Abaqus meshing complex geometry

[Quincylin]

Hi,
Im trying to mesh the geometry below with just one type of mesh (i.e. no free mesh). At the moment I have made partial progress by partitioning the instance with some datum planes (as shown by the regions highlighted in yellow, as opposed to orange where mesh cannot be assigned), but I'm still not able to mesh the whole thing. Would be highly grateful if anyone could shed light on how to do it!

 

[FEA way]

If this thread can’t be simplified for the analysis, it won’t be easy to mesh it. But partitions are key to the success. You need a lot more of them (they should divide the geometry into the simplest possible shapes). However in this case partitions may not be enough and you might have to use virtual topology feature. Even if you fail to mesh this part with hexahedral elements, good quality second order tets should give you accurate results as well.

 

[Quincylin]

Thanks for the speedy reply. The reason I want to mesh it with a single mesh type is because I need to import it into Paraview, which requires one configuration file per mesh type and so a single mesh type would be very handy. I've tried virtual topology but still cant figure out a systematic way to mesh the whole structure.

 

[Mustaine3]

I think this part cannot be fully hex meshed. At the start and the end of the thread you'll always have a problem. If you don't want to mix elements, then you have to go with tets.

 

[FEA way]

Try to separate thread segments using partitions. Datum planes aren’t the only option, you can use other techniques such as extend face or extrude/sweep edges as well. If this approach doesn’t work (and that might be the case) then either simplify the thread (Replace faces tool can help) or use tetrahedral elements for the whole part.

 

[Quincylin]

I tried meshing the whole part with tets but the elements in the thread part are severely distorted and the following error pops up:
2751 elements are distorted. Either the isoparametric angles are
out of the suggested limits or the triangular or tetrahedral
quality measure is bad. The elements have been identified in
element set WarnElemDistorted.
Any idea how to resolve it? I also tried to refine the meshes but no luck!

 

[FEA way]

In case of such complex geometry free meshing with tets is not as easy as it could seem. Proper partitioning and virtual topology may be required in this case as well in order to obtain good quality mesh. If you can share your model here then I will take a look at it and try to tell you how to mesh it with tets.

 

[Quincylin]

Here is the step file for the thread part. feel free to import it into the abaqus cae. Thanks!!

 

[FEA way]

Abaqus was able to mesh this part using tets even without any changes. But you can use Virtual Topology —> Combine faces to combine some small faces in order to obtain better quality mesh.

 

[Quincylin]

Some elements are still distorted when I inspect it using 'verify mesh' (highlighted in yellow in the image below), and when I merge the small faces abaqus takes ages to mesh. Do you get the same distortion if you verify the mesh?

 

[FEA way]

It seems that you should reduce the global size. Assigning local seeds may also help.

 

[Quincylin]

may I know the global size of your mesh?

 

[FEA way]

Sure, I used 0.4 for the global size and it seems sufficient.

 

[Quincylin]

Thats what mine looks like with 0.4. There are still 35 distorted elements, wondering if they matter in the analysis?

 

[FEA way]

No need to worry about that. There are pretty much always some elements showing warnings (highlighted in yellow) with default mesh verification settings in Abaqus.

 

[Quincylin]

Thanks so much for the help! But the following error still persists:

*** Error: package.exe / rank 0 / thread 0 encountered a system exception 0xC0000005 (EXCEPTION_ACCESS_VIOLATION)

When I look at the abaqus_acis.log file more closely, I notice the following error, which I suspect might be the reason why abaqus terminates:

*** Warning (spaacis/src:UNITS_NOT_EQUAL)
save units not equal to the restored units

Really not sure how to fix this and there is very limited info online. Would greatly appreciate for any help!

 

[FEA way]

This sounds like a system error, not related to a particular analysis. Try running some simple simulation. Or run your analysis once again with different settings (for example without parallel processing).