Cancel
Showing results for 
Search instead for 
Did you mean: 

Orthotropic material with plastic properties in Femap w/ NEi Nastran

Experimenter
Experimenter

Hello all,

I am trying to use a model (3D solids) with a 3D orthotropic material and nonlinear material properties (plasticity). I am simply defining the material as bi-linearly plastic, but it seem as if NEi Nastran does not recognize the plasticity introduced and considers the material elastic. I have tried running the model using a linear orthotropic material, as well as with a nonlinear isotropic material, both of which have behaved just fine.

Does anyone have any idea as to what might cause this?

Regards,
Niklas

3 REPLIES

Re: Orthotropic material with plastic properties in Femap w/ NEi Nastran

Experimenter
Experimenter

Hello Niklas,

 

As I understand it, plasticity is not supported in 3D orthotropic materials, so that would explain the issues you are encountering.  Can you tell me a little bit more about your application?  I wonder if there may be a different approach we can use.

 

Mitch

Re: Orthotropic material with plastic properties in Femap w/ NEi Nastran

Experimenter
Experimenter

Hello,

 

I am trying to model pretension between two rotationally symmetrical pieces by applying a temperature increase and enabling thermal expansion in the r- and t-direction, but not in the z-direction, hence my need for the orthotropic material. After the pretension is applied I want to run a nonlinear plastic analysis with the mechanical loads.

 

Niklas

Re: Orthotropic material with plastic properties in Femap w/ NEi Nastran

Experimenter
Experimenter

Thanks Niklas,

 

Do you need the orthotropic material for the second phase of the analysis, or is it just for the thermal stress case?  In NEi/Autodesk Nastran you can run the two cases separately and transfer the strains from one to the other, which would allow you to use an isotropic material with plasticity for the second phase.

 

During the first run you would need to turn on TRSLSTRNDATA (under Output Control Directives).  This will create a BDF file with the strain information.  Then in the second phase you would need to add INITSTRAIN=100 (default, you can open the BDF file that was created to confirm.) to the case control which is right before begin bulk.  After begin bulk, you will need to include the data from the previous run using INCLUDE 'filename.bdf'

 

Another option for the interference fit is to use the contact to create the interference.  If you edit the connection property in Femap, you will see Penetration Surface Offset.  You can enter a value in length units and it will create the interference.

 

I hope this helps.

 

Mitch