Dear Siemens PLM Community,
I am trying to simulate the compression of gyroid lattice in FEMAP, but I am getting some troubles.
The model consists in a cylindrical gyroid that is “gripped” by two RBE2s. They both are fixed, while the top one has an imposed displacement.
The mesh is generated in Matlab, then it is modified from linear plot to plate.
The quality of the mesh is not optimal, I report below the default FEMAP mesh quality check:
The displacement is <10% of the total height and is applied at 1 mm/min, hence I tried with a nonlinear analysis (SOL106). The material is defined as Nonlinear Elastic (with a …vs stress curve).
The problem arises during the simulation… The Nastran error is the following:
I used the default FEMAP settings for the analysis, then I tried with the below settings but the error still occurred.
Somebody knows if there are “better” settings? Or it is better to use an advance nonlinear?
It may be a problem of mesh quality? I have also tried to use a mesh with more nodes, however the analysis does not converge.
Thank you in advance.
Mesh quality is very poor. Usually Nastran refuse to solve model with Jacobian greater than 0.9 but in your case Jacobian is 0.97. Internal angle of 87.7 deg indicate that this quad element almost collapsed to triangle.
You can read in Femap help about mesh quality metric.
Thank you for your answer Karachun, however I forgot to specify that I am using triangular elements.
I report the Nastran quality check:
Anyway, I am conscious of the poor mesh quality. I tried to remesh, but I had no success due to the complex geometry. Do you have any suggestion?
You can generate surfaces for meshing using the command, Geometry, Surface, From Mesh. Do not try to create a single surface for the entire model, but instead create several small surfaces and then rotate and/or copy to create the entire model.
Dear Chip Fricke,
thanks to your suggestion, I was able to generate a new tri mesh. Now FEMAP and Nastran quality checks give, respectively:
However, I performed the same analysis as above and I got a new error:
Do you know which can be the reason of the error and how to solve it? Increasing the number of elements might be a solution?
Actually, the analysis with the new mesh diverges when it is almost finished (I mean in terms of prescribed displacement). The intermediate outputs could be fine for me. However, may I consider them "correct"? May I discard some outputs before the convergence error?
Thank you in advance.
Here is some suggestions:
1) set load to 50-80%, calculate model and check maybe load is too high and mesh become too distorted due to deformations;
2) set Max Iterations/Steps to 10-25;
3) increase timestep number;
4) reduce convergence tolerance by one order of magnitude;
5) enable Arc-Length method or Modified Newton-Raphson;
6) enable midside nodes in mesh (Modify->Update Elements->Linear/Parabolic Order or Midside Nodes);
Intermediate output can be requested by option Intermediate 3..All or 1..Yes.
In addition, you can find some useful information in documentation: