GALCIT SM Report 87-19 

POSTBUCKLING DELAMINATION OF A STIFFENED COMPOSITE PANEL USING 

FINITE ELEMENT METHODS 

S. Natsiavas", C.D. Babcock** and W.G. Knauss** 

1 

California Institute of Technology 

Pasadena, California 91 125 

August, 1987 

(NASA-CR-182803) POSTBUCRLIIG DELAHINBTIOB N 8 8- 220 98 

OF A STIFFENED COHPOSITE PANEL USING FINITE 

ELEEENT PlETHODS ;California IInSta of Tech, 1 

20 P CSCL llD Unclas 

G3/24 0141220 

Research Fellow in Mechanical Engineering and Aeronautics 

Professor of Aeronautics and Applied Mechanics 

* 

** 
ABSTRACT 

A combined numerical and experimental study is carried out for the postbuckling 

behavior of a stiffened composite panel. The panel is rectangular and is subjected to static 

in-plane compression on two opposite edges to the collapse level. Nonlinear - large deflection - 

plate theory is employed, together with an experimentally based failure criterion. It is found that 

the stiffened composite panel can exhibit significant postbuckling strength. 

INTRODUCTION 

An understanding of the behavior of composite structures is important since these 

structures are increasingly finding wide use in many Engineering fields. An area of special 

interest is the investigation of the failure mechanisms in multilayered composite panels subjected 

to in-plane compression. The available data in the literature indicate that composites may have 

considerable postbuckling strength, depending on ply thicknesses and orientation [ 1-31. 

Ignorance of their response and failure mechanisms results in an excessively conservative 

design, which does not fully exploit all of the possible structural advantages. 

The problem of the postbuckling behavior has been extensively studied for metal 

structures, but some new phenomena may arise for layered composite structures. For example, 

one of the most frequently observed failure in stiffened composites is debonding and separation 

of stiffeners as the structure is loaded into the postbuckling regime. This failure is caused by the 

step change in thickness induced by the attachment of the stiffeners to the panel. When the panel 

buckles, some joints may fail, which leads to separation of a stiffener from the panel. This 

separation results in loss of the postbuckling load carrying ability and hence lowers the ultimate 

strength of the structure. 

In order to be able to construct safe and efficiently stiffened panels from composite 

materials, it is necessary to fust understand the mechanics of the stiffener/panel separation 

process. This understanding requires examination of the postbuckling behavior of the panels, 

which involves large out-of-plane displacements relative to the panel thickness. This situation in 

1 
turn implies that the governing equations are nonlinear, which makes it virtually impossible to 

obtain closed form solutions. As a result, the most commonly employed analytical studies on the 

subject are limited to finite element or other energy type methods [l-81. In some of these 

approaches [5-71 documented to date, the composite plate is assumed to be isotropic or 

orthotropic and the emphasis is placed in the panel deflections or stresses under idealized 

boundary conditions. The finite element analysis performed in reference [3] assumes the plate to 

be anisotropic but idealized boundary conditions. This approach does not allow interaction 

between the panel and the stiffener. Finally, a more sophisticated analysis is presented in [l], in 

which the panel is modeled as a plate while parts of the stiffener are modeled as beams and parts 

as plates. This modeling is more accurate in that when the stiffener is modeled as a beam, 

distortion is not considered, which may thus result in considerable inaccuracies, depending on 

the properties of the stiffener and the panel. 

OBJECTIVE AND METHODOLOGY 

As is clear from the foregoing discussion, the existing models for the behavior 

of stiffened composite panels are still in the development stage. By using the assumptions of 

plate theory, these analysis predict the resultant forces and moments, while the displacement and 

stress fields are expected to be valid sufficiently far away from the joints. On the other hand, 

failure of the structure is most likely to occur along the lines where the thickness changes 

abruptly. For example, a sharp discontinuity will lead to a singular stress field at a reentrant 

comer. The determination of this stress field will depend heavily on the degree of idealization 

by the model [9,10]. The analysis becomes even more complicated if one attempts to account 

for interlanlinar stresses at free edges [ll-131. 

In an effort to overcome the complexities associated with tlle conversion of resultant 

forces and moments to the three-dimensional stress field ne.ar the step in thickness, a simplified 

approach is adopted here. In the absence of a suitable failure criterion for the delamination of 

stiffened composite panels, the prediction of their ultimate strength is unavoidably dependent on 

experimental data. For a given panel stiffener construction and configuration, the relation 

2 
between the macro stresses (resultant forces and moments) and the micro stresses near the 

thickness discontinuity will be the same. Therefore, the failure condition for a fixed 

panel/stiffener intersection may be characterized in terms of resultant forces [14]. 

Tlie objective is to first establish a failure envelope of the resultant forces, by performing 

experiments with the panel. Having this envelope, one will then have to determine analytically 

the levels of the applied loads which result in a critical combination of the resultant forces near 

the joints. Of course, such an envelope will depend on the properties, combination and 

orientation of the constituent laminae, as well as the configuration of the joints. However, this 

envelope will be the same for various stiffener spacings, provided that this spacing is long 

enough for the natural diffusion of the resultant forces to micro stresses to occur. 

EXPERIMENT 

Test Swcimen 

Determination of the failure envelope can be achieved by testing only a part of the whole 

panel. The specimen tested in this investigation was supplied by staff at NASA Langley and its 

dimensions are shown in Figure 1. The panel was constructed from 16 layers with orientation 

k45/90/0]~. Each lamina has a thickness of about 0.14 mrn and behaves as an orthotropic 

material with the following properties 

El = 13.1*10~0 Pa, E2 = 1.3*1010 Pa 

GI* = 0.64*1010 Pa, vi2 = 0.38 

The stiffener was constructed from 8 additional layers of the same material, with orientation 

k4514. As shown in Figure 1, the stiffener occupies the area (ACHJ). 

During testing, the edges AE and FJ were clamped on an aluminum frame, while the 

support provided along BI and DC simulated simply-supported conditions. The panel was 

loaded by applying compression on the edges AE and FJ, as explained next. 

3 
Test Setup 

A 300 Klb - capacity hydraulic testing machine was used to apply the compressive 

loading on the specimen. The specimen was placed between the flat plates in the testing 

machine and adjusted for vertical alignment. Loading was applied in a displacement controlled 

fashion. In-plane and out-of-plane displacements at selected locations were monitored during 

the course of the experiment. Dial gauges resolving 10-4 inches and LVDT’s were used for 

measuring these displacements. A load cell mounted in series with the specimen between the 

flat plates in the loading machine measured the load applied. The load displacement response 

was recorded until the specimen failed in the post-buckled region. 

ANALYSIS 

A fmite element model was developed for the pre- and postbuckling calculations of the 

test specimen described in the previous section. The MSC/NASTRAN computer code was 

employed by utilizing the mesh shown in Figure 2. Both the unstiffened and the stiffened parts 

of the composite were modeled using plate elements. Each of the 210 rectangles in Figure 2 

represents a 4-node quadrilateral anisotropic plate element (CQUAD4). Each node of these 

elements has five degrees-of-freedom, including the three displacements (u,v,w) and two 

rotations (aw/ax and aw/ay). Both membrane and bending effects are thus considered, with the 

transverse shear being neglected. The 8-node elements would have been more appropriate for 

this type of problem, but they are not available in NASTRAN for calculations involving 

geometrical nonlinearity [15]. 

The stiffness matrix for each element is computed by the code, taking into account the 

orientation and the material properties of each individual lamina and using the assumptions of 

classical laminate plate theory. The boundary conditions were chosen to simulate as closely as 

possible the experimental conditions and they were as follows: 

On AE: u = v = w = awlax = aw/ay = 0 

On FJ: 

On BI,DG: 

u = aw/ax = aw/ay = 0, 

w = aw/ay = 0. 

N, = -N = constant 

4 
With these boundary conditions, the total number of degrees-of-freedom for the mesh 

considered is 1020. In the calculations, the uniform compressive force applied on FJ was 

increased gradually and with relatively large increments before buckling. An estimate for the 

buckling load was obtained before the finite element analysis was run, by using the average 

material properties of the composite and assuming isotropic constitutive behavior. After 

buckling, the compressive load was increased in increments of about 5% of the buckling load. 

The analysis was carried out until the compressive load reached the failure value, as determined 

by the experiment. 

RESULTS 

Figure 3a depicts contours of constant out-of-plane displacement w, obtained by the 

fiiite element aiialysis for the experimentally determined critical in-plane load. Clearly, the part 

of the panel between the supports buckles in a half-wave pattern in both directions, which is in 

agreement with the observed displacement pattern during the experiment. The maximum out-ofplane displacement occurs near the center of the structure and is computed to be 4.54 mm, which 

is about two times the thickness of the panel. To examine the spatial convergence of the 

developed finite element mesh, other meshes were also used. Figure 3b, represents the 

displacement pattern which was obtained for the same structure and boundary conditions but 

from a coarser mesh (120 elements, 575 dof). 

Figure 4a shows the pattern of the in-plane deformation of the structure, computed at the 

critical in-plane load. To make the pattern look clearer, the displacements in that graph are 

multiplied by a factor of 50. Similar results are shown in Figure 4b. These results were obtained 

from the coarse mesh discussed above. The in-plane displacements are smaller in the middle of 

the panel due to the large out-of-plane displacement in that area. , 

The relation between the total compressive end load and the corresponding average endshortening is shown in Figure 5. The conthiuous line represents numerical results obtained by 

the fier finite element model, while the broken line corresponds to results from the coarse mesh. 

The stars represent experimental results in which the end-shortening is measured by a dial5 
gauge, while the dots are experimental results where the inplane displacement is measured by the 

LVDT. Similar meaning is also given to the continuous, and broken lines and the stars on 

Figure 6. hi this figure the displacement axis represents values of the out-of-plane displacement 

measured during the experiment, in the middle point of the panel. From both of these two 

graphs, it is observed that the numerically obtained curves show the same qualitative behavior as 

the experimental curves. This behavior is typical for the postbuckling behavior of plates and was 

also observed in previous work on the subject [1,2,5,7]. Also, both the experimental and the 

analytical results indicate that the panel exhibits substantial postbuckling strength. According to 

the experimental results appearing in Figures 5 and 6, the failure load is estimated to be about 

three times the buckling load of the structure. 

Comparing the numerical with the experimental results, a considerable difference is 

observed. Some of that difference is expected and is probably due to the following reasons. 

First, the panel is modeled without taking into account geometrical imperfections. Also, the 

analytical boundary conditions do not match exactly the experimental support conditions, 

especially dong the simply-supported edges and at the edge were the load is applied. From 

Figure 4 one can see clearly that by applying uniform forces along the edge, the in-plane 

displacement v of the loaded end is not uniform. Another factor that can affect the results is the 

accuracy of the values of the material properties, dimensions and orientations of the laminae. 

For example, the measured thickness of the panel was found to be about 10% less than the value 

obtained by milltiplying the number of laminae of the composite tines the thickness of each 

lamina. Finally, some of the numerical problems encountered by using the finite element code 

are discussed next. 

By comparing the continuous with the broken lines of Figures 5 and 6, it is seen that the 

spatial convergence of the finite element mode is acceptable as far Bs the end-shortening and the 

out-of-plane displacement at the middle of the panel is concerned. Similar conclusions can be 

drawn by comparing Figures 3a and 4a with Figures 3b and 4b respectively. However, this is not 

the case when the contours of the resultant moments and forces are examined. Figure 7a depicts 

6 
contours of constant resultant shear force Qx, obtained by the fine mesh at the critical load, while 

Figure 7b shows similar results obtained from the coarse mesh. Clearly, the convergence of this 

resultant load (which involves third derivatives of the out-of-plane displacement with respect to 

the spatial coordinates) is not satisfactory. A similar behavior was observed for the other 

resultant forces and moments. This indicates the need for more study on the subject. Finer 

meshes should be tried and at least another finite element code should be employed for the same 

problem and the obtained results should be compared with the present ones before any 

confidence in the numerical results is established. It is of great importance to investigate if and 

how the spatial convergence of the solution is affected by the presence of the step in thickness, 

induced by the stiffener [ 161. Another area which needs further study is how the sudden stiffness 

reduction occurring at buckling, effects the convergence of the numerical solution. Clearly, the 

convergence of the resultant forces and moments is of vital importance since these loads are 

required in developing the proposed failure envelope for the structure. 

Finally, for the composite panel tested, the resulting failure was due to delamination near 

the points G and I rather than the expected panel/stiffener separation. During the test, the panel 

deformed in such a way that the area near the step in thickness was under compression, rather 

than tension. As can be deduced from Figure 6, the maximum out-of-plane displacement for 

compressive loads near the failure level was about three times the thickness of the panel. Tlis 

fact allowed the deformation pattern of the panel to be readily observable in the postbuckling 

regime. 

SUMMARY AND CONCLUSIONS 

A finite element model was developed for the postbuckling behavior of a stiffened 

graphite/epoxy rectangular plate loaded by in-plane compression. Both the unstiffened and the 

stiffened parts of the structure were modeled as anisotropic, plates and the NASTRAN computer 

code was used for the numerical calculations. Experimental data for the same structure were 

also obtained and compared with the numerical results. The discrepancy between the numerical 

and the experimental results needs to be investigated further. Effects due to the change in 

7 
thickness induced by the stiffener and the great reduction of stiffness at buckling on the 

convergence of the numerical solution have yet to be examined. Resultant forces and moments 

need to be computed accurately if a failure envelope is to be established for a composite 

structure. Finally, both the numerical and the experimental results show that the stiffened panel 

can exhibit a significant postbuckling strength. From the experimental data, the failure load was 

about three times higher than the buckling load, indicating how much the design of such 

structures can be improved, once their behavior is reasonably predictable. 

ACKNOWLEDGEMENTS 

This work was supported by NASA, under grant number NSG 1483. The fit author 

wishes to thank Professors C.D. Babcock and W.G. Knauss for the opportunity to work on this 

project and for many fruitful discussions. The help of Drs. J.F. Ha& G. Ravichandran and 

Mr. R. Madhaven is also gratefully acknowledged. 

REFERENCES 

1. 

2. 

3. 

4. 

5. 

6. 

7. 

8, 

Starnes, J.H., Knight, N.F. and Rouse, M., "Postbuckling Behavior of Selected Fiat 

Stiffened Graphite-Epoxy Panels Loaded in Coinpression," AIAA Journal, Vol. 23, 

Stevens, K.A. and Davies, G.A., "Failure of Buckled Composite Plates," Intern. 

Symposium on Composite Materials and Structures," pp. 345-350, Beijing, China, June 

1986. 

NO. 8, pp. 1236-1246, 1905. 

Agarwal, B.L., "Postbuckling Behavior of Composite Shear Webs," AIAA Journal, 

Agarwal, B.L., "A Model to Simulate Failure Due to Stiffenerrneb Separation of 

Composite Tension Field Panels," AIAA Paper No. 82-0746. 

Vol. 19, NO. 7, July 1981,~~. 933-939. 

Stein, M., "Postbuckling of Orthotropic Composite Plates Loaded in Compression," 

AIAA Journal, Vol. 21, No. 12, Dec. 1983, pp. 1729-1735. 

Stein, M., "Analytical Results for Postbuckling Behavior of Plates hi Compression and in 

Shear," NASA TM 85766, March 1984. 

Harris, G.Z., "Buckling and Postbuckling of Orthotropic Laminated Plates," AIAA Paper 

No. 75-813,16th Structures, Structural Dynamics and Materials Conference, Denver, 

CO, 1975. 

Turvey, G.J. and Wittrick, W.H. "The Large Deflection and Post-Buckling Behavior of 

Some Laminated Plates," Aeronautical Quarterly, Vol. 24, 1973, pp. 77-86. 

8 
9. 

10. 

11. 

12. 

13. 

14. 

15. 

16. 

Kuo, M.C. and Bogy, D.B., "Plane Solutions for the Displacement and TractionDisplacement Problems for Anisotropic Elastic Wedges," J. Applied Mechanics, March 

Ting, T.C.T. and Chou, S.C., "Edge Shgularities in Anisotropic Composites," Int. J. 

Solids Structures, Vol. 17, No. 11, pp. 1057-1068, 1981. 

1974, pp. 197-208. 

Pipes, R.B. and Pagano, N.J. "Interlaminar Stresses in Composite Laminates Under 

Uniform Axial Extension," J. Composite Materials, Vol. 4, 1970, pp. 538-550. 

Wang, S.S. and Choi, I., "Boundary-Layer Effects in Composite Laminates," J. Applied 

Mechanics, Vol. 49, Sept. 1982, pp. 541-5GO. 

Zwiers, R.I., Ting, T.C.T. and Spilker, R.L., "On the Logarithmic Singularity of FreeEdge Stress in Laminated Composites Under Unifoim Extension," J. Applied Mechanics, 

Vol. 49, Sept. 1982, pp. 561-569. 

Babcock, C.D. and Knauss, W.G., "Effect of Stress Concentration in Composite 

Structures," SM Report 84-17, Caltech, Pasadena, CA, 1984. 

McCormick, W .C., (ed.), "MSC/NASTRAN User's Manual," MacNed-Schwendler 

Corp., Los Angeles, CA. 

Tong, P. and Pian, H.H., "On the Convergence of the Finite Element Method for 

Problems with Singularity," Int. J. Solids Structures, 1973, Vol. 9, pp. 313-321. 

9 
I 

In. 80 mm 

1 

- 

I 

0 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

1 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

G 

T 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

I 

(AB 1 5.08 mm 

(AC) = 25.40mm 

(AD) =146.05mm 

( AE 1 = 152.40 mm 

AB C DE 

- x. u 

~ 

Figure 1. Specimen Geometry 
1.600E-0 

1.400E-0 

1.200E-0 

1.000E-0 

e. 000~-0 

6.000E-0 

4.000E-0 

2.000E-0 

0.080E+0 

7 

C 

C 

C 

C 

C 

i 

m C I I W IJ m c m c m C 

(u t 

Figure 2. 

w w w w w 

B m m m m 63 m m 6) m 63 m m N P 

Finite Element Mesh 

4-1 

I 

W 

m 

m 
MIN(-)=-4.54E-03 

MFIX(+)= 3.96E-04 

CONTOUR LEVELS 

FI=-4.31E-03 

B=-4.09E-03 

C=-3.87E-03 

D=-3.64E-03 

E=-3.42E-83 

F=-3.19E-03 

G=-2.97E-83 

H=-2.74E-03 

I=-2.52E-03 

53-2.38E-83 

K=-2.87E-83 

L=-1.85E-03 

M=-1.62E-03 

N=-1.40E-03 

03-1.17E-03 

P=-9.49E-04 

Q=-7.25E-04 

R=-5.01E-04 

S=-2.77E-04 

T=-5.23E-05 

U= 1.72E-04 

~ - _I-- - 

Figure 3a. Contours of constant out-of-plane displacement at the critical load (Fine Mesh). 
I 

MIN(-)=-4.55E-03 

MQX(+)= 3.27E-04 

CONTOUR LEVELS 

Q=-4.32E-03 

B=-4.18E-03 

C=-3.88E-03 

D=-3.66E-03 

E=-3.44E-03 

F=-3.22E-03 

G=-2.99E-03 

H=-2.77E-03 

I=-2.55E-03 

J=-2.33E-03 

K=-2.11E-03 

L=-1.89E-03 

M=-1.67E-03 

N=-1.44E-03 

0=-1.22E-03 

P=-1.00E-03 

Q=-7.80E-04 

R=-5.58E-04 

S=-3.37E-04 

T=-1.15E-04 

U= 1.06E-04 

Figure 3b. Contours of constant out-of-plane displacement at the critical load (Coarse Mesh). 
-~ ~ ~~ 

Figure 4a. In-plane Deformation (Fine Mesh). 
Figure 4b. In-plane Deformation (Coarse Mesh). 
0 0.5 I 1.5 

END- SHORTENING, v [mm] 

Figure 5. In-plane End Load vs. End-shortening. 
* lo4 

1 

E 

n 

a 

. 

z 

s 

w 

> 

v) 

v) 

w 

a 

a 

z 

0 

u 

- 

- 

- 

- 

- 

0 2 4 6 0 

OUT-OF- PLANE DISPLACEMENT, w * 10-3 [mm] 

Figure 6. In-plane End Load vs. Out-of-plane Displacement in the middle of the panel. 
I 

MIN(-)=-1.55E+04 

MFIX(+)= 4.95E+04 

CONTOUR LEVELS 

FI=-1.25E+04 

B=-9.59€+03 

C=-6.64E+03 

D=-3.68E+03 

E=-7.27E+02 

F= 2.23E+03 

G= 5.18E+03 

H= 8.14E+03 

I= 1.11E+04 

J= 1.40€+04 

K= 1.70E+04 

L= 2.006+04 

M= 2.29E+04 

N= 2.59E+04 

O= 2.88€+04 

P= 3.18E+04 

Q= 3.47E+04 

R= 3.77E+84 

S= 4.86E+04 

T= 4.36E+04 

U= 4.65E+04 

_____ .~ - ~- 

Figure 7a. Contours of constant Shear Force Qx (Fine Mesh). 
8 

L= 1.17E+04 

M= 1.43E+84 

N= 1.69E+84 

MIN(-)=-1.99E+04 

MFIX(+)= 3.88E+04 

CONTOUR LEVELS 

1 

Fl=-1.?3€+84 

B=-1.46€+04 

C=-1.28€+84 

D=-9.37€+83 

E=-6.?4E+83 

F =-4.11E+83 

G=-1.48E+03 

H= 1.16E+83 

I= 3.79E+83 

J= 6.42E+03 

K= 9.05E+03 

Q= 2.48E+04 

R= 2.7SE+84 

S= 3.81E+84 

T= 3.2?E+04 

U= 3.54E+04 

~ 

Figure 7b. Contours of constmyshear Force Qx (Coarse Mesh).