Best Practices for Fluid Domain Extraction and Conformal Meshing of Complex Gyro

[smohse01]

Hello,

I am working on a Conjugate Heat Transfer study of a Gyroid TPMS structure.

I am trying to extract the fluid domain for the Gyroid in SpaceClaim. I exported the Gyroid as a CAD body from nTopology and imported it into SpaceClaim.

In SpaceClaim, I successfully constructed the solid enclosure representing the fluid domain around the Gyroid. However, at the final step, when I try to perform a "Split Body" or "Combine" operation to subtract the Gyroid from the fluid block (to extract the internal fluid volume), the operation fails to execute.

What is the recommended workflow or best practice in SpaceClaim to perform a Split/Combine operation on such mathematically complex, highly curved solid CAD bodies?

Thank you!

[NickFL]

Have you looked into Fluent Meshing? There you can import the STL directly and then use the mesh (or remesh the STL surface) when creating your fluid domain. Plus it has the ability to ignore small holes that often appear when working with STLs.

[smohse01]

Thanks for the tip! Actually, I tried exactly that. I imported the overlapping bodies into Fluent Meshing and used Share Topology to do the subtract at the mesh level.

While it successfully generated a mesh, it created a huge mess in the solver. The fluid domain got split into multiple fragmented cell zones, and the boundaries got sliced into hundreds of tiny face zones. Setting up the periodic BCs on those fragmented faces became an absolute nightmare.

That's why I feel like the only clean way to do this is to find a way to get the CAD-level subtraction working in SpaceClaim first, before bringing it into the mesher.

[Rob]

And there's also Synopsys Simpleware, but that may not be on the Campus system. 

 

[smohse01]

Thanks! Unfortunately our university doesn't have a license for Simpleware.

[Rob]

Yet... 

As a comment and following Nick's idea. Using volume extract means working at the full volume level. If you go into Fluent Meshing and cap the "holes" to form the fluid region you can class the solid as "dead" for meshing. One of the problems with gyroid type geometries is that they're very organic and often break traditional CAD which then form pockets and isolated regions. If you take the solid surface with caps as opposed to a "solid" fluid region there's less to go wrong. 

[smohse01]

Thanks for the suggestion!

I will try importing surface-only geometry to bypass the CAD-level Boolean issues. However, since my study is Conjugate Heat Transfer I have a follow-up question:

Does importing surface-only geometry (where the fluid and solid domains are separated by the shell) reliably support CHT simulations? Specifically, will the interface generated between the solid Gyroid (Solid Zone) and the surrounding fluid (Fluid Zone) be robust enough to handle the thermal gradient (Coupled condition) correctly?

I am concerned that if the interface is not 'solid-to-solid' or 'solid-to-fluid' via a clean volumetric interface, the heat conduction across the copper-water boundary might suffer. Is the 'Wrap' or 'Share Topology' approach on surface bodies considered standard practice for thermal validation in high-performance heat sink simulations?

[Rob]

The face you have or create IS the surface between the fluid & solid assuming the mesh is conformal. Whether that surface is what you started with due to wrapping tolerance or geometry corruption is a different question. Fluent uses the mesh surface to define the shapes, and then the cell resolution to calculate the gradients. 

 

You could have the surface in exactly the correct position but a very coarse mesh. The CFD result won't be overly accurate but the geometry is correct.

Equally, the surface may not be in quite the right place but the mesh is well refined to capture the gradients. The CFD result will be computationally/numerically accurate but may not agree with physical testing. 

[smohse01]

Thank you for the clarification. To summarize my current situation: I am attempting to generate a clean, watertight Fluid Domain in SpaceClaim by either subtracting the Gyroid from a box or using Volume Extract. However, both operations consistently fail due to the geometric complexity of the TPMS lattice, leading to kernel crashes or generic intersection errors.

Specifically, I have attempted the following in SpaceClaim:

1. Direct Boolean Subtract/Combine: Fails due to 'unable to intersect' or kernel crashes.

2. Volume Extract with capped surfaces: Fails with 'all ends have not been capped' even when using overlapping/oversized boundary surfaces.

3. Imprint & Split: While the imprint succeeds in creating curves on the box, the subsequent 'Split Body' operation fails, preventing the extraction of the fluid volume.

I am aware that I could import separate bodies into Fluent Meshing, but as I mentioned, my previous attempts resulted in fragmented face zones, which made setting up robust periodic Boundary Conditions extremely difficult.

Given that my goal is a Conformal Mesh with a clean, periodic-ready interface for CHT:

1. Is there a specific 'repair' or 'simplification' workflow in SpaceClaim that makes these TPMS geometries compatible with Boolean kernels?

2. Or, if CAD-level Boolean is inherently unreliable for this specific geometry, what is the 'gold standard' workflow in Ansys to achieve a watertight fluid-solid interface without creating thousands of disconnected face zones during the Share Topology process?

Any guidance on the exact meshing workflow that preserves periodicity while maintaining a robust thermal interface would be greatly appreciated.

 

[Rob]

Treading carefully as I'm not permitted to use "experience" that's not public knowledge and I wrote the how to on this about 20 years ago! 

Read Fluent's rules on solid zones for periodic boundaries very carefully. It's covered in the User's Guide in Boundary Conditions and Energy/Heat Transfer. Then read the fluid zone rules, noting that you can only have one translational periodic repeat direction. Don't worry too much about conformal meshing - the non-conformal option is often simpler but will need you to switch off one-to-one pairing via the TUI. 

I would look at fixing the stl surface in whatever tool it was generated in, I would also consider remeshing there too. Then look at how the fluid zone will be created. Chances are some of the failures are caused by near tangential contacts or slivers where you've clipped the edge of a solid/fluid part. From there find and cap the fluid zone & mesh. 

Can you share some images? Those may mean Nick and I can advise what to focus on.