Hello Simcenter community,
I'm running some simulations with SOL601,106 in NX Nastran 11. I modeled contact between parts with fine mesh in order to respect Hertz contact theory and get accurate contact normal and shear stress. In one simulation, some elements are deactivated because material failure seems to be reached. But I do not want this to happen. To prevent this I chose:
- XTCURVE : "Extended" in NX11 strategy parameters ;
- And I draw a tri-linear curve with strain extending until 0.99 mm/mm with a plateau in order to ensure that element won't disappear.
Despite this I always get some elements deactivation in my analysis and i do not understand why. Do you have ideas ?
I'm not sure it is possible.. But I can build my own model with the same materials and typology and will be able to share it there. I'll do that as soon as possible. Thanks.
Edit : I changed what was needed to share the model. Thanks a lot. Any other suggestion on the model is welcome.
What strain do you expect? - I'm not sure but if you expect nonlinear strains with values of 99% as you mentioned before, I think you have to activate nonlinear displacements and strains in solution parameters, right?
- Sometimes activating U/P-formulation yields better results, too.
- Adina has additional elements with more grid points in element face and volume to improve stablity.
Your contact element desity is really different in size for source and target and as I believe the smaller elements are in the target region, but that is not so good, I'm sure.
Nevertheless there are a lot of penetrations with that mesh and after ignoring it there are large forces to get lost of the penetrations and your circular faces are not circular after that.
I could not solve it, did you? - Maybe you could plot your last displacements, stress and strain pictures.
Best wishes, Michael
Actually, i o not expect such strains. I just added 0.99 to be sure that the element won't be deactivated. But such strains should not occur.
- Ok thanks
- Ok thanks
You're right concerning this density. However, i wanted to model tied contact at this location because it is not the interesting part. I did not know that tied contact could be so dependant on mesh size. I did this to reduce model size. I tried to use GLUING but calculation was far too long... But it seems that the tied contact is not really good in this case.
The interesting part is the non tied contact between cylinder and other parts. There, meshes are really close. I could solve until 50% of load and there is already large strain. I think the part is not resistant enough because i have another case with different materiels and everything went well. Here is a picture of deformed shape.
It turns out that, in addition to the last point on the stress-strain curve being used as a rupture criteria when XTCURVE=0, there is an internally coded criteria that an element will be considered ruptured whenever strain exceeds 100.0
In this model, there seem to be a few spurious contact results causing this. In the one area I investigated, there is line contact between a cylinder and a flat face. In increments <= 26, the strains in the region of contact are all on the order of 0.011:
At increment 27, the strains for this single element jump to 200-600:
The surrounding elements all remain at ~0.011:
In the next increment (28), element 1270688 is removed and the surrounding strains remain at ~0.011:
I believe that this could be related to your disabling of contact updates (via DISP=1 on BCTPARA and CTDISP=1 on NXSTRAT). You may also need to add a small amount of compliance to the contact (set CFACTOR1 in the range of 1.0e-6 to 1.0e-8 on NXSTRAT)
The high strain may be triggered by the use of incompatible modes with plasticity and the relatively high aspect ratio of the elements. This may cause spurious modes as described in the article below
You could try using the u/p formulation (UPFORM=1 on NXSTRAT) to see if that resolves the high strain.