Does anyone know of solutions around stiffness singularities? Why they exactly occur? How to help optimize the study settings or options to help converge the result?
Does anyone know of solutions around stiffness singularities? Why they exactly occur? How to help optimize the study settings or options to help converge the result?
I physically understand your recommendation and would like to try it. But where in the options can I change it to low order elements? And when you refer to a higher density or smaller element size, you simply are recommending a coarser mesh correct? Thanks for the input.
in the mesh dialog you have the option to switch to "draft" mesh - that invoke low order tet's and shells. The beams are all low order all the time.
By higher density I mean more elements of a smaller size which allows for higher distortion over all (hopefully) but less in any individual element. Maybe you could post what your mesh looks like. If it is already quite fine plot the aspect ratio and maybe jocobian. for doing a dog bone type study you don't want any aspect ratio much beyond 3 and nothing over 10. If you use the 29 point jacobian check you don't want much over say 20 and down inthe single digits would be preferred. I think you would get an error at anything over 40 in the solver. You should run jacobians at different setting withteh same mesh settings. It does not change the mesh but provides a better estiamte of the jacobian withthe higher points. If you are going to induce a lot of distortion you want to start with somethng that is not too badly distorted to start with - ideally aspect ratio of ~1 and jacobians in the 0-1 range.
Bill,
Does it make sense to start with meshes that are distorted the opposite of what will happen in the analysis? For example, if you were running a dogbone tension test with the dogbone horizontal, would it make sense to start out with tall, skinny elements, so that they can stretch to be roughly square and then beyond to short in the vertical and wide in the horizontal?
Jerry S.
Hi Jerry,
It is my opinion that if you are using geostar and building a highly controlled mapped mesh you could likely make some hey on that front but in SWX Sim I don't think you can exercise the right level of control to get it done with the tet element topology. Somebody could prove me wrong but it seems a bit too trial and error for me to recommend doing it.
Bill,
Thanks. I normally use ANSYS, so I have a bit more control over the mesh. I have actually tried this out a couple of times. It seems to have worked at least once, but it's a bit hard to say what really causes issues or what fixes them.
Jerry S.
agreed.
Hi joe, switching to 2d might get you through the hump.
Jerry, your idea about the element shapes is interesting but I would be concerned with the formulation assuming all the elements are perfect.
Overall these problems are trial and error like bill said.
The solver is unable to converge. For your problem you should try making the elements smaller so the distortion is less which is my guess at what your issue is. You don't have a buckling problem as your specimen is loaded in tension. You may also wan to try low order elements to see how they stack up against the tet 10's. They are far more stable than higher order formulations with mid side nodes. In linear problems the tet 4 tend to be overly stiff. they may not be as stiff in a NL problem due to the convergence iterations. But high density maybe required as well to get a decent approximation.