Nastran separation contact type (friction contact) results in asymmetric deformation for symmetric loads

[louroumova]

Hello all,

Our company is looking into using Nastran non-linear static analysis to model the loading on structural elements during transport. The non-linearity originates from the fact that the primary body is made of hard steel material, and it comes into contact with the soft material of the supports. For that purpose, a simplified version of the general models is developed in Inventor, and Nastran FEA applied to it. The same CAD geometry is used to set up an equivalent FEA using Ansys and the results are compared. For both cases the primary body modeled as a shell element while the supports are modelled as solids; the gap between them is of variable size (from 0 to 11mm) as the shell is cylindrical and the support is tangent to it. The idea is for the shell to rest on the supports given some gravity loading, so in subcase 1 a displacement of the shell towards the supports is applied to achieve initial contact and then is subcase 2 the gravity is ramped up. 

The issue is that the Nastran simulation results in asymmetric deformation given symmetric displacement and gravity loading conditions when separation contacts are used. To verify the set up in Nastran first analyses with ‘Bonded’ contacts are developed and it is observed that the two software produce almost the same stresses and deformation for this linear analysis given any gravity load. Then, the contact type is set to ‘Separation’ with:

• Friction coefficient of 0.1
• ‘Unsymmetric contact’ type where the master entity is the steel shell, and the slave entity is the soft support.
• Elements orientation is also correctly set to top/bottom for the shell element.

Ansys produces the expected symmetric deformation for that case as well. While the Nastran model does not converge with the default setting for the contact data. Hence, the ‘Penetration offset’ and the ‘Activation distance’ are adjusted so that simulation converges. Models with various combinations of those values have been simulated and convergence is achieved but all the resulting deformations have some degree of asymmetricity which is above the acceptable levels. Moreover, mesh refinement of different degrees has been implemented but the issue still stands. The following reasoning is applied when the input settings are varied:

• The ‘Penetration offset’ is set to 0.5mm as the support is initially tangent to the primary body. Values from 0.25mm to 1mm have been attempted but results in greater/same asymmetricity.
• The ‘Activation distance’ is set to 1.1*(mesh size of master surface) for the various mesh sizes attempted. Greater and smaller values are also tried but no improvement.
• The ratio of the mesh sizes at the contact is varied from 1 to 1.5 where the primary body that is the shell modeled with quad elements has the greater mesh size.  A ratio about 1 to 1.3 seems to fit best.  
• The smallest mesh size of the shell element that is successfully modeled is 27mm where the thickness of the shell is 25mm. Smaller mesh size somehow results in a shell with two top skins (or two bottom).  

We have run out of troubleshooting options to implement. Are there any further model improvements which you could suggest? Would you know the reason for these asymmetric deformations? The way it stands now, Nastran is unable to handle separation with large deformation where bodies are coming in and out of contact unlike Ansys. The model which results in the most symmetric results is included in this message. The Inventor Nastran version is 2021.0.0.401. Thank you for your help in advance!

-Lora 

[delaroca]

Hi @louroumova ,

I took a look at your model and made some changes that I think will be beneficial. I mostly simplified it with two symmetries (X and Z directions), making it 1/4 of the original model. This should increase the precision (element count-wise) and solve for the 'asymmetric' results.

For the loads, I simplified the simulation (unfortunately I didn't have much time to tweak this model, I'm at work now), but you can modify it back, refine the mesh, add your subcases, change the material, and I think it should work. I tried with a displacement of 40 mm, with 20 nonlinear steps converging at displacement and work, and it ran to completion, here is the shell equivalent stress view:

Attached is the model with the simplifications I made. I hope it helps.

*I used inventor and inventor nastran version 2023

[louroumova]

Hey @delaroca,

First of all thank you very much for your reply and input!

Indeed this would help resolving the asymmetricity and will give higher fidelity results. I have also tried restricting the motion in x-direction and then stresses and deformation compare well with Ansys.

However, what we are looking into is verifying the Nastran settings (or rules for the settings) with Ansys are reusing them later. Therefore, I'm performing this simulation as part of a Nastran feasibility study where the end goal was to model a commercial case with 3 times bigger cylinder of variable thickness with 20+ pad supports instead of 4 to which 3D linear and rotational acceleration loads are applied. That is the reason I have refrained from modeling only part of the set up; in the end I will not have any planes of symmetry.   Nastran does not seem to be reliable enough for such use if there is random asymmetricity in deformations for a symmetric load. Moreover, as the commercial cases are way bigger,  the number of elements needed for them is 3 to 4 times greater which makes the software prone to crashing or it slows down the interface which makes it not so user friendly (of course this is computer specific issue but I'm using quite the standard work desktop). 

The way it seems now, Nastran is not capable of handling such levels of complexity for Non-linear analyses which makes it not suitable for our needs.  I'm still looking for hard confirmation if that is indeed the case.

[John_Holtz]

Hi Lora,

Just to be clear, I assume you are taking about this type of result:

Figure 1: Deformed shape shown greatly exaggerated (original setup)

It is interesting that the results (stress, displacement, etc.) are symmetric, but the line of symmetry has rotated. I do not know why that happens, unless the problem is relying on friction to prevent it from rotating is the problem. Mathematically, the pipe can rotate any angle and still have the same result and same forces from friction because they all satisfy a static condition.

I prefer using more deterministic methods to provide stability than friction. Instead of friction, I added some weak springs to the model and applied the gravity load only. The analysis would get to 50% to 60% completion, and then the stress in the support pads would go to zero. This implied that the pipe was penetrating too far into the pads which caused the contact to failed. I then increased the contact stiffness from 1.0 to 10. This is the result that I got:

Figure 2: Result with no friction, higher contact stiffness, and springs for X & Z stability.

All the results are symmetric (about both plans of symmetry) without showing any rigid body rotation of the pipe.

Let us know if you have any questions.

John