Nonlinear Statis - Nonlinear Setup

[zondashF5M2Q]

I am working with a nonlinear analysis of a model, and I am confused on what values I should have in my nonlinear setup. I currently have my number of increments set at 5 and it doesn't take too long to solve (about 10-15 minutes). Currently, there are no numerical values in the the advanced settings for the setup. I was reading that unless I have issues with the model converging, there is no need to change anything in the advanced setup. 

So is the model converging even if I do not have convergence criteria and error tolerances set? The analysis will complete if I have no inputs in the advanced setup so I am not sure if it is best to leave it alone or if there are values I should be adding. 

Some clarification would be appreciated.

Thanks!

[delaroca]

Hi, @zondashF5M2Q ,

The Nonlinear Setup already has all its fields filled with automatic numbers. For instance the "load error tolerance" is set to something like 0.0001 (or close to it). They are just hidden.

However, nonlinear simulations can be tricky, and not all run smoothly from these automatic settings. So in case of convergence trouble, you can alter some of these parameters to better converge the simulation.

You can find the meaning of each here:

https://knowledge.autodesk.com/support/inventor-nastran/learn-explore/caas/CloudHelp/cloudhelp/2018/...

And some parameter values can be found here:

https://knowledge.autodesk.com/support/inventor-nastran/learn-explore/caas/CloudHelp/cloudhelp/2020/...

For instance, checking only "displacement" and "work" in the convergence criteria, already makes the simulation takes less time and effort converging while giving similar results when "load" is also applied. Sometimes too few increment numbers will have trouble converging (each load increment will generate high displacements), and giving it more steps will be nice (15, 20, 40 steps for instance).

In short, you can tweak the advanced parameters settings if the simulation has trouble converging into a solution. There are many posts in this forum regarding convergence problems in nonlinear simulations and how you may tweak those parameters to solve your problems:

https://forums.autodesk.com/t5/inventor-nastran-forum/failing-a-simple-compression-test-nonlinear-st...

https://forums.autodesk.com/t5/inventor-nastran-forum/problem-with-nonlinear-static-convergence/m-p/...

https://forums.autodesk.com/t5/inventor-nastran-forum/nonlinear-static-analysis-failed-10-times/m-p/...

Best regards

PS: Intermediate output set to 'on' is good to see what's happening while the simulation runs

[zondashF5M2Q]

Thank you! So do I have to have the criteria I would like it to converge selected? Or if I have none selected will it automatically converge to that automatic value? 

[delaroca]

When you run the nonlinear simulation, in case it converges, it'll converge with those automatic settings (in case you didn't change any).

It may happen that the problem will converge with no issues first try.

But for more complex cases, with friction, many parts, contacts, and displacements, the solution may fail. Then you'll need to tweak those advanced parameters. Increase the number of steps, check only displacement and work (or displacement and load), increase iterations before stiffness update, etc.

It is, unfortunately, something of trying and error. Although there are some good practices, as to check at least two convergence criteria (disp & work or disp & load, for instance) and have a decent number of increments (for nonlinear static, it is recommended 15 or above).

There's no method that'll 100% guarantee a solution, especially for more complex cases. Tweaking is often required.

Usually, reducing the features/constraints applied and simplifying the simulation as a whole is the best way to make the problem converge (in case you are having trouble).

[grafiti8640]

Can you tell me what a load error tolerance of 0.0001 means? Is it 0.0001 % or 0.01 % or dimensionless? I have difficulties to make sense of this value. And what would be the highest value to obtain reasonable results?

Thanks in advance for a short response.

[John_Holtz]

Hi @grafiti8640 

The short answer is the tolerance is a relative error, so the value is dimensionless. It is some type of root mean square (RMS) or error norm for all nodes in the model.

Remark 17 for the NLPARM help shows what the default values are depending on the setting of the parameter NLTOL. That can provide a sense of what the magnitude does to the accuracy.

It gets very complicated to say specifically how the tolerance relates to the accuracy. There are many factors that are involved, such as the number of increments in the analysis (and how accurately the analysis follows the changing stiffness graph), the degree of nonlinear, and so on.

John

[delaroca]

Hello, @John_Holtz 

Actually, I'm very interested in seeing how each of these relative errors is computed (for displacement, load, and work). Is there any associated documentation?

I couldn't find any good resources on this topic, specifically on how exactly Nastran computes these convergence criteria errors.

Kind regards,

Leonardo de la Roca