I am analyzing the scoliosis correction, you can check the model and results -here-.
You see two rigid braces compressing the body while doing that it tries to straighten the spine in the middle. I am able to get some results on this model when Nlgeom is off with small mesh distortions. Now I would like to enable Nlgeom and see how it differs but I got errors. I am guessing some mesh elements get inverted results in negative jacobian. So I would like to ask,
Is the mesh looking ok, fine enough, and or is there better mesh for contacts? In my early attempts, I saw that the contact between the body and spine was ill, and didn’t fit each other, so with an external program I took a boolean difference of body with the spine model and volume meshed them both and imported as .inp. The new mesh was 99% fitting. Should I consider the same approach for between braces and body models as well?
Should I try the other solver types than the default one(PaStiX)? I usually tried Pardiso in other FEA solvers, but in PrePoMax I only used Pastix and it gave me convergence all the time.
I understand the difference between tie constraint and tied contact. I think in articles people chose the tie constraint but I would like to try tie contact as well. Does this make a difference in getting convergence?
I heard about only compression boundary condition. Does this work in my model?
What is a Slip wear model? Should I consider it? Because in there I saw there is a kind of mesh update. With it maybe I can get rid of elements invertments or is this only my imagination?
Where I can read more about Calculix Nlgeom? I only found the Calculix User manual and it includes many things but Nlgeom :(. Is there a theory manual somewhere?
Aside from my questions what things should I consider further? I appreciate any help, thank you.
PaStiX is good enough in most cases but it may still cause some issues and struggle with very large meshes. Then Pardiso is usually the best choice.
Tied contact requires more computational resources, tie constraint is more reliable and versatile and sufficient in most cases (unless the contact pressure has to be evaluated, for instance).
It can be used instead of contact with a rigid surface of the same shape as the deformable surface. It uses GAP elements internally and requires NLGEOM to work properly. There’s also the surface spring constraint which acts like elastic foundation (in both directions).
It’s used for wear analyses using Archard’s model to compute the wear depth. So it’s quite specific and not just a general adaptive mesh refinement.
What do you want to know about it ? The theory manual for CalculiX is the book " The Finite Element Method for Three‐Dimensional Thermomechanical Applications" by G. Dhondt (CalculiX developer) but it’s just about the finite element method theory with little practical aspects.
In short words, when Nlgeom is enabled, geometrical nonlinearity is accounted for - stiffness changes due to deformation can be modeled along with effects like nonlinear buckling and preload. It’s meant for large displacements/rotations and strains.
Yes, but in that area I fixed their all degrees of freedom. Even though it’s very poor I am thinking it doesn’t affect the results. I could be wrong what do you think?
Yes. In my initial versions, I didn’t want to include real material properties so I set their young modulus to 1 and the braces are completely rigid. For the contact, I choose Linear 5.
I chose the master surface as the body and the slave as the one penetrating the braces right?
For your other answer thank you! I will focus on the ill mesh areas and also what focusing else could give me better results?
In the case of such complex models, it’s best to simplify them gradually (remove the features one by one) and check what happens. Non-convergence is usually due to contact but mesh density and quality are also very important.
