Learning Forum

[alexiospaschou]

I have created a square RVE (representative volume element), which contains some inclusions. I have created the mesh in GMSH and I have imported it in Ansys. In GMSH I have created two different physical groups, one for the matrix material and one for the inclusions material. These groups exist in Ansys under Named Selections.

Afterwards, I assign the materials to the two groups. At this point, everything is checked except Geometry which has a question mark. When I try to solve this, the aforementioned error pops up.

If I assign a material to Geometry, then Geometry is also checked and the solve runs with no errors. But I want to assign two different materials for the two groups. Is there a way I could fix that?

[Sheldon Imaoka]

It seems that your mesh is treated as a single body - under the "Geometry" branch in the Tree Outline, do you see 1 part or 2 parts? When you say that you "assign the materials to the two groups", how are you doing this? Are you using "Commands (APDL)" objects?
If you are using "Commands (APDL)" objects, then the material assignment should override the initial material assignment in Mechanical, so what you did should be fine. If you supply answers to the above questions, it may be clearer for others to provide assistance, depending on how your materials are currently being assigned.
Regards Sheldon

[alexiospaschou]

Hi Sheldon thank you very much for your reply. Under the "Geometry" branch I see 1 part, named "Surface Body 1(External Model)".
I am not using any APDL commands. I assign the materials to the two groups, which are listed in "Named Selections" branch. I upload some pictures to be more precise. In the first picture you can see the whole mesh and in the next two pictures you can see the meshes corresponding to the two physical groups. I right-click to each of the two groups under the "Named Selections" branch, then I click "Create Material Assignment" and then I assign the material.
At this point the "Geometry" branch has a question mark. When I try to solve this, the error pops up. If I assign a material to Geometry, this weird check symbol with "X" appears next to "Surface Body 1(External Model)" (picture 4). Afterwards, I can solve the problem. But which material assignment is used? The one from the "Geometry" branch or the one from the "Named Selections" branch?
Regards Alex

[Sheldon Imaoka]

Hi Alex When you mention that, in Figure 4, you have an "x", it is actually not an "x" but a green checkmark with an additional tick mark. An actual "x" would appear in red color. The additional tick mark means that it is a meshed part (please see Mechanical help, under "Application Interface -> Outline -> Understanding the Tree Outline" for additional details on the Status Symbols).
The Material Assignment overrides the material assigned under the Geometry branch. To verify this, add a "User Defined Result" object under "Solution" with Expression "PNUMMAT". PNUMMAT gives you the numeric material ID - if the material ID is the same, it's most likely the same material, but if the material ID is different within the same part, it's a different material. This should show that 2 different material IDs are used in your model. (The meaning of the ID number is internal and part of the solver input file "ds.dat" if you are curious and want to view it, but if you just want to verify visually that 2 different materials are used, a User Defined Result for PNUMMAT will help you see this.)
One thing you may need to be careful about is that, when plotting stresses and strains, the default is to average values - since you use "Material Assignment", it won't automatically not average across the different material boundaries. Thus, I'd recommend looking at unaveraged stresses and strains, so the results don't get smeared at the boundary between your two materials.
Regards Sheldon

[HOANG CUC]

Dear Alex,

 

I am having problems importing files from GMSH into ANSYS. I see you imported successfully, so can you explain each step you did? From the step you create the mesh in GMSH and export it. And finally, how do you handle importing files into ANSYS?

 

Regards Phuong Cuc Hoang