Learning Forum

[Kevin1993]

Hello,

I'm studying about steel structure non-linearity behaviour under seismic loading, but when I try to run analysis in Ansys Mechanical APDL suddenly the analysis terminated and I get several warning with 1 error messages "The solver engine was unable to converge on a solution for the nonlinear problem as constrained....", after checking to "Solution information" it is clearly stated

 

*** ERROR ***

Solution not converged at time 2.5 (load step 3 substep 1).
Run terminated

 

Right now I'm a little depressed. I can't figure it what or why solution not converged.
Your reply will be very helpful.

Regards,
Kevin

[peteroznewman]

Kevin,

I'm looking at the Remote Displacement load.

This is pushing and pulling on the top of the structure with larger oscillations of displacement.  Why are you doing that?

It is the worst idea for efficiently solving the deformation of the structure out to the limits of displacement.

A much better idea is to have a single step that goes out to 30 mm.

Perhaps you are trying to build up plastic strain. You don't have the correct material model to accomplish that. You must use Charboche.

[Kevin1993]

Dear Peteroznewman,

 

About "This is pushing and pulling on the top of the structure with larger oscillations of displacement.  Why are you doing that?" , I want to do cyclic analysis to the structure following testing procedure from ATC and AISC until the material become plastic.

"It is the worst idea for efficiently solving the deformation of the structure out to the limits of displacement.", Any suggestions how do i know the structure displacement limit?

"A much better idea is to have a single step that goes out to 30 mm.", I'm sorry but I don't get what do you mean about this one.

"Perhaps you are trying to build up plastic strain. You don't have the correct material model to accomplish that. You must use Charboche." yes i was trying to do analysis until the structure become plastic not elastic anymore, and i will study about "Charboche".

Is there anything wrong in my model? I'm a newcomer to Ansys.

Thank you Peter, your reply and suggestion are very helpful to my research and thesis.

[peteroznewman]

Dear Kevin,

I don't have a copy of the testing procedure from ATC and AISC so I don't know what you want to simulate.

Do a Save As to a new file name so you can go back to your initial model later, after you have read more about Charboche.

You can use the material model you have to find out the tip displacement when plasticity begins.

You do that by having a single step with an End Time of 30 s and a single value for the remote displacement: 30 mm.

Under Analysis Settings, make sure Large Deflection is On.

Turn on Auto Time Stepping.

Set the Initial, Minimum and Maximum Substeps to 60.

This will give you a data point about every half mm.

Click on Solution and request an Equivalent Plastic Strain.

The Plastic Strain result will be zero for small displacements while the material is in the elastic region, then it will be non-zero when some elements reach the yield stress.

The time in seconds when the plastic strain goes above zero is the value of displacement in mm since the end time and displacement values were equal.

 

[Kevin1993]

Dear Peter,

 

Thank you so much for your assistance Peter, i will follow your instruction and update it in here.

I will summarize what research i'm doing, and i will post it here so you can understand what i meant.

Anyway how to setting time duration in one single step, because i can't edit it. each step default time is 1 second.
Is there any video or tutorial about this?

 

Regards,

Kevin

[peteroznewman]

Here is what you had and what you want.

    

Edit the Remote Displacement, select all the rows except the last one and delete rows.

[Kevin1993]

Dear Peter,

My research goal in ANSYS was to verify existing experiment.
The experiment was a laboratory test, the test setup looked like my model,
this experiment simulate cyclic loading with hydraulic jack pushing and pulling at the top.
One of the experiment result was a "load vs displacement" diagram.

 

[peteroznewman]

What conclusions were drawn from the experimental data?

[Kevin1993]

Dear Peter,

Should i start a new discussion rather than continue this one?
because our topic had changed from "converge error" to my research "plastic strain analysis".
Actually my answer already answered in one of your post, I will choose one of your post as solution to close this discussion.

Besides that conclusions were drawn from the experimental are usually behavior (plastic deflected shape), displacement (to plot load vs displacement), and stress (to indicate yield).

[peteroznewman]

Yes, you can close this discussion and start a new discussion for the new topic.

[Kevin1993]

Peter right now i'm still having issue about convergence, my model have 4 warnings and 1 error. Major issue that stated in the warning and solution information are rigid body motion and element convergence.

I already try several option such as make element size smaller and increase substep, but it's doesn't solve the issue at all.

Just information for material properties i'm using kinematic hardening condition.

[peteroznewman]

Where did you get the data in the multilinear kinematic hardening model?

The convergence problem is because you put 1E-06 as the entry in cell C2. That value should be the Yield Strength.

Do you know the difference between:

• Engineering Stress and Strain


• True Stress and Strain

???

The values in that table are supposed to be True Stress and Strain.

Review this discussion.

You can use a kinematic hardening material model to pull the column to one side and observe the plasticity developing and the force diminishing.

You should not use this material model to cycle the tip back and forth. You should use Charboche Kinematic Hardening for cycling. This is third time I have mentioned this.

I recommend you insert planes in DesignModeler and Slice the geometry up to get regular shaped elements like this:

[Kevin1993]

I'm sorry, i'm too stubborn and don't realize it Peter.
Thank you very much for your help.

Besides that actually right now i'm still learning how to use chaboche material, because i still don't understand it.

Anyway i can't open the files to attach, it says it's saved on the newer version.

[peteroznewman]

I was working in ANSYS 2019 R2.

[Kevin1993]

Okay thanks Peter, your answer are very helpful.