[LaszloBarta]

Hello,

I am looking for procedures to check mass and more importantly heat balance on my cases. Radiation included. Is there a utility for this? Im using openfoam 3.0.0 package.

Thanx, laszlo

To be more specific: I have an inlet boundary with fixedvalue velocity and temperature condition. i am using the DO method for radiation heat transfer. I am looking for a special boundary condition which sets the radiation heatflux to zero at the input. Anyone has an idea?
Thanx laszlo

[hcl734]

Did you made any progress on this?
Which solver are you using?

[LaszloBarta]

Hi, I was able to resolve mass balance with using paraFoam calculations. It lookes fine. But, regarding energy closure, I was not able to solve my problem. Which was : if I have an inlet boundary condition with high temperature inflow (Like 2000 K) the radiation through this inlet boundary is just too high, and I was not able to set this zero. This problem is related to high temperature flame entering a combustion chamber. Will work on this further. Laszlo

[hcl734]

You can also measure mass flow using functionObject

MassFlowInlet
{
      type            faceSource;
      functionObjectLibs ("libfieldFunctionObjects.so");
      enabled         true;
      outputControl   timeStep;
      writeInterval   1;
      valueOutput     false;
      log             true;
      patch YOURPATCHNAME;
      source     patch;
      sourceName $patch;
      fields (phi);
      operation sum;
      region    YOURREGION;
}

But for heat balance with radiation I am clueless

[LaszloBarta]

Hi, this is great, I will try this. I have not used functionObject yet, but I suppose the function must be put into the controlDict file...
Regarding radiation heat flow this is what I do: in paraFoam I select all the boundary patches and use the "integrate variables" comand, and in the spreadsheet data one can find the Qr summed over all boundaries. This is fine, however at inlets I am not sure how the radiation heat flux is calculated. At wall boundaries I have constant wall temperature condition and inward radiation is calculated based on this. But at inlets, since it is open to exterior space, I am not sure how the radiation heat flux is calculated. I guess some exterior temperature must be set with some emissivity value. So basically, due to this problem, the heat balance is not closed. In Fluent, there was an inlet boundary condition where I could set the exterior temperature. Thanks for the reply! Laszlo

[hcl734]

The use is described here
http://cfd.direct/openfoam/user-guide/function-objects/

Some examples for functionObjects

    energyAbsorbedSOLID
    {
        type patchExpression;
        outputControlMode timeStep;
        outputInterval 1;
        accumulations (
            sum
        );
        patches (".*");
        region YOURREGION;
        variables ("kvar=YOURHEATCONDUCTIVITY;"
                   );
    expression "kvar*(snGrad(T))*area()";
        verbose true;
    }

   energyInlet
   {
        type patchExpression;
        outputControlMode timeStep;
        outputInterval 1;
        accumulations (
            sum
        );
        patches ("YOURINLETPATCH");
        region YOURREGION;
    variables (
                   );
    expression "(YOURHEATCAPACITY*T*phi";
        verbose true;
     
  }

Give us some feedback when you got further

[LaszloBarta]

Hi, Thanks for your suggestions! The "type faceSource" works allright, but I could not manage to get massflux on two different patches, only one patch worked for me. I am not sure how to include multiple patches. I have two input patches, acctually.
The "type patchExpreesion" didnot work, a fatal error was returned saying "Unknown function type patchExpression…".??
Thanks for your reply! Laszlo

[hcl734]

Originally Posted by LaszloBarta

Hi, Thanks for your suggestions! The "type faceSource" works allright, but I could not manage to get massflux on two different patches, only one patch worked for me. I am not sure how to include multiple patches. I have two input patches, acctually.
The "type patchExpreesion" didnot work, a fatal error was returned saying "Unknown function type patchExpression…".??
Thanks for your reply! Laszlo

You got to install swak4Foam and load some additional libraries for using expression based stuff
But swak4Foam is pretty standard when using OpenFOAM so take a look at it
https://openfoamwiki.net/index.php/Contrib/swak4Foam

libs (
      "libOpenFOAM.so"
      "libsimpleSwakFunctionObjects.so"
      "libswakFunctionObjects.so"
      "libgroovyBC.so"
      "libsimpleFunctionObjects.so"
      "libfieldFunctionObjects.so"
     );

If you want to get results for two patches you can just copy the object (my dummy solution, cause I didn't figured out the delimiter notation )