Learning Forum

[1234mamanunu]

Hello to all,

 

I would like to simulate a 3point bending case with ansys. In this case, a plastic bar is loaded by a cylinder. I would like to see the stress in the bar after a 7.5 mm displacement in the y direction of the loading cylinder

 

I am using the static structural model with the following setup:

 

Geometry [has a symmetryPlane]:

 

Boundaries:

Fixed support

• Remote displacement

Analysis settings

I am getting the following error "Solver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully " , however the solver still works but it does not move the loading in the y direction. It has a strange behavior.

 

Result:

https://gfycat.com/sillyleanaustralianfreshwatercrocodile

 

Does anyone know how to solve this?

Is the static module adequate for this problem?

 

Best Regards!

 

 

[peteroznewman]

Yes, Static Structural is the right analysis to use.

1) Check that the direction of the Normal in the Symmetry Region is the X-axis.

2) Add a second Symmetry Region for the Z-axis to reduce the degrees of freedom of the beam. Since you are using frictionless contact, there is nothing to stop the beam sliding along the Z-axis.  You should slice the geometry in half, or just say your beam is twice as wide.

3) Does the top roller begin tangent to the beam?  That is what you want. You don't want to start with a gap.

[1234mamanunu]

Hello Mr Peter,

Thank you very much for your valuable help

 

I added both symmetry planes and reduced the model in half

Plane1:

Plane2:

Contact1:

 

Contact2:

 

Solver:

 

Error:

 

partial Result:

https://gfycat.com/vapidwidekillifish

 

Its almost there, but it seams to have convencenge issues

 

Best Regards!

[peteroznewman]

Do not begin the analysis with a gap between the roller and the beam.  In CAD, move the roller to be tangent to the beam.

In the Details window of the Symmetry Region, is the Normal correct?  You showed the faces, what is in the Details window?  The reason I ask is because the default value in the Detail is NOT to automatically be normal to the faces picked.  You have to set it to the correct normal yourself.

[1234mamanunu]

The normals are Ok.

I moved the roler to be tanget to be beam.

Symmetry regions:

 

I am still getting the same error:

[peteroznewman]

1) Under the Solution Information folder set the Newton-Raphson Residual plots to 5.

2) Solve.

3) Reply with an image of the Maximum value of the Newton-Raphson Force Residual.  This is often where a smaller element can help convergence.

4) Under Solution Information, reply with the Newton-Raphson Force Convergence Plot. In some models, it is helpful to insert a command to tell the solver to use more than the default 26 iterations before starting a bisection.

5) There are changes to the element formulation that can help such as Reduced Integration if the above does not help.

[1234mamanunu]

Here are the results:

To topic 3:

1st :

2nd:

3rd:

 

4th:

5th:

 

worksheet:

Are these type of cases hard to solve?

Is it possible to upload the case?

Best Regards!

[peteroznewman]

Here is how to create a file that can be uploaded using the Attach button that appears after you post.

This post has a video showing how to track down convergence issues. There are other posts in that Disucssion you might find interesting.

 

[1234mamanunu]

 

 I will update the case here if anyone wants to help.

If I am able to solve it, I will upload the solution.

[peteroznewman]

The biggest problem is that the contacts are not closed. Insert a Contact Tool under the Connections folder to learn this information.

The corrective action is to Adjust to Touch on the two contacts since the gap is small.

I flipped the Contact and Target sides of the contact.

I made smaller elements. I changed the Step controls.

It now solves.