Learning Forum

[ma826]

 Hi 

I am trying to run a non-linear static structural analysis but I faced the following error:

"The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information."

 

I tried to follow all non-linear steps such as:

Research Licence; finer mesh and increase in substep; in contact tool, all contact status is closed;  large deformation is on

 

I used multi linear isotropic hardening model

based on the below link (Peter's suggestion)

/forum/forums/topic/elasto-plastic-curve-and-multilinear-isotropic-hardening/

 

Can anybody help me how I can solve the issue?

Best Regards

[ma826]

thanks peter, The archive file is too big to upload, is there another option to send the file to you all?

 

here is the attached archive file

 

[peteroznewman]

Either in Mechanical, RMB on Mesh and Clear Generated Data or 

in Workbench, RMB on Model and Clear Generated Data

then Save the Project, then make the Archive. It will be smaller.

If it is still too big, members are posting with a Google Drive link.

[ma826]

I just uploaded the archive file above,

Thanks

[peteroznewman]

The model looks good, but it is a large model that can't be solved on a Student license.

There are several Discussions to overcoming convergence issues.      Here is one.       Here is another.

I would advise you to take two planes through the center of the part and slice it into a quarter model and use symmetry.

That way you will fail 4 times faster  : )

[ma826]

Thanks Peter,

I had a look at the both links. very helpful.based on Newton iteration, it seems that the convergence problem related to contact at the lattice structure.  I decreased contact stiffness and rezoning as well, but still convergence problem remains. (can be due to that the total applied displacement is about 70% of total structure height: large loading?)

Can you please let me know how I can slice my model as it current takes time (~15 hrs)

 

Thanks again

 

[peteroznewman]

When I say "slice" that is the DesignModeler term. But you have your own CAD system. All that means is to cut the geometry in 4 pieces through the center and throw away 3 of the 4 pieces. On the cut faces of the remaining piece, add a displacement BC and set the normal to the cut plane equal to zero and leave all other displacements Free.

Please show me your N-R Force Convergence Plot.

All I did was change the units from m to mm and change the solver to Direct and it is converging quite well so far...but maybe the problem comes later.

[ma826]

Thanks once again,

yes, you are right, convergence problem happened later when more loading occurred..

below is the N-R figure 

[peteroznewman]

Are you going to do the 1/4 symmetry model?

[ma826]

sure, but 1/4 symmetry model can only boost the simulation faster but I dont think the contact problem can be solved, isn't it?

 

 

[ma826]

Hi agian,

it faced again contact problem (after 5 hr running)

here is the N-R figure:

 

also, the solver solution is here:

 

any help will be highly appreciated

Thanks

 

[peteroznewman]

Please show the N-R Residual Force Plot. Was it on the way to converging or was it diverging?

The 1/4 model ran for 5 hours while the full model ran for 15 hours. Say it takes you 10 tries to get to a good result, isn't it better to get there in 50 hours rather than 150 hours?

Have you tried relaxing the contact penetration tolerance so it can keep solving?  Have you tried making the contact stiffness higher so there is less penetration?

[ma826]

Hi Peter,

I sliced the structure and run 1/4 for faster simulation. there is still convergence error (after a while, ~0.5s) and is not able to solve for whole applied displacement. based on solver output and N-R residual force  it is related to contact of the strands of lattice.

I used rezoning (nonlinear adaptive region) as well.

I would be greatly appreciate if you can have a look at attached archive file and let me know what else I can do it.

Regards 

[peteroznewman]

Hi,

Please check your material properties. The data in the Multilinear Hardening looks like it may have the wrong units.

I changed the units to MPa and the solver had no problem starting after failing when the units were Pa.

 

[ma826]

Hi Peter,

It is strange. because in my model, the unit is MPa as below picture shows. I created the multilinear model based on what you mentioned in the below link: 

I attached the excel file of material tensile test and data that I used, calculated true stress, true strain, elastic and plastic strain

/forum/forums/topic/elasto-plastic-curve-and-multilinear-isotropic-hardening/

 

 

[ma826]

I can not attach excel file, here is the picture of stress-strain data

 

 

Many thanks Peter

[peteroznewman]

You have to put Excel files in a Zip file to attach.

The archive above definitely had Pa as the units, which caused it to fail to converge right from the start.

It also had a different material Name.

  

[ma826]

Thanks Peter, 

You are right.

I got confused and showed you window of material properties for first full scale lattice.

I changed unit in 1/4 scale.

Is there anything that I have to change in analysis setting (like N-R option to e.g Unsymmetric or force convergence ..)

 

Thanks once again

[ma826]

here is the solution output:

[ma826]

one more thing;

based on solver output. the element is Solid185 which is not suitable for nonlinear behavior. can it be the problem?

[peteroznewman]

SOLID185 is suitable for nonlinear behavior, why do you claim it is not?

You had 1 step to do 4 mm and it failed to converge about 10% or at 0.4 mm.

I suppressed the Nonlinear Adaptive Region.

I made Step 1 be 1 mm and Step 2 take it to 4 mm.

The result was the the bottom foam just sank into the bottom block.

That was because you have changed the normal stiffness to 0.01

I recommend you Flip Target/Contact sides and change the Detection Method.

I can't test this now, so you will have to give it a try.

 

[ma826]

Hi Peter, Thank you for your helpful comments.

I did the changes and run it, waiting for the output (after 10 hrs, still waiting). Hoping can get the results.

about number of steps, I did the below changes as you mentioned. is it correct?

 

[peteroznewman]

After 10 hours, you should Interrupt the solution and see how the solution looks. It could be completely useless so it is best so check that it is useful. If it is useful, you can Restart the solver at the point where you interrupted it.

The Step Controls look fine.

[Rohit G]

Hi all

I am trying to run hyperelastic analyis for a composite model

I am getting the same error 

"The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information."

I am new user of ansys , please help me to resolve the issue 

PFA the link https://drive.google.com/file/d/1FOuXEkPFHDYYQBIfmlqnUBs6xlnu4B1E/view?usp=sharing

 

Thanks in advance