Using solid laminate elements

[timtimtim44]

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

 

[jbrackin]

Using a solid laminate element requires the use of either an isotropic material, or a 3D anisotropic material to create the layup. I suspect you created a 2D orthotropic material?
Use the 2D orthotropic material to create layups for shell elements.

 

[timtimtim44]

I've tried both 3D orthotropic and anisotropic material. FEMAP says that both are invalid material types when I try to incorporate them in the lay-up editor...

 

[jbrackin]

I see the message you are referring to now.
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.

 

[timtimtim44]

Cheers for that, but I have encountered additional trouble now. When I ignore it things seem to be working until I try to export the analysis file. Then I get the error message that "Laminate Solid Property 4 is not supported". In the .dat file created there is no property card created which references the material either. I have meshed it using hexmesh (Chexa-elements). Do you know what I might be doing wrong?

 

[jbrackin]

Can you post the model? Do you have extra materials layups and properties that are not being used by the mesh?

 

[timtimtim44]

Thank you, I'll post it when I return to work tomorrow morning. Been thinking about my model as I walked home, there's no unused lay-ups or properties as far as I know but I'll double-check that. However there is two holes in it. One of which I use for constraining it (pinned constraint simulating a bolt) and some of the elements around it were meshed as CPENTA instead... I'm wondering if this is the problem, I'll see if I can get rid of them tomorrow. But this shouldn't have prevented FEMAP to assign the correct property to the other elements or?

 

[timtimtim44]

Ok, I worked my way around the CPENTA elements but the result is still the same. I have uploaded my model as a femap neutral file, if you have time to look at it I would greatly appreciate it. I hope it's rather self-explanatory... I've only modeled a segment, I intend to put circular symmetry on it as soon as I get the laminate property sorted.

 

[jbrackin]

It looks like the real problem with your model is the mesh. You have many "cracks" where the mesh is not congruent. A coincident node check and merge will correct some of them, however there are areas where your geometry needs more preparation to make the mesh congruent. You can use View/Select free edge plot to see the many cracks.
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.

 

[timtimtim44]

Well I haven't been able to get as far as an error message from Nastran yet, but I will post it if I get one. I'll keep working on the mesh. I'm not sure that I follow you on the element dimensions, are you saying that nastran writes one entire lay-up to each element, i.e. should I mesh it so that my elements are as thick as the lay-up?

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?

 

[jbrackin]

For solid laminates, the layup you create is assigned to an element via the property that you reference. So you need to make sure that the layup definition is for a single element thru its thickness. If you mesh the part with one element thru the thickness, then your layup should be the total thickness. If you have 2 elements thru the thickness, then the layup you create is for 1/2 the thickness and you need to make sure you get the stacking in order for the 2 layers of 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.

 

[timtimtim44]

Righto, that was a good explanation on the elements. Is there a problem that currently I only have access to two types of solvers? I can solve it using either MSC Nastran and/or Abaqus... will any of them work?

 

[jbrackin]

I know MSC Nastran has solid laminate, not familiar with Abaqus, but would expect it has the capability. I would consult documentation to understand details of their implementations. There could be some differences in assumptions and details. If you still get error messages, then request support from MSC or Abaqus. You coulkd also post any detail error messages to get some help here.

 

[timtimtim44]

I managed to get a hold of an NX solver, so hopefully as soon I get the installation sorted I should be able to run my simulation. I noticed that when I export my model as an NX .dat-file it uses PCOMPS elements. Does anybody now if there is a way to get the ply's to orient themselves according to the element coordinate system as I can do with PCOMPLS elements? My model has the shape of a cone with upper and lower flanges and at the moment my materials are pointing in all kinds of directions.

 

[jbrackin]

The different Nastran's implement features in different ways, but mostly end up with the same capability.
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.