Mesh control seems to be applying on only one side

[naqib_mashrur4YFQQ]

 I applied mesh control at the edges where the separate solids meet, as can be seen in the image. However, it seems like the mesh control is only being applied to one side of the selected edge, i.e. one of the two connected solids. I am guessing it's because the edge "belongs to" only one of the solids - but I wanted to make sure I am right about that. I also wanted to ask if this would cause any issues for my analysis. Should I apply the mesh control to both solids to get meaningful results?

[John_Holtz · Accepted solution]

Hi Naqib,

Your guess is correct: the mesh control is applied to a part and it only affects that part. If you want the mesh refinement on the adjacent part, you can select that edge also.

Technically it is okay to refine one part but not the adjacent part. The contact with connect the faces regardless of the mesh size. However, I would think that you want to refine both parts to get a better "match" for the contact and have similar size elements (and similar stiffness) on each side of the contact.

Since the mesh is somewhat random, there will always be some randomness right at the contact face. The goal is to try to reduce that.

John

[Ihor_Radikhovskyi]

Hi,

Just to add to John’s explanation:

In many cases this will still solve correctly, but if the mesh density is very different on each side of the contact, it can introduce local inaccuracies — especially in stress results near the interface.

In practice, I try to keep a similar element size on both sides when the contact area is important for the results (e.g. load transfer, stress evaluation).

If the contact is not critical, refining only one side is usually fine.

[naqib_mashrur4YFQQ]

Thank you both for the explanation. I think with this information, it is best I apply the mesh control to both faces, especially at interfaces that show higher stresses.

[naqib_mashrur4YFQQ]

@John_Holtz and @Ihor_Radikhovskyi, I had a follow up question for you both. What is the best way to apply mesh control to both solids? I made the solids in inventor by extruding the solids on top from the one at the bottom. The Nastran environment cannot find an edge on the bottom solid to apply mesh control to. 

[John_Holtz]

Hi Naqib,

You should be able to hide the part that already has the mesh control so that you can select the edge on the part that was not being selected. Just right-click the part to hide in the Nastran Model Tree and uncheck Display. This will hide the CAD part. Now you can edit (or add) the Mesh Control and select the geometry on the visible part. Note that hiding the part does not hide the mesh. It is not necessary to hide the mesh to make the selection, unless the mesh makes it hard to see what you are selecting.

John

[naqib_mashrur4YFQQ]

I am able to hide the part, but the solid at the base does not have the geometry feature. I don't have an edge I can select. I am trying to see if I can split the bottom face in inventor using the project geometry tool, but the split tool is not taking the entire sketch as one sketch.
Re: Split tool not selecting all the curves from a D sketch - Autodesk Community

[naqib_mashrur4YFQQ · Accepted solution]

For anyone who might read this later, I was able to solve the issue. I had multiple parts connected to one part, and I used the Project Geometry tool to generate sketches on the part I wanted to split. The generated sketches had overlapping lines. The split tool does not like it if there are overlapping lines and closed loops. I had to turn the overlapping lines in the 2D sketch into construction lines using the construction sketch tool. I had to do with twice on every overlapping line segment so that the line sketched from both solid was converted into a construction sketch. After converting every overlapping line into a construction line, the split tool was able to accept the edited sketch and split the solid.