Composite analysis doubt in Nastran card. 1

[pcomp]

I am studying carbon fiber laminate for structural loads thro FEA. I use hypermesh/optistruct (same as Nastran keyword format) to analyze the FE models. My model contains 64 lamina with repeating material directions. (The laminate has 8 quasi-isotropic lamina assemblies. Each quasi-isotropic lamina assembly has 8 layers/lamina with material angle in 0, 45, 90,-45, -45, 90, 45, 0 as the stacking sequence) I use Pcomp and Mat8 combination. My material has failure strain values to capture the failure index based on maximum strain theory.

As the post processing becomes laborious with 64 laminas, I tried to use SMEAR property in PCOMP card. I used COMPRO program to generate the material property for quasi isotropic laminate based on 8 layers with above mentioned stacking sequence. Then I reduced the number of layers in my FE model, from 64 to 8 and I referenced smeared material property for each layer.

Now my doubt is
1) Should I turn on smear field in Pcomp card? Or does not matter?

2) What angle I should use for each layer? Does the angle matter in this situation as the E1=E2 in the smeared property?

3) My biggest doubt is interlaminar shear stress (SB) in PCOMP card. When I did my first analysis (with individual 64 layer), I used the shear strength of epoxy resin for SB value. (However I did not model separate bonding layer between carbon fiber layers, as bonding layers are very thin, may be 0.001 inch due to our high pressure compaction. Also, if I model bond layer it will become 128 layers, instead of 64 layers.). When I used the same SB value in second analysis (8 layers with smeared material properties), the results are completely different with first analysis particularly bond failure index. It is so higher than the first analysis. I do not know how to fix this. Gurus, help me to fix this and how to perform smeared analysis.

Thank you.

 

[SWComposites]

1) No, you do not need to use the SMEAR parameter as you have already done that with your input

2) 0 degrees; the angle matters because the smeared properties may not be isotropic, which is not just E1 = E2

3) Not sure exactly why the interlaminar shear streses are different, but it could have to do with the element formulaton. You should run a simple test model (cantilever or 3-point loaded beam) where you can calculate the results by hand. Run it with both of your material inputs and with a single layer using your calculated sheared properties, and plot the interlaminar shear stress (not the failure indicies) versus position thru the thickness. If you can't figure out what is going on with these test models, post the details of your test models and the interlaminar shear stress results here.

 

[pcomp]

Swcomposites,

Further on this topic, I doubt my failure strain values used in quasi isotropic laminate. These values are important in determination of failure indeses based on max.strain failure theory. We know the XT,YT, Xc,YC and Sxy of a single lamina. The compro program does not report smeared values of failure strains at laminate level. It only reports E1, E2, G12, nu12. Can we calculate failure strain of quasi-lamainate without physical test, through indivudual ply strain value?

 

[SWComposites]

You can calculate the quasi-isotropic laminate failure strain using the maximum strain failure theory and your ply data. Essentially the max strain theory says that the laminate failure strain is equal to the ply failure strain. However, the predictions will most likely not match laminate test data. For reason, most aerospace companies use laminate level test data (rather than ply level data) to establish strength values.

For the results of an extensive evaluation of failure theories, see this paper:

M. J. Hinton, et. al., “A Comparison of the Predictive Capabilities of Current Failure Theories for Composite Laminates, Judged Against Experimental Evidence”, Composites Science and Technology, Vol. 62, 2002, pp 1725-1797.

along with many of the references listed therein.

Steve