[choist31]

Dear All,

I am developing the two submerged heater rods model by modifying the tutorials; chtMultiRegionTwoPhaseEulerFoam.

When I try to add one more heater by duplicating the geometry and thermal properties from existing example, I faced the following error message:

--> FOAM FATAL ERROR:
Cannot find file "points" in directory "water/polyMesh" in times "0" down to constant

I have updated many input parameters as a result of newly added heater rod model. For your clear understanding, please see the attached file ; current working model.

Your any comments on my errors would be great helpful for me like OpenFOam beginner.

Best wishes,

Sung

[korenml]

Originally Posted by choist31

Dear All,

I am developing the two submerged heater rods model by modifying the tutorials; chtMultiRegionTwoPhaseEulerFoam.

When I try to add one more heater by duplicating the geometry and thermal properties from existing example, I faced the following error message:

--> FOAM FATAL ERROR:
Cannot find file "points" in directory "water/polyMesh" in times "0" down to constant

I have updated many input parameters as a result of newly added heater rod model. For your clear understanding, please see the attached file ; current working model.

Your any comments on my errors would be great helpful for me like OpenFOam beginner.

Best wishes,

Sung

Hi Sung,
I have checked your files and I had to make several changes to work it. I hope it will help you.

First change was in topoSetDict, where you set action new instead of add. The option new replaces previous cellSet.

 // Heater2; added heater   
       {
        name    bottomWaterCellSet;
        type    cellSet;
        action  add; // it adds heat2CellSet to current cell set, instead of replacing it (action new)
        source  cellToCell;
        sourceInfo
        {
            set heater2CellSet;
        }
    }

The second change was for 0.orig/solid2/T where I changed region from solid2 to solid. This specify region (solid or fluid) not the name of the region.

    solid2_to_water
    {
        type            compressible::turbulentTemperatureTwoPhaseRadCoupledMixed;
        value           uniform 400;
        Tnbr            T.liquid;
        kappaMethod     solidThermo;
        region          solid;
        // Name of the other phase in the flid region mixing with 'liquid' phase
        otherPhase      gas;
        qrNbr           none;
        qr              none;
    }

Last mistake was that you forgot to set the boundary condition for water_to_solid2 in /0.orig/water/k.liquid.

    water_to_solid2
    {
        type            kqRWallFunction;
        value           $internalField;
    }

Best,
Tomas

[choist31]

Dear Koreanml

I do appreciate your kind and clear reply on my questions. I have resolved these issues long time ago.
For my project fund issue, I am holding on my CFD work now. Anyway, the ID sounds like you are Korean.
Anyhow, I am so glad to know you like kind and highly level of OpenFOAM user.
As you may know, since I can't get a prompt response through this thread, I also get some help from commercial company.
If you don't mind, I would get more comments or advice for any my future work. I sincerely hope to keep in touch with you.

Best Wishes,

Sung Won Choi

[qingqingliu]

How do you solve your issue? I met the same issue with you.

Originally Posted by choist31

Dear Koreanml

I do appreciate your kind and clear reply on my questions. I have resolved these issues long time ago.
For my project fund issue, I am holding on my CFD work now. Anyway, the ID sounds like you are Korean.
Anyhow, I am so glad to know you like kind and highly level of OpenFOAM user.
As you may know, since I can't get a prompt response through this thread, I also get some help from commercial company.
If you don't mind, I would get more comments or advice for any my future work. I sincerely hope to keep in touch with you.

Best Wishes,

Sung Won Choi

[govind_IITD]

Hi,


I am also modifying the quenching case for wall heating boiling problem. I am stuck at fluid-solid interface boundary condition. I am applying const heat flux at the bottom surface of the wall and zero gradient for the sides of wall.


How do I take care of the fluid-solid interface in this case both for gas and liquid ? Initially domain is filled with the water only.




Regards,
Govind