[charitonas]

Hi,

I would like to calculate the wallHeatFlux with rhoCentralFoam but i always get an error:
"Trying to construct an genericFvPatchField on patch movingWall of field e"

I am using OpenFoam 2.1.x but i have tried it with newer versions and i couldn't figure it out.

Could anyone help me?

[wyldckat]

Quick answer: Please provide more details. For example, which tutorial case can be used for achieving the same result?
I ask this because I tried "compressible/rhoCentralFoam/forwardStep" and got a completely different error.

[charitonas]

Hi Bruno,

I am trying my own case. A simple lid driven cavity flow.Here is my thermophysical properties.However,the problem arise from the T file and the smoluwskiJump property.I don't know why

[wyldckat]

Hi Chariton,

Still doesn't get me much. Are you certain you're using 2.1.x?
Because I get this error message:

--> FOAM FATAL ERROR: 
Not implemented

    From function basicThermo::h()
    in file basicThermo/basicThermo.C at line 260.

FOAM aborting

My guess is that you have modified thermodynamics library.

Either way, try adding this line to your "system/controlDict":

libs ("librhoCentralFoam.so");

it should load the library that has that boundary condition.

Note: if you already have the "libs" entry, then keep in mind it's a list, e.g.:

libs (
"librhoCentralFoam.so"
"libOpenFOAM.so"
);

Best regards,
Bruno

[charitonas]

Hi Bruno,

I did modified the library.I am now moved to Openfoam 2.2.2. My problem is that if i include the rhoCentralFoam in the libraries i will not get any error at all. However, when i try to view the results, the wallHeatFlux is always 0. Similar problem can be found on the post below.

http://www.cfd-online.com/Forums/ope...heat-flux.html

I followed these instructions. The wallHeatFlux can work. My main questions-mentios are:

1)If i turn to OpenFoam 2.1.x i will get errors or not?
2)If i choose fixedValue in 0/T everything its ok.

A friend of mine suggested me the below:

snGrad(T) = grad(T) & n

n is normal vector that you need to define it.

But i don't know how to define the n normal vector. Could you help me defining that?

Thanks
Chariton

[wyldckat]

Quick answer:

• Without a test case, the best I can suggest is that you edit the source code for your "wallHeatFlux" utility and comment out this line:
  

  if (isA<wallFvPatch>(mesh.boundary()[patchi]))

  This line is what is enforcing that only walls can be used for calculating the heat flux.
• As for your other question, I think you're trying to calculate something similar to "wallGradU", therefore, check the source code for it:

  echo $FOAM_UTILITIES/postProcessing/wall/wallGradU/wallGradU.C

  There you'll see that "snGrad" should be accessible from the T field directly.

[charitonas]

Hi Bruno,
I have checked what you suggested me and i commented out that line but without any results. I have attached the test case if this can help

[charitonas]

Hi Bruno,

I am attaching also the wallHeatFlux

[wyldckat]

Hi Chariton,

Sorry, but only today did I finally managed to look into this.
I've tested the case "kn0.005" that you provided in post #7 and I was able to get results by doing the following steps:

1. I've used OpenFOAM 2.2.2 and I didn't make any changes to wallHeatFlux.
2. I ran the following commands:
   

   blockMesh
   rhoCentralFoam

3. While the solver was still running (takes a while to run the whole case), I then edited the file "system/controlDict" and added the following line:
   

   libs ("librhoCentralFoam.so");

4. Still while the solver was still running, I ran:
   

   wallHeatFlux

5. And it did give me results, such as:
   

   Time = 6.425e-08
   Selecting thermodynamics package 
   {
       type            hePsiThermo;
       mixture         pureMixture;
       transport       sutherland;
       thermo          hConst;
       equationOfState perfectGas;
       specie          specie;
       energy          sensibleInternalEnergy;
   }
   
   Reading/calculating face flux field phi
   
   Selecting turbulence model type laminar
   
   Wall heat fluxes [W]
   movingWall -9.86075e-07
   fixedWalls -2.44182e-07

edit: I went back and re-read your posts. So the problem was in visualizing the results. That's because you have to load the patches in ParaView, instead of the internal mesh, as shown in the attached image.

Best regards,
Bruno

[charitonas]

Hi Bruno,

Thank you for your reply and for your time. I figure it out by editing the code and now its ok. However, i will try your suggestion as well.