convergence problem

Post Reply
Telec
Posts: 27
Joined: Sun Oct 11, 2020 8:27 am

convergence problem

Post by Telec » Wed Oct 28, 2020 4:28 pm

Hello,
using the instructions obtained on the forum I modeled a simple pinned plate in the 4 corners loaded with a concentrated load in the center. As material I used DmageTC3d and ASDShellQ4 as element. After several attempts I managed to obtain satisfactory results but the analysis always stops due to convergence problems. How can I fix them?
model.rar
(80.96 KiB) Downloaded 7 times
Moreover, there is no longer the possibility to insert the p-flag in the test control?

Also I noticed a strange thing, decreasing the load increment, the analysis does not converge and gives me less precise results. (Analyze 30 or 35 gives me good results inspite of 50 or 100 steps)

I tried to use a triangular mesh with ShellNLDK element and the analysis reaches 100% without convergence problems but with an incorrect result.

STKO Team
Posts: 339
Joined: Tue Oct 29, 2019 8:45 am

Re: convergence problem

Post by STKO Team » Fri Oct 30, 2020 3:45 pm

After several attempts I managed to obtain satisfactory results but the analysis always stops due to convergence problems. How can I fix them?
I made some changes in the analysis. But the most important change is that you used LoadControl while I used DisplacementControl. Note that you will never manage to run an analysis with a softening regime, with a LoadControl integrator, that assumes that the resisting forces will always be increasing.
Also I noticed a strange thing, decreasing the load increment, the analysis does not converge and gives me less precise results. (Analyze 30 or 35 gives me good results inspite of 50 or 100 steps)
First, in general in nonlinear analysis with brittle materials, it is always a good idea to use many time steps (small time increments). It will improve accuracy and convergence.
Here we have an extra issue: When you use the DamageTC3D with the IMPL-EX method, your analysis will always converge (if equilibrium exists of course, and assuming that is the only nonlinearity in your model...), but the response is semi-explicit, so it depends on the time step size. The smaller it is, the better.
I tried to use a triangular mesh with ShellNLDK element and the analysis reaches 100% without convergence problems but with an incorrect result.
That element is for nonlinear geometric analysis...
Moreover, there is no longer the possibility to insert the p-flag in the test control?
Yes, it is not used anymore because now we have a much cleaner way of showing the analysis statistics. See the monitor utility in the 2 files attached.

Finally, here are 2 files with all the corrections:
The first one is like the original one (with corrections only with respect to the analysis settings). That is, still pinned in 4 corners and with a concentrated load.
Note however that, when dealing with brittle materials, it is not a good ideat to place BC and Forces punctually, as this will create high stress concentration and premature failure. In the secon file, I used a more realistic apprach, modelling the pins with contact elements, so that the reactions forces will be redistributed over a small area rather then a point. Similarly I applied the force distributed onto a small loading steel place, that then is placed in contact with the slab.

model.zip
(119.43 KiB) Downloaded 6 times
model_3.zip
(189.31 KiB) Downloaded 6 times

Telec
Posts: 27
Joined: Sun Oct 11, 2020 8:27 am

Re: convergence problem

Post by Telec » Tue Nov 03, 2020 1:37 pm

Note that you will never manage to run an analysis with a softening regime, with a LoadControl integrator, that assumes that the resisting forces will always be increasing.

yes I know. In this case, however, I was only interested in making a comparison with an experimental test performed on the same plate for which I have a curve that stops before reaching the peak point.
In this case, using the DISPLACEMENTCONTROL I get a different result from the experimental one.
First, in general in nonlinear analysis with brittle materials, it is always a good idea to use many time steps (small time increments). It will improve accuracy and convergence.
Here we have an extra issue: When you use the DamageTC3D with the IMPL-EX method, your analysis will always converge (if equilibrium exists of course, and assuming that is the only nonlinearity in your model...), but the response is semi-explicit, so it depends on the time step size. The smaller it is, the better.
if instead I wanted to use an IMPLICIT answer what would change?
That element is for nonlinear geometric analysis...
To take into account the geometric non-linearities with the ASDSHELLQ4 element, do I have to check the COROTATIONAL option instead of LINEAR?

STKO Team
Posts: 339
Joined: Tue Oct 29, 2019 8:45 am

Re: convergence problem

Post by STKO Team » Tue Nov 03, 2020 3:41 pm

In this case, using the DISPLACEMENTCONTROL I get a different result from the experimental one.
Theoretically there should be no difference, at least up to the peak point, where of course the load-control would stop. If you have different results is probably due to the fact that, when moving from load-control to disp-control, you changed the time-step size, and as I've seen, you where using a time step which was too large for the IMPL-EX method. I'm pretty sure that, if you repeat the same analysis with both disp-control and load-control, with small enough time steps, they will match up to the peak.
If instead I wanted to use an IMPLICIT answer what would change?
The solution would be implicit, as 99% of the nonlinear models. However it will make the solution a lot more nonlinear. In this case you don't have a limit on the step-size (because it is completely implicit). However, since you will have convergence problems, the time step will be smaller anyway.
To take into account the geometric non-linearities with the ASDSHELLQ4 element, do I have to check the COROTATIONAL option instead of LINEAR?
Yes

Post Reply