ANSYS Meshing Issue - How To Mesh Complicated Geometry (~80,000 Faces)?
 

I am attempting to mesh a complicated design (~80,000 faces) for a microchannel heat sink, as pictured, and I would appreciate some advice. I have tried a range of different mesh controls (especially face sizing and body sizing), mesh settings and element sizes, and all have failed to produce a working mesh. The most common errors are shown in the attached picture, in particular the one regarding "The following surfaces cannot be meshed with acceptable quality. Try using a different element size or virtual topology." However, I have already reduced the element size to 2x10^-6 m, which takes two days to resolve before failure.


Unfortunately I cannot alter the geometry significantly, as it is imported from generation in SolidWORKS as either a STEP or an x.t file. As such, any advice for how I can successfully mesh the geometry for CFD analysis in FLUENT would be greatly appreciated.


I can provide more details or the geometry file itself if required.


Thanks in advance.

Hi Sam,

It's a bit difficult to get a sens of the geometry, but I would use Spaceclaim to edit the .step file. As it's a direct modeller you can directly edit geometries without the need to reverse engineer them.

So I would start with cleaning-up unnecessary geometrical details, and also run through some of the repair tools in Spaceclaim (gaps, duplicated edges, etc...).

Then I would play around with the mesh parameters.

Have fun ;)

Thank you for your response. Please find attached some images that might better visualise the geometry. The design is a 15mm long microchannel with two large "hills" or "rolls" that make up the major features. The shape was defined via topology optimisation in COMSOL, then a solid body was generated in SolidWORKS. I am hoping to use FLUENT to simulate a fluid passing over this geometry.

I have attempted to use the Repair tools (especially Repair Faces) in Design Modeller, as well as the Merge function, and they have either not solved the meshing issue or failed outright. I will try to repeat the process in SpaceClaim, though I am less familiar with that program. I'll let you know if it works or not.

Best regards.

Unfortunately, I have now attempted to use SpaceClaim to simplify the geometry, without success. In particular, when I try to use options such as Small Faces, the program crashes.

Do you have any other advice on how to simplify the model without significantly altering the design?

Thanks again.

Hi Sam,

In design modeller it will be way more complicated than in SpaceClaim. I'm thinking of two approaches. First you can play around with the repair tools. In your case as it appears that you have a lot of small faces you could also imprint different "regions" of your model and use the split face first and then regroup several faces using merge tool / repair tools. If your model is too large for your hardware resources it could be that the small faces repair tool crashes. If I remember correctly you can limit the number of faces to correct at once to help SpaceClaim to progressively repair / smooth your model.


Second option which I think would be more straight forward is to directly import the .stl file from the Comsol optimization and use the facette smooth tab in Spaceclaim. This will avoid initial processing in Solidworks before sending the geometry to SpaceClaim. Once you're happy with the smoothing you can then transform the facetted geometry to solid > rbm on the geometry > convert to solid > merge faces.

Have fun ;)

Thank you for your suggestions - this ended up being the solution. I eventually solved the issue by importing the original mesh generated by COMSOL into SpaceClaim, then employing both the "Smooth" and "Reduce Faces" tools in tandem to simplify the geometry, before finally using SolidWORKS to turn the smoothed mesh into a solid body. This body retained many of the same features as the original, but was much less complex, having two orders of magnitude fewer faces. In turn, this permitted both meshing and heat transfer analysis in FLUENT.

Thanks again for your assistance,
Sam