Hyperelastic net under gravitational load

[MOZER8]

Hello Everyone,

I have modelled a net with following parameters:

Net elements: Truss(T3D2) - hyperleastic
Frame: Beam(B31) - linear elastic
BC: constraint: DispXYZ=0 at two side of the frames
load: 1G gravity which is normal to net
Step: General static, nlgeom=on

It is a pretty straight forward analysis. I want to analyze hyperelastic net under gravitational load. However it doesn't converge (due to numerical singularities). Could you please check attached inp file and advice me? It is a very small model, it shouldn't take more than 1 minutes to solve. Thanks in advance.

 

[Erik Panos Kostson]

OK, without looking at it. Since you have subdivided the trusses we have a link mechanism between each one of them so that will not solve. Typically one will have some pretension in the trusses before adding an out of plane loads, because if they do not have tension they cannot take the out of plane load (this is what is called a geometric non-linearity or tension stiffening terms). So in your first step (before gravity comes on) just add in plane disp. in the opposite direction at the BC and stretch the net a bit. (In short they/trusses need a pre tension)

 

[FEA way]

I checked this model in Abaqus and I agree that this is because of the lack of pretension. You can add Predefined Field to the Initial step, select Stress type and enter some small value for Sigma11.

 

[MOZER8]

Thank you for the suggestion. The thing is, two different material is used in this net assembly. Inner net is hyperelastic material with very small stiffness. On the other hand, frame is made of steel (relatively high stiffness). Thus if I apply large displacement, experience high stress values on the frame. If I apply small displacement values, analysis aborts with same error. Could you suggest me a method for applying axial loading to hyperelastic material, without affecting steel frame?

 

[FEA way]

I ran it with a small initial stress of 5 MPa applied as described above to the set consisting of truss elements only and the analysis worked without any problems.

Just add for example:

*Initial Conditions, type=STRESS
Set_name, 5, 0, 0

 

[Erik Panos Kostson]

I can confirm also that it solves without any problems (eventhough I had to use less elements- have a node limited version).

 

[MOZER8]

Pretension for initial conditions solved my problem. Thank you for your help.

 

[MOZER8]

FEA way, Erik,

Thank you very much for the support again. I have completed the first analysis with your support.

Now I need to inport these analysis results into an explicit dynamic analysis as a initial contidions. So I select initial state from predefined field menu. This gave me the following inputs:

*Instance, library=21_Truss_Hyperelastic_loose-gravity, instance=Net-1
*Import, state=yes, update=no
*End Instance


When I started the explicit analysis, nothing happens. It doesn't start to solve(no change in CPU and RAM) and it doesn't give any error. Is there any trick is needed to be consider?

Thanks in advance.

 

[FEA way]

Do you run this from CAE or command line ? This sounds like a temporary error or license loss. Restart your PC and try again, also make sure that different analyses can be run.

 

[MOZER8]

First, I was running it from CAE. After I switched to command lin, it realized it can't find .res file from previous analysis. It seems I forgot to turn the restart on. It is running without a problem now. Thank you for your support again.

For others who check this topic later. Frequency was changed from 0 to 1 as it is shown below. It writes a .res file for restart operations. In CAE, it can be changed from module:step Output/Restart request.

*restart, write, frequency=1