[dglee]

Hi guys,

I was looking for the way to set the VOF initial position by using a certain shape (closed volume of STL file).
Finally I was able to do that.
Since I was not able to find this way from web searching, I write this thread here. Just prepare your stl file and set your setFieldsDict file with "surfaceToCell" optioin.


/*--------------------------------*- C++ -*---------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 4 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*--------------------------------------------------------------------------*/

FoamFile
{
version 4.1;
format ascii;
class dictionary;
object setFieldsDict;
location "system";
}
defaultFieldValues
(
volScalarFieldValue alpha.secPhase 0
);
regions
(
// Select based on surface
surfaceToCell
{
file "sphere.stl";
outsidePoints ((-1 -0.8 -0.5)); // definition of outside
includeCut false; // cells cut by surface
includeInside yes; // cells not on outside of surf
includeOutside no; // cells on outside of surf
nearDistance -1; // cells with centre near surf
curvature 0.9; // cells within nearDistance
fieldValues
(
volScalarFieldValue alpha.secPhase 1
);
}
);

[JFM]

Hi Dongguk Lee

I appreciate you providing this post I have been looking for this type of approach for a period of time. I have taken your approach and tried to apply it to my particular case, however I am recieving the following error message:

Create time

Create mesh for time = 0

Reading setFieldsDict

Setting field default values
    Setting internal values of volScalarField alpha.water

Setting field region values


--> FOAM FATAL ERROR: 
Cannnot read "test_1.stl"

    From function bool Foam::triSurface::read(const Foam::fileName&, const Foam::word&, bool)
    in file triSurface/triSurface.C at line 360.

FOAM exiting

The code I have used in the setFieldsDict is:

defaultFieldValues
(
    volScalarFieldValue alpha.water 0
);

regions    // Select based on surface
(
      surfaceToCell
    //     https://www.cfd-online.com/Forums/openfoam-solving/189582-vof-initialization-stl-file-closed-volume.html
    {
        file                     "test_1.stl";
        outsidePoints            ((3.02858 1.94427 83.2));    // definition of volume outside
        includeCut                false;                        // cells cut by surface
        includeInside            yes;                        // include cells inside surface
        includeOutside            no;                            // exclude cells outside surface
        useSurfaceOrientation    true;                        // use surface normals
        nearDistance            -0.01;                        // cells with centre near surface
        curvature                0.9;                        // cells within nearDistance
        
        fieldValues
        (
            volScalarFieldValue alpha.water 1
        );
    }
);

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

I have also attached a copy of the STL file I am hoping to use to set the initial phase conditions. This STL includes a volume of the alpha (water) phase and has been snapped to the external boundary vertices (inlet/outlet/wall patches) with the exception of the top surface which is set at the desired water surface elevation within the model domain.

I have checked the db/dictionary (surfaceToCells) and the layout of the function and what you have provided appears to be fine so i guess the issue relates to the STL itself.

Any assistance guidance will be appreciated.

Regards
JFM

[dglee]

Hi JFM,

I tried with your "test_1.stl" file and it works fine.
Could you please try again, but please locate the "test_1.stl" file in your project directory. not inside of 0 or constant or system.

[Adyk]

I know, this is an old thread, but maybe you read it anyway. This is exactly the same problem I struggle with:


Here is the error message

--> FOAM FATAL ERROR: 
Cannot read "1.stl"

    From function bool Foam::triSurface::read(const Foam::fileName&, const Foam::word&, bool)
    in file triSurface/triSurface.C at line 304.

FOAM exiting

and this is my setFieldsDict

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
    volScalarFieldValue alpha.water 0
    volVectorFieldValue U (0 0 0)
);

regions
(

    surfaceToCell
    {
        file "1.stl";
        outsidePoints ((1 1 0.01)); // definition of outside
        includeCut false; // cells cut by surface
        includeInside yes; // cells not on outside of surf
        includeOutside no; // cells on outside of surf
        nearDistance -1; // cells with centre near surf
        curvature 0.9; // cells within nearDistance

        fieldValues
        (
            volScalarFieldValue alpha.water 1
            volVectorFieldValue U (0 0 0)
        ); 
    }

);

Well, i don't really understand the "outsidePoints ((x y z)); // definition of outside" , how do i define them? which values of my shape define the outside? Probably that's my problem..

I attached the stl file.

Hope you can help me!

[ybapat]

Hello,


Outside point is point outside the stl and inside the geometry. Also I recommend you rename you file to start with string instead of 1. You need to keep the file in project directory or provide full path.



Regards,
-Yogesh

[Adyk]

Thanks for your reply! Finally I got it. But there's another problem.. This is for my bachelor thesis, so it would be great, to get it work.
Okay, I'll rename it.
Does it matter, where this outside point is? And how can I define the position of the stl in my Mesh?

At the moment, I don't see the phase in ParaView. When I look at p_rgh or U I can see something (don't know what it is exactly, but something happens). But the shape itself is not visible (see attached files)
I also did the volume rendering, but there is nothing..

Does "surfaceToCell" give me the phase at all? Or is it just for U, p etc?

[ybapat]

Hello,


Outside points is just any point outside the closed STL in which you want to patch the phase. surfaceToCell can be used to patch any scalar, vector etc. field.



Regards,
-Yogesh

[ybapat]

Outside points is just any point outside the closed STL in which you want to patch the phase and inside the mesh