[robob]

How to create waterproof stl files with Freecad?
See this thread for guidance how to do it with Salome.
But in Freecad you can't mesh everything and select some mesh parts for the boundaries, or can you?

[Dano62]

I've been creating models in Freecad then exporting them as an STP file to Salome to waterproof them and improve the surface before exporting as STL. So far it's worked fine, even if it's another step.

[robob]

Ok, thanks for mentioning Freecad -> Salome workflow. But I`m interested to do it in Freecad alone. I have read somewhere, that for tighter cfd integration it needs first be implemented by someone. But currently in all cfd workbenches for freecad its not possible, I guess?

[HakikiCanakkaleli]

Hi,

Could you please elaborate what exactly you meant in the following?

Originally Posted by robob

But I`m interested to do it in Freecad alone. I have read somewhere, that for tighter cfd integration it needs first be implemented by someone.

To myself, a CAD program was not expected to produce adequate-quality surface meshes to be utilised in a CFD simulation, because it mainly focuses on providing solutions for improvements of a mechanical design. IMHO, CAD is inherently indifferent to challenges posed by (detailed) flow physics and its modelling.

[robob]

I want to answer my own thread:

these are the links from freecad forum, which explains my problem and which give solutions:

https://forum.freecadweb.org/viewtopic.php?f=37&t=16855
https://forum.freecadweb.org/viewtop...hilit=openfoam

[derekm]

with freecad I create the item with part then call in a python script

             mobjs=[]                
             mobjs.append(this_obj)         #        
             Mesh.export(mobjs,tmp_dir + "/" + str(this_obj.Label)+".ast")                
             del mobjs

separate STL for each region. They appear to be watertight so far. I then use them in snappyHexMesh etc..
The combination of FreeCAD driven by python and snappy works well for me.

[robob]

Hi Derek Mitchell,

how do you mesh your part? Is it one mesh per part or do you mesh surfaces from this part individually? What do you mean by regions in freecad? How do you create mesh regions in freecad?

greets

[derekm]

Originally Posted by robob

Hi Derek Mitchell,

how do you mesh your part? Is it one mesh per part or do you mesh surfaces from this part individually? What do you mean by regions in freecad? How do you create mesh regions in freecad?

greets

regions as in chtMultiRegionSimpleFoam regions
Used it upto 35 regions so far.
The FreeCad is used to create STL files these are used in snappyHexMesh to create the mesh and cellZones. Then splitMeshRegions converts the cellZones into Regions. then changeDictionary fixes up the fields.
When I cut one region from another I get a watertight interface by using the code above.

[robob]

Thanks for your response Derek,

you have explained more the openFOAM side of things...
Do you have multiple parts in Freecad or one single part? Do you make some groups in freecad for naming/selecting the faces and surfaces? How do you export the stl files?

My workflow in the past, which has its problems (not really watertight) was this:
1. Create one part in Freecad
2. extract/group the wanted surfaces from this part in Freecad
3. for each group of the part mesh it -> get multiple mesh files in Freecad
4. export the mesh files to stl

thank again

[derekm]

To create in FreeCAD two regions shell and inside.

Using part create a volume inside another outside.
Cut the inside volume from outside volume. { select inside and outside then part>boolean>cut }
Select the resulting shell and file>export as .ast.
Select the inside volume and file>export as .ast.
Rename the .ast files as .stl.
FreeCAD uses mm, to convert metre scale use surfaceMeshConvert.

[robob]

thanks for answering,
I will try it someday

[robob]

okay,

the method which derekm explained, is probably the same as in Freecad: how to prepare a mesh suitable for OpenFOAM?,
which I think again is not correct because, it is not watertight. Sorry derekm.

The color section approach, specified in the first link of my post #5 https://www.cfd-online.com/Forums/op...tml#post688163
is not very good, because it is not very scriptable, and everytime some geometry is changed in dimension and is new generated you have to set the colors again...

So I search again for another approach and now I have this:
Freecad -> export as step -> import into GMSH -> make physical groups -> mesh with gmsh -> export as default `.msh` file (or similar) -> use openfoams gmshToFoam script -> then use `surfaceMeshTriangulate` to get the stl/obj.

It seems, of course a bit tedious, to generate stl/obj like this. But it has some advantages:

1. you can use freecad
2. you get watertight (combined) stl/obj
3. the exported step file can be changed in dimensions and has same boundary conditions with the gmsh script and its numbering (at least if the same object within freecad is exported and only if this object has no other faces added or removed...)
4. most this works from command line and can be automated
5. you can use gmsh (which is one of the best open source mesher)
6. and, if it is sufficient and snappyhexmesh is not needed, you can directly use the gmsh mesh (because of gmshToFoam)
7. you can visually check/validate the obj files and their groups back in freecad/paraview

I also found out, that there are gmsh groups from from within FEM workbench: https://forum.freecadweb.org/viewtop...19481&start=10
You export this mesh as FEM mesh formats (*.unv, *.med, *.stl, *.dat, *.inp, *.vtk, *.vtu), I guess, which is an "smesh" object. Unfortunately I have not found out, how to get individual stl/obj files from that.