[mmohaqeqf]

hey guys;
I have just started applying the following work flow, but it seems I am missing something because I have had mixed results (successful and unsuccessful):



1. freeCAD: creating geometry and exporting it as a step file.


2. Salome:

2.a) importing the step file in Salome Geometry module, separating the patches (i.e. exploding the faces, e.g. inlet, outlet, wall etc.).

2.b) then, using Salome Mesh module to separately do surface meshing (triangular) on patches using the same mesh properties for all the patches (to make sure the resulting model is watertight).
2.c) export each face (i.e. patch) as a stl file separately.


3. using cat command in bash to make a single stl file out of all the individual stl files.


4. making sure the resulting stl file is closed (i.e. surfaceCheck command).


5. using the resulting stl file as an input to cfMesh.


Like I said, this work flow seems to be working for some of my cases, while not working with others, and I don't know where is it that I am ignorant about.


Take the attached step file (created by freeCAD 0.18) as an example. It is the simplest geometry possible: a converging straight pip; so one circular inlet, one circular outlet and a wall.
I follow the work flow above and the resulting stl file is watertight, but when I try to mesh it with cfMesh I get the following error:


terminate called after throwing an instance of 'char const*'



Just to isolate the issue even further, I used meshmixer to explode the patches and cat them back together: and now cfMesh is happy and easily meshes my geometry. So, I am pretty sure my issue is in the Salome section of my work flow. Now what makes it more confusing is that the above work flow works with some of my models, but not on others.
So I am trying to understand where I get it wrong.

It would be nice if someone could reproduce this work flow using the attached step file and let me know if it is working for them or not.



Thanks


ps: I am aware of the following links, but I just want to see which section of my work flow needs fixing.


https://curiosityfluids.com/2019/02/...-your-meshing/


General workflow to create a flawless mesh in cfMesh

[mmohaqeqf]

Ok, the snappyHexMesh was able to successfully mesh my geometry.
I did remove/uninstall OpenFOAM and re-installed it, but cfMesh is unable to mesh this simple geometry; I just don't know why?

[mmohaqeqf]

So, here is my findings about this work flow so far, which I put here for future reference:


I created a simple 3D circular pipe in freeCAD.
I exported the geometry as three different file types acceptable by Salome: brep, iges and step.
I imported each one of the above file types into Salome, exploded the surfaces, and surface-meshed them and then exported the surfaces individually as separate stl files. I then concatenate them into a single stl file, to be meshed by cfMesh.


1) The final concatenated stl file from the freeCAD's brep file resulted in a watertight geometry and cfMesh could mesh it happily.


2) The final concatenated stl file from the freeCAD's iges file resulted in a non-watertight geometry.


3) The final concatenated stl file from the freeCAD's step file resulted in a watertight geometry, but cfMesh threw out an error and could not mesh it.


So, I think generally it is not a very reliable work flow, as it seems to me that freeCAD and Salome cannot communicate with each other efficiently. I highly recommend making your geometry in Salome itself (I know the GUI is clunky!!) and then either do the entire volume discretization in Salome or surface-mesh it and send it to cfMesh for volume discretization.


However, if you still want to apply this work flow (freeCAD => Salome => cfMesh), I think it is best to export your geometry in brep format from freeCAD.


Hope it helps someone in the future.

[hogglife]

Hi,

Maybe helpful for others bothered by this.

I have tried the geometry your provided in 1st post with Salome and waterproof stl is obtained.

The key is to make conformal mesh at the boundary between two faces as explained below. (In your case, the boundary is the edges where two faces intersect.)

chtMultiRegion not solving for velocity field

Explode the boundary edge from each face. Then create submesh on one with a prescribed mesh size while for the other one uses the "Import 1D Elements from Another Mesh" and points it to the previous edge which already creates submesh on. One note is the previous edge you point to should be the one under "Groups of Edges". If there is not, create it by right-click on the submesh of the previous edge under "SubMeshes on Edge" and choose "Construct Group".

I am not familiar with mesh with Salome too. But the above mesh works for me. Maybe there is more convenient way.