Mesh Failed - Thread Analysis

[travis.potier]

I am trying to analyze the 3D effects off a threaded connection. I've rebuilt the model multiple times, rotated the thread in case knife edges causing problems. When I'm able to get the male threads to mesh, the female threads fail. I make modifications to get the female threads to mesh and the male threads fail. I've utilized a 180 degree symmetry model. There's no indication as to where the problem is, only that the mesh has failed.

Has anyone dealt with such issues (mesh failing with no indication as to why?), and were you able to solve it?

[John_Holtz]

Hi Travis,

Mesh failures are frustrating. What version are you using? Version 2025 has a new diagnostic tool which sometimes will point out where the problem occurs. Otherwise, here are a few tricks that I typically use.

• Try a finer mesh.
• If one part does not mesh but other parts do mesh, try making the parts that do mesh invisible. Leave the part that does not mesh visible. Another option is to use the Mesh Table to mesh only the part that is failing.
• If those do not solve the problem, temporarily change the idealization of the failing part to shell. Enter a dummy thickness. 
  • If the surface mesh is successful, look for white/gray lines on some of the edges. These indicate where the mesh on one face does not match the mesh on the adjacent face, and that is why the volume mesh fails.(These "free edges" are usually small and hard to find!) The faces should share the same edge but do not. In some cases, I delete the face that appears to be the problem and heal the part to fix the problem.
  • If the surface mesh fails, I start to cut away parts of the model to try to isolate the problem. For example, does the "left" side mesh but the "right" side fail? Then cut the "right" side in half and repeat.

The other thing to check is whether the part file will mesh or not. Sometimes meshing works in the part but not when the part is in the assembly. I suspect it is related to a tolerance based on the overall "size" of the model. The assembly is usually larger than the part itself, so that changes the tolerance. I have not determined if there is anything that can be done to fix this, other than hiding parts or using the Mesh Table.

John

[travis.potier]

Hi John,

Thanks for the response. I will look into updating to 2025 (I'm currently working in 2024), and hopefully the diagnostic tool will help. I have an assembly made up of individual parts (surface contacts). I started opening the parts up in their own window (.ipt instead of .iam) to make modifications to the part. As I'd make modifications I would go into the Nastran environment with the individual part and try to mesh it. I've been able to determine that it is the thread "cutting" that is causing the problem (I went step by step when creating the model and checking the mesh). There's no obvious edges or discontinuities that would cause meshing problems (I've created and analyzed many other similar models that did not have this problem).

I've pushed the limits of my computing power regarding mesh size, so a finer mesh may work, but unfortunately I'd need to much more powerful computer for that.

Thanks,

Travis

[John_Holtz · Accepted solution]

Thanks for the update.

This reminds me of something that most likely applies to your model (threads). I do not know the terminology, so I will use a couple of figures. In Figure 1, a simple cylinder, the curved surface is curved in only one dimension. In Figure 2, a fillet that goes around a curve, the fillet is curved in multiple directions. (A torus is another example but not too common in engineering.) I believe Inventor treats figure 1 as a curved surface and figure 2 as a "spline". Inventor Nastran has problems meshing splines based on my experience. (Not sure if the problems are from Inventor, Nastran, or both.) A thread would be an example of a "spline".

Figure 1: Cylinder is an example of a curved surface about one direction.

Figure 2: A fillet between two sections of a shaft is an example of a curved surface about multiple directions.

What I see is the mesh gets twisted on the spline surface, almost as if the spline has extra curves in it. The surface mesh may be successful, but the volume mesh doesn't know how to fill inside the twisted surface. One way to see such mesh issues is as follows:

• Set the idealization to shell.
• Mesh the part. This meshes the surface. (If the surface mesh fails, there are other problems with the part.)
• Hide the CAD part. This leaves a shaded view of the mesh only without the theoretical CAD surfaces blocking the view.
• Look closely for a mesh that does not looks smooth. The mesh could be more dense in a region which makes it easier to see the problem area.

P.S. My fillet example may be an extreme case. I have not had problems when the geometry is this simple. Something more complex like an airplane wing can be problematic. The outline of the cross-section is a spline, and the extruded spline with a tapered wing creates a more complex spline surface.

By the way, I like the improvements in version 2025, such as being able to delete multiple analyses at a time, and the checkmark on the right-click context menus. It makes me happy. So by all means, update to version 2025 for these reasons. But so far, the half dozen models that I have tried with the mesh troubleshooter has not helped identify the problem. Let me know what success you have with it.

John

[travis.potier]

Hi @John_Holtz John,

I went ahead and updated to 2025. Like you, the troubleshooting found no problems. However, I also deleted all of the chamfers I had in the thread profiles (based on your explanation of Nastran not handling toruses well). That appears to be the issue here. I am now able to generate the mesh. Considering I'm not concerned about the contact stresses of the thread profile, I believe this will work for my purposes. I'll accept your comment as the solution to close this topic out.

Thanks,

Travis