[mega1]

Dear Yann,

After running surfaceCheck this is what it gives;

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Reading surface from "constant/triSurface/geom90degarc.stl" ...

Statistics:
Triangles : 0
Vertices : 0
Bounding Box : (1.79769e+307 1.79769e+307 1.79769e+307) (-1.79769e+307 -1.79769e+307 -1.79769e+307)

Region Size
------ ----


Surface has no illegal triangles.

Triangle quality (equilateral=1, collapsed=0):
0 .. 0.05 : #0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 ? in "/opt/openfoam9/platforms/linux64GccDPInt32Opt/bin/surfaceCheck"
#4 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#5 ? in "/opt/openfoam9/platforms/linux64GccDPInt32Opt/bin/surfaceCheck"
Floating point exception (core dumped)

-----------------------------------------------------------------------
I don't understand what it is.

[Yann]

It seems there is something going on with your STL.
What software did you use to create it?
Is it binary or ASCII? If it's binary, maybe try to export it in ASCII format and try again.

Yann

[mega1]

Originally Posted by Yann

It seems there is something going on with your STL.
What software did you use to create it?
Is it binary or ASCII? If it's binary, maybe try to export it in ASCII format and try again.

Yann

Dear Yann,
Yes I think so. I made the geometry with the blockMesh file, then imported it through Paraview in .pvd format and then changed the extension to .stl. I think it's not the right way. Is there any other way to do the .stl file? Are we supposed to use solid edge only to do the .stl?

Thanks a lot!

[Yann]

You can create the geometry in any CAD software and then export the geometry as STL. You should be able to do this with Solid Edge indeed.

If you want to create a STL from blockMesh, you should load it into paraView, then use the "extract surface" filter to extract only the mesh boundaries and then file/save data/ and choose stl format. But this is quite an unusual and tedious process.

Yann

[mega1]

Okay, I will try this way. Thank you very much Yann for your help!

[mega1]

Dear Yann,

I made the geometry with AutoCAD and imported it into OpenFoam as .stl file. Finally it gives me the shape of the porous zone which I needed but the geometry isn't perfect when opened in paraview. Any suggestions how I could improve the geometry? Thank you.

[Yann]

Hi Megan,

Could you also display your STL file on the screenshot so we can see what is wrong?

Also please note topoSet does not modify the mesh, it only assigns some cells or faces to different zones/patches, etc... The expected result is to get a porousBlockage cellZone made out of all the cells contained inside the volume of the STL file.

Yann

[mega1]

Hello Yann,
Attached is the screenshot of stl file.

[Yann]

OK then since your STL file seems to be fine, something must be going on with topoSetDict.

Could you post your whole case here? It would be easier to debug if I can have a look at the file and run few tests.

Yann

[mega1]

Hello Yann,

I have attached the blockMeshDict and topoSetDict files here. Thanks again!

[Yann]

Thanks, but can you send your whole case in a zip file? I cannot test anything without the STL file and I have to rebuild a case around your files if I want to be able to test it.

[mega1]

Hello Yann, sorry about that. I have attached the zip file here.

[Yann]

Thank you!

I changed 2 parameters in the topoSetDict:

• outsidePoints: it's not a good idea to use the origin as an outside point. Better using any coordinate located inside the domain but outside the STL volume and not on any patch.
• nearDistance: I deactivated this parameter by setting it to "-1" since it does not seem appropriate for your case. It allows topoSet to select cells located at a certain distance of the surface and it is used in combination with the curvature parameter (some additional information in this thread: how surfaceToCell works?). I think this was the the main reason for your issue.

    // porousBlockage
    {
        name    porousBlockageCellSet;
        type    cellSet;
        action  new;
        source  surfaceToCell;
        sourceInfo
        {
			file	"constant/triSurface/Drawing4.stl";
			
			outsidePoints
			(
				(0.011 0.011 17.551) 
			);
        
			includeCut  true;
			includeInside  false;
			includeOutside  false;
			nearDistance	-1;
			curvature	1;
			
			// Optional entries
    			useSurfaceOrientation false;
    			fileType        stl;
    			scale           1.0;
		}
    }

This seems to have solved the issue and to give a proper cellZone.
Let me know if this is the result your were expecting!

Cheers,
Yann

[mega1]

Hello Yann,
This is exactly what I needed. I can't thank you enough for your timely help!! God bless you!

[farzadmech]

After two years, I came up with the same problem and I encounter something which I forgot to mention. You should put your stl file in the main directory alongside 0, constant and system.


Thanks,
Farzad

Originally Posted by farzadmech

Dear Yann and friends
My problem is solved. For outsidePoint (X Y Z), just go to constant/polyMesh and open the points file, and choose a point which is outside of the stl file. The second figure shows the imported stl file to my meshed geometry.


Thanks,
Farzad

[farzadmech]

Just one thing to remember, we need to name the generated cellSet using below red command;

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(

{
        name    seeedCellSet;   // 
        type    cellSet;
        action  new;               
        source  surfaceToCell; 

        sourceInfo
        {     
	      file  "seed3Space.stl"; 
        outsidePoints   ((-0.05 -0.05 -0.0494));    // definition of outside
        includeCut      true; //false;              // cells cut by surface
        includeInside   false; //false;              // cells not on outside of surf
        includeOutside  false;              // cells on outside of surf
        nearDistance    -1;                 // cells with centre near surf   //(set to -1 if not used)
        curvature       -100;  //0.9;                // cells within nearDi
   	                  
        }
	}
	
    {
        name    seeed;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set seeedCellSet;
        }
    }
////////////

 
 );
// ************************************************************************* //
// ************************************************************************* //
// ************************************************************************* //

Which gives below attached result and works for porous media without aby problem.

Thanks,
Farzad

Originally Posted by farzadmech

After two years, I came up with the same problem and I encounter something which I forgot to mention. You should put your stl file in the main directory alongside 0, constant and system.


Thanks,
Farzad