Learning Forum

[Gijoys4v]

Hallo Ansys student community,

I am facing a problem.

I have a very thin metal & alloy sheet (0.1mm) of 4 layers. The length of the plate =70mm and width is 4mm. Among the 4layers one is only 1micrometer thick. I have to fix the sheet at one end and I have to provide a 360 degree twist on to the other side. I had given bonded contact between the layers. I had given 360 degree in a single step and given 100 substep. But the problem doesnt converge. Inorder to check; I had given 45 degree twist and 90 degree twist. This time the problem converged. But I want to give 360 degree twist. Then I had given 360 degree twist in 8 steps with 45 degree each and the substep of each was 100. Then also the problem doesnt converge. I also tried by giving very fine mesh. But the problem doesnt converge. 

All the time it is showing the message "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."

which is the best method to get this problem solved? is it increasing the number of elements by reducing the mesh size? or increasing the the number of steps? or increasing the number of substeps?

Please help me to resolve the issue.

[peteroznewman]

1) If the 1 micrometer layer is on the outside, don't create geometry for that, just create geometry for the other 3 layers, then in Mechanical, use a Surface Coating and pick the outside faces of the layer that the coating is applied to.

2) Don't use Bonded Contact, use Shared Topology.  If you are using DesignModeler, pick the three solids and Form New Part. If you are using SpaceClaim, click on the Workbench tab and click the Share Button.  When the Geometry update is complete, delete all Contacts in the Connections folder.

3) I assume you have large deflection turned on in the Analysis Settings. You need lots of substeps. Keep the Initial and Minimum Substeps equal.

4) You might benefit from inserting a Command object with the command NEQIT,50 to force the solver to keep iterating for longer than the default 26 iterations before it does a bisection.

5) You may benefit from Reduced Integration on the brick elements. You might also benefit from setting some Keyops on the elements that provide hourglass control.

[Gijoys4v]

Thank you for your response,

Actually the thin layer of 1micrometer is 2nd from top. Yes, large deflection is ON. You told me "Keep the Initial and Minimum Substeps equal.".How much I have to give. Is 100 is enough? How can I reduce integration on the brick elements?

Also you told me "You might also benefit from setting some Keyops on the elements that provide hourglass control.". This part I havent understood. Because I am beginner in Ansys. hourglass control means?

[Gijoys4v]

Hallo, I tried with shared toplogy and kept minimum and initial substep equal. This time it havent run. Can you please look on to my shared file. it is ansys 16.0

[peteroznewman]

Delete the Displacement Constraint, use the Remote Displacement to apply the 0.21 mm stretch along X.

Change the Remote Displacement to look like this:

Add a Mesh Method of Sweep to all bodies and set the element size to 1e-2 mm to get a few elements through the thickness.

Under Analysis Settings, change the Solver Type to Direct.

Step 1 should have Auto Time Stepping On and use 10 Initial and 10 Minimum Substeps.

Step 2 can have 100 Initial and 100 Minimum Substeps.

I suppressed the Command Object because I don't know if changing the mesh messed that up.

I solved this on the ANSYS 2019 R3 Student license.

[Gijoys4v]

Hallo,

you told me 

Under Analysis Settings, change the Solver Type to Direct.

Step 1 should have Auto Time Stepping On and use 10 Initial and 10 Minimum Substeps.

Step 2 can have 100 Initial and 100 Minimum Substeps.

But what should be the maximum, I have to give?

[Gijoys4v]

Thankyou so much and thanks a lot.

Now it is solved when I tried in Ansys 19. Previously I tried in Ansys 16. Also there I kept face deformable instead of rigid. 

 

Now I am going to try with command ON. Actually I need this. Becasuse I want to give some initial strain to all bodies.

I will inform you the progress

[Gijoys4v]

it converged with command ON.. thanks a lot