ABAQUS: Model not converging after turning on NLGEOM (Even with very small steps)

[hwa0725]

Hi all,

As the subject, the model is running fine with NLGEOM turned off but as soon as I turned it ON, the model struggled to converge. I have reduced the initial and minimum increment step size and increased the number of attempts (I_A) the solver can reiterate with a lower step size and still no luck getting this to work...

I am doing a multisteps analysis, however, the model can't even get past the first step, in which I pre-loaded the column axially with compression load before loading the end of the cantilever in the second step.

Attached is my Abaqus model if anyone wants to look at it.

https://files.engineering.com/getfi...C82-7091-4064-9cb6-be627e48203b&file=test.cae

https://files.engineering.com/getfile.aspx?folder=f417f467-8fa3-4770-8032-cceaf6072728&file=test.jnl

Many thanks, folks!

Regards,

Heng

 

[FEA way]

Reducing the increment size so much won't help. You should gradually simplify the model to find the source of the issue. Especially focus on connections. In such assemblies, it's often the case that some parts are not properly connected and only enabling geometric nonlinearity reveals that. I would also recommend using a frequency analysis to check the connections.

 

[hwa0725]

Hi FEA way,

Thanks very much for replying. I tried the frequency analysis as you have suggested and the connection looks alright, nothing is flying apart.

The strangest thing is that the model only converges under a certain combination of load and initial increment. I have tried to play around with the solver setting, for example, switching between symmetric and unsymmetric matrix storage, direct and iterative methods and full newton and quasi-newton solution techniques but none of these seems to work.

I also checked if the mesh was ok and apparently, I received no warnings in the check using the Verify Mesh method.

Could it be the way that I am applying the load? I applied a concentrated load to a reference point that was coupled to the cap plate of a column. I am using kinematic coupling with all DOF locked and then applying boundary conditions to the reference point along with the concentrated load. I would presume this is the standard way of doing it.

Many thanks!

Regards,

Heng

 

[FEA way]

For me, the 3 parts detach. Maybe because I couldn’t download your .cae file for some reason so I had to download rhe .jnl file instead and recreate the database from it which resulted in some keyword errors so maybe interactions were not recreated (there aren’t any). Can you try uploading the .cae file again (maybe zipped) ? If it doesn’t work then the .inp file might suffice but .cae would be better.

 

[hwa0725]

Thanks very much mate, I have reattached the link to download the zip folder with .inp and .cae files in it.

 

[hwa0725]

I think I might have found the issue. The concentrated load I was applying was too low relatively causing abaqus to think the section was too stiff. I was applying a load at a fraction of 0.001% to the axial capacity of the column. Increasing the load to 1% of that works like a champ. As the 1% load is still very low relative to the column capacity, I need to increase the initial increment to ensure abaqus don't reduce the subsequent inc and worsen the convergence.

So am I right in saying that Abaqus or other FE software don't like models with low loading-to-stiffness ratio?

 

[centondollar]

So am I right in saying that Abaqus or other FE software don't like models with low loading-to-stiffness ratio?

No. There is no physical problem with small loading, but a loading too large may cause failure (e.g., buckling-type loss of stiffness) at the first load increment, leading to non-convergence. Reducing the initial load level will counteract such effects (some software restart automatically at smaller load levels if convergence is not achieved), but the loading should of course be applied as it is applied in reality.

The abaqus software manual should include a chapter on settings for non-linear analysis. My guess is that you've ticked some box that stops the analysis due to very small loading, although I find such a setting unintuitive - see my previous comment.

 

[hwa0725]

[No. There is no physical problem with small loading, but a loading too large may cause failure (e.g., buckling-type loss of stiffness) at the first load increment, leading to non-convergence. Reducing the initial load level will counteract such effects (some software restart automatically at smaller load levels if convergence is not achieved), but the loading should of course be applied as it is applied in reality./quote]

Hi Centondollar,

Thanks very much for your reply. Yeah, I would have thought so that a small loading should not be a problem. However, when I applied a load equivalent to 1% of the column axial capacity, it ran like a champ. No luck getting anything run when the load is less than 0.01% of the column axial capacity, even with a time step of 1e-30 and still not getting any sign of convergence.

I am not aware that there is any tick box that will stop the analysis when the loading is small. If it does, Abaqus would have probably thrown an error saying "the load is too small and the analysis was aborted" without even attempting to do any calculation/iteration to begin with.

Regards,

Heng

 

[ThomasH]

I don't understand if you have managed to get a solution or not. But one way the investigate if a small load step is a problem would be to try it on a model that you know works.

The only explanation I can think of is something weird. If you have a very low load, that could mean that contact can't be correctly established. And that would mean that it doesn't converge, meet criteria, from a numerical point of view.

But my experience is the opposite, small steps makes it converge. But my experience is not with ABAQUS. There may be something specific for ABAQUS even if I doubt that .

 

[centondollar]

"If you have a very low load, that could mean that contact can't be correctly established."

Geometric non-linearity (static load stepping) does not involve contact, so it shouldn't be that, although OP might have omitted some details from the model.

 

[IceBreakerSours]

1) Start from scratch - Are the units consistent? Are the input "numbers" correct?
2) Build complexity in a step-wise manner - i.e., the baby steps strategy. Ensure something is working, you understand how a key feature works, and add complexity one layer at a time.
3) Since you find yourself in a bit of a spot, try to do a "binary search" and isolate the source of the trouble. By that I mean, take out sources of nonlinearity one at a time, and see if the model performs any better.
4) There is no harm in playing with knobs but, over time, try to turn them with a decent appreciation of the physics and the numerics of the problem at hand. Reducing the initial time step size is rarely the answer for most problems I and others I know have run into.
5) Do you have someone to talk to? A mentor, perhaps? Do you have other sources of support? Maybe something to talk about with your manager.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083