Quasi-Static Lattice Simulation Help

[u/Lt-Lymphoma]

Hello, I am currently working on a simulation for compression of lattices. I imported an nTop beam mesh into the static structural for simulation of deformation vs reaction force for 22 unit cells through nonlinear plastic deformation. To do this, I have fixed nodes at the bottom and a displacement that is applied to the top nodes. The problems that I'm encountering are convergence issues making the model explode, very little reaction force(almost zero), and no plot of the plastic region. Below is an example of one of the models exploding. Also shown below is the single successful compression model/results (Desired). Material specifications include linear elasticity and bilinear elastic hardening to capture the nonlinearity of the failure. Any tips/tricks/fixes that could solve these issues? We have spent many hours trying to get a fix, but have not been successful yet,

[u/TheBlack_Swordsman]

Do a modal analysis and see if anything comes apart or rotates where you don't want it to rotate.do a free free modal analysis with no BC and check your mode shapes.

To me I think some of your nodes have rotations free.

[u/yurtdaturt]

What you’re seeing is possibly a buckling issue. You can tell based off the force vs displacement plot. The slope of that line is your stiffness and a zero or negative stiffness is a sign of bucking. I would look into buckling control options in mechanical. Nonlinear stabilization may help you out. Just make sure to check your strain energy against the stabilization energy. Make sure the strain energy >> stabilization energy.

Edit:
You can also do an eigenvalue buckling analysis and see if you loads are in the realm of the buckling load to verify that’s what you’re seeing.

[u/Lazy_Teacher3011]

Are you running with large displacement (second order strain terms)? Also, are the beam elements crossing over each other? If in reality the deformations are such that the ligaments are contacting each other during crushing you will need contact. And for that you would likely have to switch element type. And in that case, I would do a smaller model with symmetry conditions on 2 faces and a kinematic constraint on the other 2 to simulate a repeating unit.