[mykkujinu2201]

Dear all,

Currently, I am trying to solve a case which requires fully developed inlet velocity profile. The inlet has square cross section. In addition, the fluid is non-Newtonian so there is no exact solution for the inlet velocity profile.
I have two options; putting straight channel longer than entrance length or calculating the straight channel separately and mapping the fully developed velocity profile to inlet of the original case.

I know there is "mapFields" utility but that utility maps fields not surface and both cases have overlapped section.
What I want is that mapping the cutting plane (not outlet patch) inside the first case to the inlet of the second case. How can I do this?

Any advice would be helpful.

Thanks.

Jun

[fra76]

Originally Posted by mykkujinu2201

Dear all,

Currently, I am trying to solve a case which requires fully developed inlet velocity profile. The inlet has square cross section. In addition, the fluid is non-Newtonian so there is no exact solution for the inlet velocity profile.
I have two options; putting straight channel longer than entrance length or calculating the straight channel separately and mapping the fully developed velocity profile to inlet of the original case.

I know there is "mapFields" utility but that utility maps fields not surface and both cases have overlapped section.
What I want is that mapping the cutting plane (not outlet patch) inside the first case to the inlet of the second case. How can I do this?

Any advice would be helpful.

Thanks.

Jun

Hi,

For this problem I normally sample a plane in the source case, using foamCase as output format. Then I take the output of sample, place it in constant/boundaryData and apply it to the inlet of the second case, positioned in the same place as the cutting plane, using timeVaryingMappedFixedValue BC.
I am not sure if the sampled data is ready as it is or the files need some little manipulation, but the general process is what is described above.

Hope this helps,
Francesco

[mykkujinu2201]

Dear Francesco,

Thank you for the reply.
Actually, it seems that you gave me the correct solution.
I thought timeVaryngMappedFixedValue BC might be the solution but I doubt whether it is or not. Anyway, I could start to check with your advice though it needs some more as you already said. The sequence is as below.

1. Sample the surface using sampleDict. Export the sampled data in the format "foamFile".
2. Make directory at constant/boundaryData/inlet/0.
3. Among the sampled data, copy "points" to constant/boundaryData/inlet.
4. Among the sampled data, copy field data to constant/boundaryData/inlet/0. in my case, I only need velocity field U so I coppied U from sampled data.
5. Header should be added for "points" and field files. As in pitzDailyExptInlet tutorial, add headers for each files.
6. Set the boundary type to timeVaryingMAppedFixedValue and add "offset (0 0 0); setAverage off;" for vector field or "offset 0; setAverage off;" for scalar field.
7. Run the simulation.

I only checked it for simple 2D channel flow. I will apply this to my case and let you know the result.

Again, thank you so much.

Best regards,
Jun

[mykkujinu2201]

Dear Francesco,

I tested for my case which is about 3D problem.
It works pefectly.

Thank you again.

Best regards,
Jun

[fra76]

Great!

Have fun,
Francesco

[Rotidpor]

I tried the following with the 2106 version.

Originally Posted by mykkujinu2201

1. Sample the surface using sampleDict. Export the sampled data in the format "foamFile".
2. Make directory at constant/boundaryData/inlet/0.
3. Among the sampled data, copy "points" to constant/boundaryData/inlet.
4. Among the sampled data, copy field data to constant/boundaryData/inlet/0. in my case, I only need velocity field U so I coppied U from sampled data.
5. Header should be added for "points" and field files. As in pitzDailyExptInlet tutorial, add headers for each files.
6. Set the boundary type to timeVaryingMAppedFixedValue and add "offset (0 0 0); setAverage off;" for vector field or "offset 0; setAverage off;" for scalar field.
7. Run the simulation.

Well, I have no clue about what is happening, openFoam complains and says this :


--> FOAM FATAL ERROR: (openfoam-2106)
Only 0 provided.
Need at least three non-colinear points to be able to interpolate.

From Foam::coordSystem::cartesian Foam:ointToPointPlanarInterpolation::calcCoordin ateSystem(const pointField&) const
in file triSurface/triSurfaceTools/pointToPointPlanarInterpolation.C at line 57.

FOAM exiting

Has anyone any idea ? I just want to use a boundaryField that I sampled from another case as a fixedValue BC, it shoudn't be that hard... Meshes are different but topologically, the patch is strictly the same...

[shiyu]

Hi Rotidpor, I have just encountered the same problem with version 2206. I am wondering if you have fixed this kind of error.
Thanks.

Originally Posted by Rotidpor

I tried the following with the 2106 version.




Well, I have no clue about what is happening, openFoam complains and says this :


--> FOAM FATAL ERROR: (openfoam-2106)
Only 0 provided.
Need at least three non-colinear points to be able to interpolate.

From Foam::coordSystem::cartesian Foam:ointToPointPlanarInterpolation::calcCoordin ateSystem(const pointField&) const
in file triSurface/triSurfaceTools/pointToPointPlanarInterpolation.C at line 57.

FOAM exiting

Has anyone any idea ? I just want to use a boundaryField that I sampled from another case as a fixedValue BC, it shoudn't be that hard... Meshes are different but topologically, the patch is strictly the same...

[Rotidpor]

Well, it might not be the most elegant way to solve this but anyways...
I solved the issue in my case by using the file faceCenters instead of points. I just follow the procedure written here but I replace "points" by "faceCenters" (also generated by sampleDict) and rename it points.


I don't know what is going on, don't know how it works but it does, at least in my case.