shows an example of a Madymo seat model generated using multi-body techniques. This model represents an over-spar bench seat, where there is no significant deformation. Because of the rigidity of
the seat, structural deformation and stresses were not required. Therefore, a multi-body model is sufficient in determining the response of the occupant. The seat structure, seat cushion and crash vehicle was represented by multi-body planes. These planes are positioned so that it reflects the correct configuration of the actual seat structure. Each plane has inertial and stiffness properties that are typically obtained from sub-component compression test. For example, the plane representing the seat bottom has a stiffness function that represents the actual seat cushion behavior. system. The planes are fixed to the vehicle inertial
Contact is defined between the occupant and planes in terms
of load versus deflection.
Figure 5-7 Multi-body model
The model above is particularly useful as a parametric tool because of its simplicity and low computational cost. Changes to the model are
easily made, and the next load case is analyzed. 5.4.2 METHOD 2 - FINITE ELEMENT MODELING The most representative technique to model structural objects is to use the finite elements (FE) method. FE models are generated to obtain
detailed response of structures and to determine failure modes. Madymo and MSC/DYTRAN have extensive non-linear FE capabilities. Finite element models are more difficult to generate than multi-body models. However, FE models are more practical because they predict
realistic structural response and offer the capability to output stresses, strains and internal loads. They can also be utilized to substantiate structural designs. Figure 5-8 shows a process flowchart that is commonly used to generate a FE model. The precise method on how to generate an efficient FE model of a seat structure will depend on the design of the seat itself and the desired output of the model. Generally, the first step is to determine the load path of the structure for each load case. Then, lists of the
critical load carrying members within the load path are noted. Engineering judgment will be used to determine the mode of failure for each critical member. This will help determine the choice of elements to represent the structural. Geometry data of the seat structure from a CAD package, such as CATIA or Pro-Engineer, is converted to a form such as IGES which can be used by the FE pre-processor as surfaces or solids for generating the FE mesh. Each part of the seat structure is grouped and meshed Care must be taken to ensure that the shape of each
element is not distorted in order to avoid computational problems during the analysis. After all components of the structure are
meshed, the individual groups are merged by equivalencing coincident nodes.
Figure 5-8 FE Modeling Flowchart
Conduct prelim inary static analysis Determ ine critical load m em bers Extract CAD surface geom etry Im port IGES IG ES geom try into Patran Divide into sub - structures Determ ine deformation deform ation m odes
Assign node & elem ent ids
Create FE m esh
Input material m aterial properties
Input material properties
C o n n e c t p a r ts
E q u iv a le n c e n odes
R ig id c o n n e c t io n s
A p p ly b o u n d a r y c o n d it i o n s
A p p ly in itia l c o n d it i o n s
S e t C o n ta c t In te r a c tio n s
A p p ly e x te r n a l lo a d
S e t a n a ly s is co n tr ol p a ra m eters
S e t o u tp u t req u est
Sometimes, parts can be joined together using spot weld elements or rigid elements. Spotweld elements allow for the joined parts to
separate once the loads have met a user defined failure criteria such as tension, shear, torque or moments. Rigid elements are essentially
a multi-point constraint (MPC) and are used to define a set of grid points that forms a rigid element. The next step is to create a database of material properties and assigning them to its respective structure. Pre-processors such as PATRAN have capabilities that link CAD geometry to finite elements, so that the user can select the geometry instead of selecting individual elements (which tends to be more difficult in complex or large size models). Boundary conditions are applied to constrain the seat model to the vehicle. This is done by selecting the nodes where the seat is
attached to the seat rails and applying a constraint to the translational or rotational degrees of freedom. In addition, contact
is defined between parts that rest, slide or have the probability of contacting each other. External loads are applied by prescribing acceleration loads to the seat. The definition of external loads are obtained from the actual
crash sensor or the analyst can apply a fictitious triangular pulse prescribed in the FARs. The final step in the process includes setting analysis control parameters such as analysis termination time, integration method,
hourglass energy control, mass scaling and selecting the set of output request. At this point , the model is ready to be executed. However,
rarely does a FE model execute flawlessly during the first attempt. The process typically goes through a cycle of error debugging and correction of the input deck. 5.4.2.1 ELEMENT TYPES
There are many types of finite elements, and the choice of element selection will depend on the load and deformation characteristics of the actual structure that it will represent. Finite elements used for structural analysis are also known as Lagrange elements in terms of the formulations of these elements. grouped in the following categories: 1. Scalar Elements Typically consist of spring, mass and damper elements. properties are usually user defined. The stiffness Finite elements are typically
Scalar masses are commonly used
to model a concentrated mass at one location, such as an engine block, fuel contents or ballast weights. There is no stiffness definition associated with a scalar mass. Figure 5-9 Spring Element
Spring elements connect two grid points and the force acts in the direction of the connecting grid points. Spring elements connect translational and rotational degrees of freedom and may have linear or non-linear stiffness property. For translational springs, the For
stiffness is defined in terms of force versus deflection.
rotational springs, the stiffness is defined in terms of moment versus angle of rotation. 2. One-dimensional elements One-dimensional elements are used to represent structural members that have stiffness along a line or a curve. Examples of one-dimensional elements are rod and beam elements. Rod elements carry tension and compressive loads only. The mass of the elements are lumped and distributed equally at the nodes. The only
geometry property required is the cross-sectional area of the rod. Figure 5-10 Rod Element
Beam elements carry axial, torsion and bending loads. The mass of the beam is lumped and equally distributed over the two nodes. Care has to be taken regarding the center of mass, shear center and centroid definition of the beam definition for each code. Unless otherwise stated, the mass, shear center and centroid of the cross-section all
The orientation of the beam should be defined in its
element coordinate system. The geometry property required are the area and moments of inertia of the beam. Figure 5-11 Beam Element
3. Two-dimensional elements Consist of membrane, quadrilateral and triangular elements. These elements are most widely used because of the versatility and robust formulations. The mass of two-dimensional elements element are lumped and equally distributed over all the nodes. Membrane elements carry in-plane loads and do not have bending stiffness. Membrane elements can be three or four-node elements with The deformation is
three translation degrees of freedom on each node.
determined by the translation degrees of freedom on these nodes. Depending on the code, membrane elements can have linear or non-linear properties. Seat belt webbing and seat pans are modeled using
membrane elements. The geometry property required is the thickness of the membrane.
Quadrilateral shell elements are the most widely used.
They carry in-
plane as well as bending loads. Shell elements have six degrees of freedom at each node; three translations and three rotations. Transverse shear stiffness is accounted for by a shear correction factor. The geometry properties required are the shell thickness and the number of integration points through the thickness. Triangular elements typically exhibit a stiffer response and are used only as transitional elements and in areas of low stress concentrations. Most codes use a default one-point integration at the center of the element, although there are options to increase the number of integration points at the expense of computational efficiency. Note
that when one-point integration is used, the hourglass or zero energy modes are generated and which will have to be suppressed. Figure 5-12 Shell Element
Over the years, advanced formulations have allowed for more robust and computationally efficient elements, such as the Belytschko-Tsai, KeyHoff and Hughes-Liu shells. The choice of element formulation usage will depend on the need to compromise accuracy with computational
speed. suffice.
In most cases, the Belytschko-Tsai shell formulation would
4. Three-dimensional elements Three-dimensional elements are also known as solid elements and consist of tetra, penta and hexa elements. The element is capable of carrying tensile, compression and shear loads. The mass of the solid elements are lumped and equally distributed over all nodes. Figure 5-13 Solid Element
The hexahedral element is commonly used because of its efficiency, and it is easier to mesh and interface with other elements. The tetra and
penta elements are degenerated forms of the hexa elements where the grid points coincide resulting in significant reduction in performance. The solid elements use one-point (or reduced) However, this also results These modes will have to be
integration for computational efficiency. in twelve zero energy or hourglass modes.
suppressed using the hourglass energy control parameter that is available in all codes.
5.4.2.2 EXAMPLE FE MODEL
Figure 5-14 shows an example of an MSC/DYTRAN FE seat model.
purpose of the model was to obtain an accurate prediction of the structural response, locate areas of high stress concentrations and determine how the seat affects the occupants trajectory. Figure 5-14 MSC/DYTRAN FE Model
Shell elements were the most widely used of all Lagrange elements because of its robust formulation and versatility. The seat assembly consists of five (5) primary structures; pan, seat base and seat pivot assembly. The seat was modeled in the aircraft coordinate system consistent with the definitions presented in Section 4.2. The crash load from the seat back, seat bucket, seat
occupant is transferred to the seat from the anchor points on the shoulder harness and the lap belt. In the forward impact case, the
load is transferred from the seat back down to the pivot mechanism, and finally to the diagonal cross members on the seat base in the form of compression load. The majority of the seat structure was modeled using 4-noded quadrilateral CQUAD4 (KEYHOFF formulation) shell elements. Triangular
CTRIA3 (CO-TRIA formulation) elements were used as transition elements in non-critical stress areas. Seat adjustment mechanisms of
structural significance - such as Hydroloks and recline arms - were modeled using non-linear spring and simple beams elements. The seat
cushion was modeled using CHEXA solid elements with equivalent cushion thickness. The footrest and sled is modeled using CQUAD4 elements
using rigid (MATRIG) material properties. Figure 5-15 shows an exploded view of the finite element structure.
Figure 5-15 Exploded View of FE Seat
seat back seat cushion
5.4.3 METHOD 3 - HYBRID MODELING METHOD Multi-body and finite element techniques can be combined to model structures. This is a common method used in Madymo (although the same
method can be applied in MSC/DYTRAN using the rigid ellipsoid capabilities). The hybrid method is used to simplify the FE modeling
process, replacing non-critical FE elements with multi-body ellipsoids or planes. Figure 5-16 MADYMO Hybrid Modeling Model
Figure 5-16 shows an example of the hybrid modeling techniques used to model the same seat in Section 5.4.2. The seat frame was modeled However, the seat
using a combination of beam and shell elements.
cushion and glareshield was modeled using two ellipsoidal multi-body elements instead of finite elements (as oppose to the finite element cushion in Figure 5-15). In this case, sub-component test must be
conducted to obtain the load-deflection characteristics of the seat cushion and glareshield to charactrize its response during impact. The seat cushion ellipsoids are rigidly connected to the seat bucket at its corner locations using FE-to-multibody constraints. The glareshield is fixed in inertial space. Loads, constaints and
boundary conditions are applied in the same manner as the FE model. In general, hybrid models are less accurate than FE models. The hybrid model uses less CPU resource than a full FE model and is sufficient to predict with reasonable accuracy the deformation of the seat structure and the response of the occupant. 5.4.4 MODELING FAILURE OF JOINTS OR FASTENERS There are numerous methods of simulating structural failures in a nonlinear finite element model. A typical failure mode modeled in
seat analysis is failure of rivet and threaded fastener joints. MADYMO, LS-DYNA, and MSC/DYTRAN have capabilities to model simple shear and tensile failure of fasteners. More complex continuum damage
mechanics (CDM) material failure models are available for structures
modeled with these codes.
As an example, rivet failure can be modeled
using MADYMO node-to-node spotweld constraints as shown
This example defines three node-node spotwelds in MADYMO 5.4 format. The spotwelds are defined as having a maximum allowable normal force of 300.0, and a maximum allowable shear force of 350.0. criteria is defined as follows: The failure
The shear and normal failure criteria exponents are set to 2. exponents determine the rupture criterion shape.
(0.001) specifies the time duration that the failure criteria must be violated before the failure initiates. The spotwelds are defined
between nodes in FE models 1 and 2, node pairs: 743 and 21, 621 and 110, and 1219 and 35. A vector between the nodes of a spotweld must The optional FEMHIS keyword in
have a magnitude greater than zero.
the example requests output of the shear and normal forces.
5.5 RESTRAINT MODELING Restraint modeling techniques are presented for the most common restraint configurations used in FAR Part 23 type aircraft: forward, side and aft facing, 2-5 point restraints. These restraints are almost always composed of two inch nylon or polyester webbing. The belt ends attach to the seat or airframe with a pin joint or an inertia reel/webbing retractor, and are joined together with a metallic buckle on the lap belt. 5.5.1 METHODS There are three possible methods of modeling belt systems: segmented belt model (spring-damper segments). finite-element model (membrane or truss elements). hybrid model combining segmented belts and finite-elements.
ATB and MADYMO offer segmented belt models. LS-DYNA3D, MADYMO, and MSC/DYTRAN have finite elements suitable for restraint modeling. MADYMO has hybrid restraint modeling capability. 5.5.1.1 SEGMENTED BELT MODEL
The segmented belt (available in ATB and MADYMO) is a simple restraint model represented by linear segments with user defined nonlinear spring-damper characteristics including hysteresis for unloading and reloading. Initial slack or tension can be assigned to belt segments. The belt ends can be optionally defined as retractors /pretensioners. The belt segments are attached to the occupant at various points. Belt
segments allow slip along the length of the belt, but not transversely. The lack of lateral slippage may reduce the accuracy of the simulation and belt loads in some cases. The segmented belt is suitable to simulate occupant restraint and predict tensile loads where there is minimal expected transverse slippage. The webbing retractor option of the segmented belt model can simulate pay-out, locking, and pre-tension of a production inertia reel or retractor. The MADYMO segmented belt model can be locked based on user specified sensor signals including vehicle acceleration and belt feed rate. Specify the appropriate locking criteria and the forcedeflection characteristics of the device being modeled. 5.5.1.2 FINITE ELEMENT RESTRAINTS A finite element belt offers the best contact model, including transverse sliding of the webbing on the occupant and seat model. model requires the following inputs: A discrete mesh of the restraint geometry in the pre-test position. Material properties appropriate for the magnitude of loads to be applied. Element properties (cross sectional area or thickness, and formulation) Boundary conditions (contact, belt connectivity, supports). Friction characteristics (static and dynamic coefficients or friction function) The
The mesh should be generated to represent the correct belt geometry as applied to the seated occupant. Contact evaluation must be defined between the nodes or elements and the occupant. Webbing material properties can be obtained from tensile tests. In MADYMO, the recommended 2-d element for belt webbing is the MEM3NL (plane, constant stress triangular elements with in-plane and no bending stiffness) membrane element with HYSISO material (elastic isotropic material with hysteresis). The recommended 1-d element in
MADYMO is the TRUSS2 element (uniaxial with tension and compression stiffness) with HYSISO material definition. For LS-DYNA3D, use the 1-d *ELEMENT_SEATBELT with *MAT_SEATBELT (belt webbing material) and *SECTION_SEATBELT (defines a seatbelt part). LS-DYNA3D also has webbing retractor, pretensioner, accelerometer, sensor, and slipring belt options. In MSC/DYTRAN, use the CROD element with PBELT properties. 5.5.1.2.1 PRESIMULATION It is difficult to manually generate an FE mesh of an applied belt restraint. Finite element belt models typically require a presimulation analysis to obtain the initial nodal coordinates of the belt applied to the occupant. For a membrane belt model, create a flat mesh of the belt webbing and position the segments near the target location on the dummy (Figure 5-17). Use a linear-elastic material with stiffness considerably higher than the actual belt stiffness. This increased stiffness reduces element distortion during the presimulation. Define contact between the belt nodes and the dummy.
Lock the joints to prevent the dummy from moving out of the test position. Figure 5-17 MADYMO 4-Point Restraint Before Pre-simulation
There are various methods of applying the belt to the occupant in each code. In MADYMO, attach belt segments to the end nodes of the belt mesh, and apply pretensioners to pull the belts in to place. In MADYMO and other finite element codes, another method to move the belts into position is to specify a nodal displacement versus time for the belt end nodes. Request nodal coordinate output from the presimulation analysis and use the coordinate output to initialize the positions for the final simulation. Before running the impact analysis, replace the
presimulation material properties with appropriate values, and unlock the dummy joints. 5.5.1.3 HYBRID BELT MODEL
The MADYMO hybrid belt model is simply a finite element belt model combined with segmented belts. The finite element part is usually modeled as the portion of the webbing that contacts the occupant. The segmented belts usually connect the end nodes of the FE belt to the airframe or seat (see Figure 5-18). Use the segmented part of the hybrid belt to model retractors, pretensioners, and sliprings. Figure 5-18 MADYMO Hybrid Belt After Pre-simulation
5.6 MATERIAL MODELS The selection and use of appropriate material models is critical in determining the accuracy of the analysis. The formulation of advanced
material models have increased significantly, and most explicit codes have numerous material models even for a simple material such as aluminum. This makes selecting the correct material models confusing.
For example, LS-DYNA has over 100 material models, with eleven different material models to treat the behavior of foam materials. Thus, a comprehensive discussion on all the available material models is not practical. However, this section will attempt to provide some
guidance on the selection of material models that have been shown to be effective for the analysis of components that are commonly used in seat structures. The first thing to remember in selecting material models is to begin the analysis with simple material models such as an elastic material model. The reason is that simple material models make debugging
easier during the initial stages of the analysis, and allow the program to execute without introducing additional errors. Also, the response of elastic material models is easier to comprehend. The
analyst can view the results, and then make a determination if a more complicated elastic-plastic model is required to further enhance the accuracy of the analysis. Complicated material models require specific inputs and coefficients that are obtained by conducting special tests. For analysis performed
with MADYMO multi-body techniques, component test are required to obtain the load versus deflection characteristics of each structure. User manuals provided with the software provide the descriptions of each material model and suggest applications associated with it. 5.6.1 METALLIC MATERIAL MODELS Material models associated with aircraft seat metallic structures such as aluminum and steel come with a variety of formulations. These materials are considered isotropic (the an-isotropic behavior of thin sheet metals can be neglected as they exhibit such behavior primarily in high-velocity impact sheet metal-forming applications and do not represent the behavior of the same material in seat analysis). The simplest is the elastic material model, which describes a linear relationship between the six stress and strain components. Elastic material model input requires only two material constants: Youngs modulus E and Poissons ratio . If the material is expected to yield under crash loads, an elasto-plastic model can be used (Figure 5-19). In this case, the material will undergo linear elastic and linear plastic strain (bilinear or piecewise linear). In addition, most codes will also allow for a failure strain value to be defined.
Figure 5-19 Elasto-Plastic Material Model
The elastic constants, along with the yield stress, material density and hardening modulus can be obtained from MIL-Handbook-5. Linear properties for Aluminum 2024-T3 and 4130 Steel are listed in Table 5-4. Table 5-4 Input Data For Aluminum 2024-T3 and 4130 Steel
Youngs Modulus (psi) 1.05E+7 2.90E+7
Poissons Ratio 0.3 0.32
Yield Stress (psi) 48000 75000
Density (lbfs2/in4) 0.0002621 0.000741
Aluminum 2024-T3 Steel 4130
Table 5-5 shows a matrix of cross-reference for the different elastic and elasto-plastic models for the different codes. These input cards
are valid for shell elements, and the user needs to reference the users manual for the appropriate material card for other elements. Table 5-5 Matrix of Material Models for Metallic Structures
Analysis Code MATERIAL MODEL Elastic ElasticPlastic MSC/DYTRAN DMATEL DMATEP LS-DYNA3D *MAT_ELASTIC *MAT_PLASTIC_KINEMATIC MADYMO ISOLIN ISOPLA
For some metals, such as mild steel, the material yields at a higher effective stress state at increased strain rates. The strain rate sensitive behavior of steel has significant benefits for crashworthiness applications as it increases the stiffness of the structure under crash loads. formulated as
 ) + y ( p ) d = y g (
The strain rate hardening law is
where y 0 is the initial yield stress, g the strain rate dependency function and p is the effective plastic strain. The strain rate
dependency function is treated using the Cowper-Symonds strain rate empirical function   ) =1 + g ( c 1
where C1 and C2 are strain rate enhancement coefficients.
MSC/DYTRAN, the rate effects are modeled using the DYMAT24 material card. An example input card for 4130 steel (in English units) is
shown in Figure 5-20 where the C1 and C2 are strain rate enhancement coefficients are 40.4 and 5.0 respectively. Figure 5-20 Example MSC/DYTRAN Input for Strain Rate Material
$ -------- Material 4130_steel_solid id =7 DYMAT24 7 .000741 2.9e+07 .32 +A000509 +A000510 75000 0.37 40.4 + DYNA
The rate effects can also be modeled using the MAT_PLASCTIC_KINEMATIC material input card in LS-DYNA3D where the SRC and SRP input card represents the C1 and C2 strain rate enhancement coefficients. An example input deck is provided in Figure 5-21. Figure 5-21 Example LS-DYNA3D Input for Strain Rate Material
*MAT_PLASTIC_KINEMATIC $ MID RO 2 0.000741 $ SRC SRP 40.4 5.0 E 2.9+7 FS .37 PR 0.32 SIGY 75000 ETAN 176000 BETA 0
In MADYMO, the strain rate effects for steel can be modeled using the ISOPLA material card. in Figure 5-22 Figure 5-22 Example MADYMO Input for Strain Rate Material
MATERIALS * CollectorName>> 4130N steel TYPE ISOPLA E 2.000E+11 DENSITY 7915 YIELD STR 5.172E+08 RATE DEP COWPER DRATE 40.4 PRATE 5.0
An example input format (in SI units) is shown
5.6.2 COMPOSITE MODELS Laminated fiber-matrix materials such as fiberglass-epoxy are frequently used in aircraft seats, glareshields, side ledges, cabinets, and tables. Finite element codes like LS-DYNA3D and MSC/DYTRAN typically include material models for composites. Laminated structures with or without a core can be modeled using a shell element mesh. Techniques for modeling composite structures are described in the following sections. 5.6.2.1 MODELING COMPOSITES WITH LS-DYNA3D.
There are several options for modeling layered composites with shell elements. The simplest and least general is to use the BETA option of
*Section_Shell to define the material direction for each integration point through the element thickness. A user-defined integration rule
should also be used to control the layer thickness. (see IRID of *section_shell, and integration_shell). If a composite is made up layers of different materials, a more general composite can be modeled by specifying a different part ID for each integration point (see *integration_shell). Each part can refer to a different material
model with the restriction that all materials must be of the same type. For example, you could specify an element with one layer of material type 2 using Ea=10, Eb=1, and another layer of material type 2 with Ea=3, Eb=3, where Ea and Eb are the Young's modulus in the 'a' and 'b'
This method allows different material constants to be
used in the different layers, but still does not allow complete general mixing of material types in a single shell element. Figure 5-23 User Defined Shell Integration Points
For complete freedom of mixing materials in a composite, it is necessary to model the section with multiple elements, one element for each material type in the composite. The elements should all be given
a thickness equal to the total composite thickness and should all share the same nodes, so they would appear to all lie in the same space when viewed in a preprocessor or postprocessor. However, in
order to obtain the correct membrane and bending stiffness for the whole composite element, define a separate integration rule for each element in the composite with appropriate weights and through thickness locations.
A simple example of a sandwich type composite with one material in the middle and another on the top and bottom surface might have integration rules like this. The middle material could have 2
integration points with weights and thickness coordinates of Wf1 = 0.25, S1 = -0.25 Wf2 = 0.25, S2 = +0.25 The surface material could have 2 integration points with weights and thickness coordinates of Wf1 = 0.25, S1 = -0.75 Wf2 = 0.25, S2 = +0.75 In this example, Wf1 is the weight factor for integration point 1, and S1 is the thickness direction coordinate of integration point 1 etc.
The correct stiffness is achieved so long as the total weight of all elements is equal to 1, and the thickness coordinates are defined such that the integration points are at the middle center of each layer. This method has complete freedom of material type for each layer. seems like a great idea, but LS-DYNA has built in protection to prevent the input of weights that don't add up to 1. If you try the It
example, it converts the weights at all integration points to 0.5 so that they add up to one for each element. trick to get around this protection. The idea is to reduce the thickness of elements accordingly so that the correct membrane stiffness is achieved for each material. In Fortunately, there is a
other words, each element should have a thickness equal to the actual
summed thickness of layers of that material.
element thickness of both elements should be reduced to one half the total composite thickness. To achieve the correct bending stiffness
for the composite, the thickness coordinates for each integration point should be increased accordingly. In the example, since each
element has been reduced to half the composite thickness, the thickness coordinates should be doubled, so S1=-0.5, S2=+0.5 for the middle material, and S1=-1.5, S2=+1.5 for the surface material. Notice that this violates the usual restriction that the thickness coordinates should be in the range of -1 to +1. because LS-DYNA does not enforce this rule. In this simple example, each of the 4 material layers has a thickness of 1/4 of the total element thickness. However, there is absolutely However, it works
no restriction on the number of layers, thickness of layers, or material of the layers using this method. The only rules that should
be followed to achieve correct stiffness of the overall composite element are: 1. The sum of individual element thickness should equal the total composite thickness. 2. The thickness coordinates for each integration point should be multiplied by the total composite thickness and divided by the corresponding element thickness. If multi-element method is used, care should be taken if the composite is to be checked for contact. Only one of the elements making up the
composite should be checked for contact since all elements share the
However, the element thickness will be less than the
composite thickness, so it may be desirable to directly prescribe the thickness for contact (see SST,MST on *contact) if using a contact type where element thickness is taken into account. 5.6.3 SEAT CUSHION FOAM MODELS The selection of the appropriate foam model for modeling seat cushion is critical in obtaining accurate spine load prediction. Foam models For
are typically formulated for a particular type of foam behavior.
instance, LS-DYNA3D has different material models for commonly used aircraft seat cushion foam such as DAX (polyurethane) versus slow recovery foams such as Confor. Other codes such as MADYMO rely on the
user to obtain the specific load versus deflection response of the foam from a component level test as input data for the foam material model. The following is an example of seat cushion foam modeling
using MSC/DYTRAN. 5.6.3.1 SEAT CUSHION MODELING USING MSC/DYTRAN
The seat cushion can be effectively modeled using the FOAM1 material model. The model assumes a crushable material where the Poissons The yield behavior of the foam is
ratio is effectively zero.
determined by a stress-strain or crush-strain curve, typically obtained through a uni-axial compression test. The crush-stress input data for the FOAM1 material model can be obtained by conducting a high velocity impact test (reference AGATE
Report C-GEN-3432A-2 for test methodology, Figure 5-24). This impact test captures the dynamic response of the seat cushion material. In
cases where the foam is not as sensitive to the rate of loading, a comparable static test (reference AGATE Report C-GEN-3432A-2 for test methodology) is sufficient to capture the response of the foam. Figure 5-24 Foam Impact Test
As an example, an impact test was conducted on HR polyethelene foam of thickness and build-up that represents the actual seat cushion design. A leather fabric was sewn over the foam to represent the seat cover. A 51-lbm impactor was dropped on the foam sample at a velocity of 10 ft/s to obtain the bottom-out response of the seat cushion (Figure 5-25).
Figure 5-25 Stress-%Crush Foam Data
Since the MSC/DYTRAN FOAM1 material model does not incorporate hyteresis effects, only the loading function was used for the analysis. The corresponding FOAM1 input deck is shown in Figure 5-26 Figure 5-26 Example of FOAM1 material model
$ -------- Material foam id =11 HR 10/30 FOAM1 11 3.33e-6 75.00 6 CRUSH + DYNA 1.6 0.1 $ dynamic test data HR10 with 12"x12" leather cover TABLED1 6 +,.0,.0,.067646,0.109,.132487,1.051,.187033,1.540,+ +,.261175,1.901,.324763,2.221,.387647,3.204,.449529,4.253,+ +,.510053,5.765,.568779,7.747,.625082,10.20,.678216,12.99,+ +,.727285,16.58,.771185,20.79,.808633,25.34,.838227,29.96,+ +,.858571,34.07,.868466,35.84,ENDT
5.7 APPLYING BOUNDARY CONDITIONS Multi-body and finite element modeling requires the application of various boundary conditions. For dynamic seat modeling, typically only
nodal constraints and contact definitions are required.
include the application of nodal displacement constraints (or SPCs) to the seat feet, for example, to represent attachment to the aircraft. 5.7.1 KINEMATIC CONSTRAINTS Kinematic constraints consist of single (SPC) or multi-point constraints (MPC). In theory, kinematic constraints constitute the
release or removal of a particular degree of freedom. For MPCs, the motion of a dependent degree of freedom is expressed as a linear combination of one or more independent degrees of freedom. In practical terms, they are used to tie a structure to the ground, to apply symmetric boundary conditions, to remove degrees of freedom that are not used in structural analysis, or to tie structures together. SPCs and MPCs in dynamic analysis are applied in the same manner as static finite element analysis. An in-depth discussion is not required. A particularly effective constraint tool is the MSC/DYTRAN RCONN (equivalent to SPOTWELD in MADYMO) capability. RCONN is used to
connect different parts of the mesh together without having to condense adjacent nodes. structures. The desired effect is to simulate welded
RCONN represent a more sophisticated forms of MPC. In Figure A,
An example application of RCONN is shown in Figure 5-27.
the gusset and the seat frame finite element mesh were modeled in separate groups. They are then tied together using the RCONN card to
simulate a welded structure.
In MSC/DYTRAN, the RCONN input card structure is similar to the CONTACT card. The user needs to specify a set of slave nodes that The user will also need to define a
will be tied to a master surface.
monitoring distance, such that nodes with distance larger than the specified range will not be included in the connection. input deck is shown in Figure 5-28. Figure 5-27 Rigid Connections An example
Fig. A -rigid connection between gussets and seat frame
Fig. B - rigid connection between gussets and seat frame
Fig. C - rigid connection between vertical tube and seat base
Figure 5-28 Example RCONN Input Deck
$--------- web-tube weld RCONN 26 GRID SURF 1 +A000073 +A000074 NODISTANCE .020 $ $ Slave contact surface for web-tube $ SET1 1 1402 1405 1411 $ $ Master contact surface for web-tube $ SURFACE 2 SEG 2 CFACE 1 2 772 1 CFACE 2 2 773 1 CFACE 3 2 774 1
+A000073 +A000074
The slave nodes of the web (defined in SET1 entry) are connected rigidly to the master surface of the tube structure (defined in the SURFACE entry). The monitoring distance was set at 0.020 inches.
5.7.2CONTACT DEFINITION Contact definitions are required to evaluate the interactions between the seat and the occupant, between seat components, occupant self contact, occupant-to-occupant contact, and interactions with other objects in the aircraft interior. Without contact definitions, a
simulation will allow entities to pass through the same space resulting in inaccurate simulation. Defining contact correctly
requires understanding the assumptions of the contact algorithm used in the analysis code. Consult the software documentation for details Although the algorithms vary for
on the limitations and assumptions.
the different analysis codes, the input requirements are usually similar.
Generally, it is required to define master and slave contact entity sets (nodes, elements, rigid bodies). The rule of thumb is to assign
the coarse mesh as the master surface and the finer mesh as the slave surface. If the mesh densities are similar, the slave surface should
be the surface with the softer underlying material. Also, when selecting elements for contact analysis, it is better, in general, to use first-order elements for those parts of the model which will form a slave surface. interactions. Static and dynamic friction coefficients are also required. Sometimes it is required to define contact surface direction, search radius, damping parameters, contact stiffness, contact start/stop time, or other parameters. Initial penetration can be a problem in cases where finite element membrane mesh is applied to a multi-body occupant. Due to the This specifies which objects to include in contact
discretization of the belt model, it is easy to have a few nodes that are just below the surface of the occupant skin. Most contact
algorithms calculate the contact force vector based on the restoration force required to move an intersecting slave node to the surface of the master entity. Without some method of compensation, the
penetrated nodes will create enormous contact restoration forces resulting in numerical instability. To correct this, some codes can
detect penetration of master and slave contact entities at the start of the simulation by turning on the penetration check option in the
contact definition card. The code will adjust the violating node(s) or offset the initial contact forces to equilibrium. Surface-to-Surface and Surface-to-Nodes are the two most commonly used contact algorithms. Surface-to-Surface contact definitions are used where shell elements are anticipated to contact each other. Surface-
to-Nodes contact is defined where the elements form a T-join between surfaces. Examples of contact applications are shown in Figure 5-29. Figure 5-29 Contact Applications
Fig. A - surface-surface contact between inner and outer pivot tube assy Fig. B - surface-node contact between reclinearm and base assy
inner tube outer tube
active contact surfaces on base assy
active contact nodes on reclinearm Fig. C - surface-surface contact between seat bucket and base
Since the contact search process is computationally expensive, it is recommended to minimize the entities included in the contact model. Predicting the kinematics of the simulation and estimating contact points can help to choose the appropriate contact entities. For
example, simulating a pilot seat dynamic test, if it is expected that the occupant head will strike the instrument panel finite element mesh, choose a set of nodes in the expected contact area rather than the entire panel mesh. If necessary, the selected set can be adjusted
after reviewing the results, and the simulation re-run. 5.7.2.1 DEFINING CONTACT WITHIN MSC/DYTRAN
An example MSC/DYTRAN surface-to-surface contact input deck is shown in Figure 5-30. The deck defines the contact interactions between the inner and outer pivot assembly shown in Figure A. Figure 5-30 MSC/DYTRAN Surface Contact Definition
$ -------- Contact : inner to outer pivot assembly CONTACT 299 SURF SURF 73 74 +A000644 V4 BOTH 1.0 +A000645 +A000646 ON $ Slave elements SURFACE 73 SEG 73 CFACE 2163 73 5493 1 CFACE 2164 73 5494 1 . . CFACE 2171 73 9333 1 $ Master elements SURFACE 74 SEG 74 CFACE 3252 74 5402 1 CFACE 3253 74 5403 1 . . CFACE 3271 74 5441 1 .3 0.1 .3 .1+A000644 +A000645 +A000646
The contact specifies that the outer tube slave surface (defined by SURFACE 73) to be checked for contact with the inner tube master surface (defined by SURFACE 74). The outer tube is designated as the slave surface because it has a finer mesh in comparison to the inner tube. The value of the static and dynamic coefficient is 0.3. The
contact employs a Version 4 algorithm (V4 input), which simultaneously tracks multiple contacts per slave node. By specifying BOTH in the contact card, slave nodes are check for penetration on both sides of the master element regardless of the direction of the normal vector on the master surface. 5.7.2.2 DEFINING CONTACT WITHIN MADYMO
Contact in MADYMO can be defined between multi-body elements, and also between finite element models and multi-body elements. An elastic
contact algorithm is used for multi-body contacts, where the contact characteristics are user defined and the resultant contact force is a function of penetration depth. A kinematic contact algorithm is used
for finite element to multi-body contact problems, and the contact force is calculated based on the relative velocity of the node and contact surface. In most cases, contact characteristics are obtained
from component test and specified in terms of force versus deflection. Contact is defined in MADYMO via the CONTACT INTERACTIONS card. An example application of multi-body contact and input deck is shown in Figure 5-31 and Figure 5-32. The occupants head (system 1, body 6) and the glareshield (system 6, body 2) are modeled as ellipsoids. The
ELLIPSOID-ELLIPSOID card is used, and the stiffness characteristic of the glareshield is defined in the FUNCTIONS card. Figure 5-31 MADYMO Multi-Body Contact
Figure 5-32 Multi-body Contact Definition
CONTACT INTERACTIONS FUNCTIONS ELLIPSOID-ELLIPSOID ! contact between glareshield and dummy's head 6 2 1 6 4 -5 0 -1e+06 0.000000 0.000000 0.300000 1 0 0 END ELLIPSOID-ELLIPSOID FUNCTIONS ! glareshield load-deflection curve 27 0.0000 0.0000 0.001 163.8842 0.0030 326.5717 . . 0.0267 1873.9352 END FUNCTIONS END CONTACT INTERACTIONS
5.8 LOAD APPLICATION There are two methods to simulate crash loads. Method One: Prescribe the initial velocity (or velocity prior to impact) to the seat and occupant, and apply deceleration to the sled. This method simulates the physical impact event, as experienced by the occupant. Method Two: Apply the acceleration field to the occupant while maintaining the sled/seat as a stationary frame of reference. This
method is an approximation of the impact event, because it assumes that the acceleration measured by the sled is the same as the occupant. The crash loads are applied in reverse of the actual
physical event i.e. by applying an acceleration pulse to the occupant instead of a deceleration pulse to the seat and allowing the occupant to decelerate on its own. This method is acceptable only when the
inertial effects of the seat are negligible in the direction of the applied load. The advantage of applying the acceleration field to the
occupant is that it allows for the simulation of the 1 G pre-load, which is critical in predicting spine loads. Using this method, the
impact acceleration can be offset by a certain amount of time to allow for the occupant to sink into the seat cushion. 5.8.1 LOAD APPLICATION FOR 60 DEGREES PITCH TEST The illustration presented here is based on the second method described above. Two sets of load are required.
A 1 G gravity load in the negative Z direction (down) applied to the seat and occupant, and
The crash load simulating the 60 degrees pitch condition.
The crash acceleration profile used in the simulation can be in the form of an idealized triangular pulse per 23.562 or from actual test data. 5.8.1.1 EXAMPLE: LOAD APPLICATION WITH MSC/DYTRAN
Method 2 is utilized in this example.
An acceleration field is
applied to the occupant while maintaining the sled/seat as a stationary frame of reference. The 1 G gravity load is applied to the The crash
occupant via CARD A3 in the *ain data deck (Figure 5-33).
pulse is applied to the ATB occupant by means of the MSC/DYTRAN ATBACC and TLOAD card (Figure 5-34). The 600 vector is defined in the ATBACC
card by using a load factor of (-0.5, 0.0, 0.866) in the (X,Y,Z) direction consistent with the direction of the occupant coordinate system. The crash pulse has an offset of 150 milliseconds from time
zero to allow for adequate 1-G cushion pre-loading (Figure 5-35). Figure 5-33 ATB 1 G Load Application Pitch Test
CARD A1B CARD A1 CARD A3
SITTING HYBRID II DUMMY (50%) GENERATED WITH GEBOD AGATE SLED TEST IN. LB.SEC. 0.0 0.0 -386.088
Figure 5-34 MSC/DYTRAN Load Application Pitch Test
$Crash Pulse ATBACC,201,,386.04,-.5,0.0,-.866,,,+ +,LT,MT,UT,N,H,RUL,RLL,RF,+ +,LUL,LLL,LF,RUA,RLA,LUA,LLA $ TLOAD1,13,201,,,1000 TABLED1,1000,,,,,,,,+ $ ACCELERATION WITH 0.15 SEC 1 G LOAD +,0.0,0.0,0.150,0.0,0.16,4.92633,0.165,7.11431,+ +,0.17,10.4175,0.175,13.2985,0.18,14.6757,0.185,15.0433,+ +,0.19,16.9036,0.195,18.296,0.20,18.8951,0.205,19.0857,+ +,0.21,18.2143,0.215,17.4943,0.22,15.7737,0.225,15.8078,+ +,0.23,15.434,0.235,12.5829,0.24,5.92312,0.245,0.26516,+ +,0.25,-1.39478,0.255,0.0,0.35,0.0 $
Figure 5-35 Test 1 Applied Loads
1 G Preload
5.8.2 LOAD APPLICATION FOR 10 DEGREES YAW TEST The illustration presented here is based on Method 1. load are required. 1. A 1 G gravity load in the negative Z direction (down) applied to the seat and occupant, and Two sets of
The crash load simulating the 10 degrees yaw condition.
The crash acceleration profile used in the simulation can be in the form of an idealized triangular pulse per 23.562 or from actual test data. 5.8.2.1 EXAMPLE: LOAD APPLICATION WITH MSC/DYTRAN
A 1-G gravity load is applied in the negative Z-direction.
The 1-G
load is applied to the seat via the MSC/DYTRAN TLOAD1 and GRAV card. The crash scenario is simulated by prescribing an initial velocity prior to impact to all elements in the model, and applying a deceleration field to the sled. The ATB initial velocity is prescribed in the ATB input deck using the G2 card. All other MSC/DYTRAN elements receive the initial velocity Both ATB and MSC/DYTRAN initial
definition through the TICGP card.
velocities are defined at a vector of 100 from the horizontal plane to simulate the yaw condition. The sled is decelerated by prescribing a
velocity profile (Figure 5-36) to all of the elements of the sled using the TLOAD1 and FORCE cards. Figure 5-36 Test 2 Applied Loads
Figure 5-37 MSC/DYTRAN Load Application Yaw Test
$ATB Input Deck: Initial velocity definition -117.523 0.00 -27.9607 -476.9 84.07 0.00 CARD G2 $_________________________________________________________________________________ $MSC-DYTRAN Input Deck: Initial velocity & prescribed motion definition $ ------- GRAVITATION ----$1 G Load applied to the seat TLOAD1 13 444 0 GRAV 444 32.17 0 0 -1.0 $ ------- Initial Velocity BC initial velocity entire model ----TICGP 13 200 XVEL -476.9 YVEL 84.09 $ SET1 200 1 THRU 2548 2550 THRU 4413 4421+A000652 +A000652 THRU 4509 4515 THRU 8026 8139 THRU 8538+A000653 +A000653 9000 THRU 9135 12020 THRU 13102 14500 14501+A000654 $ ========= PRESCRIBED SLED MOTION ========== $ Apply prescribed velocity profile to rigid elements that represents the sled TLOAD1 13 294 2 90 FORCE 294 12020 0 1 -.9848 .1736 0 FORCE 294 12024 0 1 -.9848 .1736 0 . . FORCE 294 44479 0 1 -.9848 .1736 0 $ Pulse from crash test $ ------- TABLE 90: velocity_table ------TABLED1 90 +A000658 +A000658 0 484.3 .004 483.3 .005 481.6 .007 480.8+A000659 +A000659 .009 480 .0094 478.7 .0098 477.1 .01 476.3+A000660 +A000660 .0105 474.5 .011 473 .0115 471.8 .0125 469.7+A000661 +A000661 .0135 467.7 .0145 464.4 .015 461.7 .02 435.5+A000662 +A000662 .03 363.7 .04 278.4 .05 177.3 .055 126.3+A000663 +A000663 .06 75.9 .065 27.3 .067 8.3 .0678 .76+A000664 +A000664 .15 0 ENDT
The data deck in Figure 5-37 shows the finite element nodes (specified by SET1 and TICGP card) and ATB (last three entries of the G2 card) has initial velocities of (-476.9,84.09,0.0) in/s. This translates to a resultant impact velocity of 484.2 in/s (40.35 ft/s). The TLOAD1
card then prescribes a velocity change for the sled (elements 12020 through 44479 defined in the FORCE card) as specified in TABLE1 card profile.
5.9 FLOOR DEFORMATION The specific method for simulating floor deformation is code dependent. In MSC/DYTRAN, the 100 pitch and roll seat legs floor
deformation can be simulated by prescribing a time dependent velocity profile to the nodes corresponding to the location of the seat feet attachments. Integration of the velocity profile will yield the
required displacement of the seat legs nodes, which will then create a pre-stress on the seat. In MADYMO, floor deformation can be accomplished by enforcing a prescribed displacement. In either case, enforced motion in transient
analysis can result in numerical instability if it is incorrectly executed. 5.9.1 EXAMPLE FLOOR DEFORMATION SIMULATION USING MADYMO Floor deformation can be modeled in MADYMO by using null systems and attaching it to the seat feet fittings (a null system is used to model a system of a body with known motion relative to inertial space). Each null system, attached to the inboard or outboard seat leg, is prescribed a 100 pitch and 100 roll motions corresponding to actual test requirements. Typically, floor deformation simulation has to be
performed for a minimum duration of 200 milliseconds to avoid numerical instability. An example input deck illustrating floor deformation using null systems is shown in Figure 5-38.
Figure 5-38 Floor Deformation Using MADYMO
NULL SYSTEM INBOARD FWD LEG PITCH DOWN MOTION POSITION 0.0 0.05 -0.2286 -.05 0.01 0.055 -0.2286 -.10 0.35 0.055 -0.2286 -.10 END POSITION END NULL SYSTEM NULL SYSTEM OUTBOARD FWD LEG ROLL OUT MOTION POSITION 0.0 0.05 -0.4445 -.05 0.01 0.05 -0.47 -.04 0.35 0.05 -0.47 -.04 END POSITION END NULL SYSTEM NULL SYSTEM OUTBOARD AFT LEG ROLL OUT MOTION POSITION 0.0 0.05 -0.4445 -.05 0.01 0.05 -0.47 -.04 0.35 0.05 -0.47 -.04 END POSITION END NULL SYSTEM ! constrain inboard fwd leg nodes to null system 1- pitch down NUMBER 6 NULL SYSTEM 1 DOF ALL SET 82 ! constrain outboard fwd and aft leg nodes to null system 2 roll out NUMBER 7 NULL SYSTEM 3 DOF ALL SET 62
5.9.2 EXAMPLE FLOOR DEFORMATION SIMULATION USING MSC/DYTRAN The floor deformation requirements can be simulated using a combination of the TLOAD1 and FORCE3 card. shown in Figure 5-39. An example input deck is
Figure 5-39 Floor Deformation Using MSC/DYTRAN
$============================================================================= $ ========= FLOOR DEFORMATION: 10 DEGREES PITCH & ROLL ========== $============================================================================= $ $ Inboard leg rotation coord system CORD1C 1 368 346 54 $ Outboard leg rotation coord system CORD1C 2 346 54 80 $ $ 10 deg. Pitch down on inboard seat leg TLOAD1 1 995 2 995 FORCE3 995 80 1 5.8178 1. 0. FORCE3 995 323 1 5.8178 1. 0. FORCE3 995 366 1 5.8178 1. 0. . . . FORCE3 995 104 1 5.8178 1. 0. TABLED1 995 + + 0.0 0.0 0.02 1.0 0.03 1.0 0.05 0.0+ + 1.0 0.0 ENDT $ $ 10 deg. Outbd roll outboard seat leg TLOAD1 1 996 2 996 FORCE3 996 332 2 5.8178 -1. FORCE3 996 344 2 5.8178 -1. . . FORCE3 996 78 2 5.8178 -1. TABLED1 996 + + 0.0 0.0 0.02 1.0 0.03 1.0 0.05 0.0+ + 1.0 0.0 ENDT
A coordinate system is specified for each inboard and outboard seat rail, by means of the COOR1C card, to define a rotation axis for the seat leg. The TLOAD1 card then specifies the nodes, defined in the
FORCE3 cards, to rotate in accordance with the COOR1C rotation definition and the velocity change function in TABLE1 card. Figure 5-40 shows a seat with floor deformation simulation using the technique described above.
Figure 5-40 MSC/DYTRAN Pitch and Roll Simulation
6. GENERAL DISCLAIMER This document serves as a guideline in the application of computer models for the design and certification of seat/restraint systems. The information presented reflects the state of the computer
simulation technology at the time this document was developed. Specific modeling techniques may in fact become obsolete as technology progresses. In addition, there are other methods of modeling seating systems that are equally valid but are not specifically covered in this report. Although this document provides detailed guideline to the certification of seat designs, it does not guarantee certification. The user must still coordinate and gain approval with the FAA on the specifics related to the products certification. To the extent permitted under applicable law, the user accepts responsibility for any liability stemming from the application of this document, and agrees to hold Cessna Aircraft Company and any member of AGATE harmless from any claims of liability arising from the users commercial use of the information produced in this document. 7. ACKNOWLEDGEMENTS Special appreciation to the following members of the AGATE Advanced Crashworthiness Group who provided valuable guidance and criticism in the development of this document. Mr. Pat Mullen FAA Small Airplane Directorate Mr. Steve Soltis FAA National Resource Specialist Dr. Steve Hooper AGATE Systems Engineer Dr. Joseph Pelletteire Wright Patterson Air Force Research Labs
Dr. Karen Lyle NASA Langley Dr. Ken Lou Simula Technologies Inc. Mr. Todd Hurley Simula Safety Systems Inc. Ms. Marilyn Henderson National Institute Aviation Research, Wichita State University Mr. Thomas Hermann Raytheon Aircraft Company Ms. Sonja Englert ModWorks Mr. Paul Yaklin Cessna Aircraft Company Mr. Todd Bevan The Lancair Company
Documents similaires à aircraft crash analysis
Yokohama Revised
Plus de Srinivas Rallabandi
count id 32-new
Value Stream Analysis of Manufacturing Engineering
Tutoarial5
Tutoarial4
Tutoarial6
Tutoarial1
Tutoarial7.pdf
Tutoarial3.pdf
Tutoarial2