[songyi719]

Even after snappyhexmesh finished successfully, mesh only have result of blockmesh, so it doesn't have any patch of stl file I put in constant folder

When I checked the log, snappyhexmesh finished without error (and several Millions of cell). I used -overwrite, and used 'location inside mesh' properly

What could be other possibility to fail my snappyhexmesh result to written in mesh?

[Yann]

1. Did you run snappy in parallel or serial mode?
2. Did you try slicing your resulting mesh in paraView to see if snappy did something inside the mesh or if it's only the original blockMesh file?

In addition, posting your snappy log might help to spot something.

Yann

[songyi719]

I ran in parallel, and checked paraview, but it was only original file.

[Yann]

Have you reconstructed your mesh, or selected "Decomposed case" in Case Type when loading your case in paraView?

If not, you are probably looking at the initial mesh located in constant/polyMesh rather than the final mesh located in processor*/constant/polyMesh.

2 Solutions:

• If you use paraFoam: run reconstructParMesh -constant before running paraFoam
• If you use paraView or paraFoam -builtin: When opening your case in paraView, pay attention to the "Case Type" parameter, and switch from "Reconstructed case" to "Decomposed case"

[songyi719]

I reconstructed my mesh using reconstructparMesh, and after that I used simpleFoam, but was extraordinary fast with every force being 0 (probably bc patch wasn't overwritten and only blockmesh was left in mesh)
Few weeks ago I ran similar code with different stl file, and it worked fine. So I'm curious if stl file can affect it.

[songyi719]

Also, when I check constant/polyMesh, mesh seems to be properly updated since all files' size have increased significantly. But I can't find out why It isn't used when I decompose again and run simpleFoam parallel

Update) No, it isn't updated. I made a mistake. It is same file size as before

[AtoHM]

I'd recommend starting from a fresh directory and doing only the meshing as a first step and carefully look for the pointers that Yann provided!

[songyi719]

I reduced mesh size and started with fresh directory, and it worked!

Problem is, it shows "expected a ')' while reading binaryblock" error while reconstruction with non-reduced mesh version sim.

But it is different issue, so I will finish this question in the thread with thanks to both of you.

[Yann]

Originally Posted by songyi719

I reconstructed my mesh using reconstructparMesh, and after that I used simpleFoam, but was extraordinary fast with every force being 0 (probably bc patch wasn't overwritten and only blockmesh was left in mesh)
Few weeks ago I ran similar code with different stl file, and it worked fine. So I'm curious if stl file can affect it.

I insist on the reconstructParMesh -constant. If you meshed with snappy using the -overwrite option and then only run reconstructParMesh without the -constant option, reconstructParMesh will run but will not reconstruct anything.
(with OpenFOAM, details matter! )

In addition to AtoHM recommendation: if it worked before with another STL file, make sure your new STL is properly scaled and properly positioned relatively to the blockMesh.

EDIT: I didn't see your last message, glad to know you made it work!