Learning Forum

[JooJaehoon]

Hello!

I'm conducting compression test of quarter cylinder

It is composed by upper press, lower press and quartercylinder

Cylinder has 8 mm height and it compressed into 4 mm by upper press

Cylinder has non-linear properties(attatched as picture) and upper, lower press has rigid body(set extreme high young's modulus, poisson ratio = 0)

So, I think deformation has a large value so large deflection option must be checked

Analysis started and it's convergence failed

Error occured at convergence gauge at 16% and I attached error result picture

I attached analysis condition picture too

I raise initial substep into 1000 but it was failed too

With unchecked large deflection option, convergence completed

How can I converge this problem?

regard

[peteroznewman]

The model had some converged substeps. Select the last converged subsetp to plot the deformation. That is the row above the End Time in the Tabular Data.

Under Analysis Settings, click on the Solution Information folder, and in the Details window, select Force Convergence and reply with a screen snapshot of that graph.

Then change from Force Convergence to Solution Output. Click ctrl-F to find the word error. Read the text around that word, Copy paste the text into your reply.

Set the Initial and Minimum substeps to 1000 and solve that.  With plasticity, it is important to prevent the solver from taking large steps late in the solution time.

[JooJaehoon]

Hello! Peter!

Thank you for applying!

The first picture is force convergence graph

And, the second and third are error message in Solution Output tab

regards

 

[peteroznewman]

Was that force convergence plot from the run with the Minimum Substeps set to 1000?

Next you should look at the last converged substep. We can see the time is about 0.11 which is the fraction of the 4 mm total displacement or 0.44 mm that the top plate moved before elements became too highly distorted to continue the simulation.  I suggest you change the displacement of step 1 to 1 mm and add a second for 2 mm, and so on.  Keep the initial and minimum substeps at 1000 for step 1. Does the simulation get any further down? 

From the error message, you have an element number to look at. Create a Named Selection so you can isolate that element and watch how it deforms over the time steps that converged.

In the unconverged displacement plot, I see some elements along the center axis seem to have buckled. Are the nodes staying on the two symmetry planes you defined? Change the contour option to Capped Isosurface so you can see the elements that had displacement > 0.1.

[JooJaehoon]

No, it's rest I've post first

But, I try to analysis with applying substep as 1000, but result still have not converged with distortion of element.

Now, I set displacement step as more than 1 and will conduct analysis.

As soon as end of analysis, can I ask a question with new result?

I'm appreciate of your help.

Have a nice weekend!

[peteroznewman]

Yes, reply with new results when you get them.

[JooJaehoon]

Hi 
I finshed analysis last I mentioned and it was failed to converge.
But, I'd got method to converge this problem.
I changed static structural solver into transient structural and applied semi-implicit code.
Then, I was able to converge this analysis with small substep and basice option.
I've got hint for your comment.
Thank you