Using solid laminate elements
Using solid laminate elements
(OP)
Hello!
I'm trying to model a composite using the built-in solid laminate element type which requires me to specify a lay-up. However, it seems that none of my materials seems to be appropriate. I constantly get the message "invalid material type" when I try to select them in my lay-up editor. I'm running FEMAP 11.0.1 and solving with Nastran. From the help-file I get the impression that I should be able to do this but there seems to be no advice on how to do it. It works fine when I use shell elements, but I'd like to obtain the interlaminar shear stresses for which solid elements seems better suited. Does anybody know how to do this?
Cheers
I'm trying to model a composite using the built-in solid laminate element type which requires me to specify a lay-up. However, it seems that none of my materials seems to be appropriate. I constantly get the message "invalid material type" when I try to select them in my lay-up editor. I'm running FEMAP 11.0.1 and solving with Nastran. From the help-file I get the impression that I should be able to do this but there seems to be no advice on how to do it. It works fine when I use shell elements, but I'd like to obtain the interlaminar shear stresses for which solid elements seems better suited. Does anybody know how to do this?
Cheers





RE: Using solid laminate elements
Use the 2D orthotropic material to create layups for shell elements.
RE: Using solid laminate elements
RE: Using solid laminate elements
Just ignore the message in the Femap message window. As long as you use the isotropic or 3D anisotropic material, then the data will be correctly translated to Nastran.
Sorry for the bad message, will see that it gets corrected.
RE: Using solid laminate elements
RE: Using solid laminate elements
RE: Using solid laminate elements
RE: Using solid laminate elements
RE: Using solid laminate elements
The only error I see when a run is submitted to NX Nastran is singularity fatal message due to the mesh not being connected. I notice your model is setup for MSC Nastran, if you are getting a different error message from MSC Nastran, then it might be helpful to post the actual error message from the f06 file.
A couple of other things to be aware of with solid laminates. If your layup total thickness is different than the actual dimension of the solid element, then Nastran will "scale" all of the layer thicknesses so the total matches the solid element dimension. You should try to make sure these thicknesses match up so the scaling does not have any significant impact on your results.
RE: Using solid laminate elements
Perhaps you can answer another question that has come up? I have the impression that in order to solve this in Nastran I need to run it in a non-linear solver, such as SOL400 or SOL600, is this true?
RE: Using solid laminate elements
You also need to make sure the coordinate system is set up properly. In addition to specifying the material coordinate system, you must define or tell nastran which axis of the system you pick is the material x direction and which is the stack direction. In the Femap solid laminate property form, make sure the ply/stack direction is also set correctly so your material properties are oriented correctly.
For NX Nastran, solid laminates are allowed in sol 101,103 so nonlinear solution is not required. You can also use contact in the linear solution.
Also, just to followup on your original question about the error message, the error message is from the Femap routine that calculates equivalent laminate properties on the fly for the user. It does not handle 3D materials currently. If you have the entity info pane open, then Femap is trying to update the current equivalent property every time you select a new ply, and so it gives an error message each time you select a 3D material for a ply. This has no impact on the solution, since Nastran handles all of the calculations internally for the actual solution.
RE: Using solid laminate elements
RE: Using solid laminate elements
RE: Using solid laminate elements
RE: Using solid laminate elements
For the PCOMPS see the note below concerning material/ply orientation. This is from the QRG. I would suggest when switching between Nastran's, read the the documentation carefully for features like this. The material cord system you select is projected to the element
Ply orientation and stack direction will be determined from the material
coordinate system (CORDM). The ply orientation direction will be at an angle
relative to the local X-direction of the ply. The local X-direction is the projection
of the n-direction of the CORDM onto the ply, where n is the first number in the
PSDIR field. The stack direction corresponds to the m-direction of the CORDM,
where m is the second number in the PSDIR field.