Learning Forum

[faridnugroho21]

Hi,

So I found another error while meshing the geometry. I followed all of the instructions given in the video.

And here's my setting

For the Multizone Method

 

And here's the global mesh setting

So, how to fix it?

 

[SaiD]

Hello! Thank you so much for bringing this issue to our notice. We are looking into it and will get back to you soon.

[SaiD]

The defaults are different for Ansys Mechanical 2022 R2 and the version of Mechanical being used in the video. We will work to add the correction. But for now, under the Details of "Mesh", please go to Quality > Error Limits and set it to "Standard Mechanical". You should be able to generate the mesh then. Hope this helps!

 

[faridnugroho21]

Thank you very much for the answer sir ! :D

 

[faridnugroho21]

I'm sorry have to ask you again, when I try to mesh the topology optimized design, It failed. And then I tried to mesh it with global mesh and perform the convergence to obtain the best result for the stresh. But, the mesh cannot be more refined.

[SaiD]

Hello, thank you again for pointing this out. The way to fix this would be to suppress the MultiZone Mesh method and allow the geometry to be meshed using tetrahedral elements. I tried using a global element size of 3 mm and 2 mm and both were able to generate valid meshes.

 

I also tried inserting a Convergence object in Equivalent Stress. It did not work and the error message indicated that it was because certain objects were scoped to nodes/elements/element faces. This happens because we have a Named Selection in our model that is scoped to the mesh. When you use Convergence object, the geometry is remeshed and hence the Named Selection needs to be regenerated, but Mechanical is not able to do that. If you suppress the Named Selection and the Equivalent Stress scoped to that Equivalent Stress, you should be able to use the Convergence object.

However, when I tried using the Convergence object for Equivalent Stress of the Body (Type: Maximum, Allowable Change: 5%), I was not able to achieve convergence. This is probably due to a stress singularity occurring at the corner where the Max equivalent stress occurs. To understand more about Adaptive Convergence and Stress singularity, please check out this video:

Using Adaptive Convergence with Ansys Mechanical — Lesson 5 - ANSYS Innovation Courses

Hope this helps! Thank you again for bringing the meshing issue to our notice. 

 

[faridnugroho21]

Thank you very much! this is very helpfull, sir. :D