I have a model that runs in static linear. It will not run in static non-linear. It simply runs through the 19 time steps and constantly returns a residual convergence of 1.
Can a developer or Autodesk person have a look at it and see what I have overlooked? I have successfully changed the analysis type on a smaller model before.
I copied across to a new design scenario.
changed all plates to shells
changed element definitions
re-assigned material to be sure
re-assigned pressure load
check analysis parameters and added a load curve
I tried to attach and ach file; but it was 11 MB. To whom would I send that file?
Solved! Go to Solution.
One suggestion is to set the load curve(s) magnitudes to 0 so that there is no load on the first time step.
- If this solves, then it may be that the initial load is too large.
- If this does not solve, my guess is that something in the model is statically unstable.
- Are all of the parts connected node-to-node? (Linear stress has "smart bonding' which connects parts even if the nodes do not match; MES does not have this capability.)
- The only other thought that comes to mind is the solver that is used. Either the log file or summary file (accessible from the Report tab) indicate which solver was used, such as the iterative solver or sparse solver.
Otherwise, did you try the tips in this post to reduce the size of the archive? http://forums.autodesk.com/t5/Autodesk-Simulation-
16 years experience with Simulation Mechanical
If you can change the "Element Formulation" in "Advanced" Tab of Elment Definition of the 5 Parts (1~5) from "General" to "Thin", the model will run to completion smoothly.
The 5 Parts (1~5) have the other dimensions much larger than the thickness, so "Thin" shell will be appropriate for them.
Thank you for suggestions.
Manually setting the solver to sparse (it was automatically going to iterative AMG) allowed it to solve in 20 time steps and 1.5 hours.
Setting the element formulation to thin allowed it to run; but at 25% started reducing time steps to solve so I stopped it.
I guess I will try thin and sparse.
I would have thought it would automaticallly try sparse if iterative did not work. I would appreciate comments.
Within their capabilities, "Sparse" solver and "AMG" solver should provide similar results. However, "Sparse" solver usually works for small or medium models, while "AMG" solver works for large model.
Once "Automatic" option is defined, the code will automatically select one of them based on the size of equation.
I have this problem again. I am applying a hyrdostatic pressure and it looks like the solver does not recognize the pressure. I put a simple force on it and it does run.
Copying a design scenario (Linear) to another one (Nonlinear), we do need to click the "Element Definition" for all the parts, since Nonlinear and Linear use different AGSDB variables, defined by UI. You did right.
To use "Static Nonlinear with Nonlinear Material Models" analysis type, the model must be static stable and well constrained to avoid any rigid body motion. For your model with shells, the model should not move along x-, y-, and z- directions, and not rotate along Rx-, Ry, and Rz. Otherwise, the model generally cannot converge with "Static Nonlinear with Nonlinear Material Models" analysis type.
If you think the model is well setup, you can try "MES with Nonlinear Material Model" and see this can help.
You can send the model to me via email.