[yambanshee]

Good day!


I am trying to make use of map fields to map a corse mesh onto a finer mesh. While within the directory of the finer mesh, I run the command

mapFields -consistent ../corse

however I get an error message as follows:

Source time: 30000
Target time: 30000
Create meshes

Source mesh size: 877765    Target mesh size: 4381120

--> FOAM Warning : 
    From function Foam::triFace Foam::tetIndices::faceTriIs(const Foam::polyMesh&) const
    in file meshes/polyMesh/polyMeshTetDecomposition/tetIndicesI.H at line 75
    No base point for face 354002, 4(30691 131004 131005 30692), produces a valid tet decomposition.

This is printed 100 times with different points followed by

Consistently creating and mapping fields for time 30000

    interpolating p
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigSegv::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  ? at ??:?
#4  ? at ??:?
#5  ? at ??:?
#6  ? at ??:?
#7  ? at ??:?
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  ? at ??:?

before crashing. The two meshes are identical domains with the the only difference being the cell count. Both meshes are hex made with blockMesh, and their checkmesh outputs are attached bellow. I would greatly appreciate a response!


Regards

[clapointe]

As far as I know, the consistent flag expects the two cases to be identical. I am not sure how identical it expects them to be (does this include mesh size?). Have you tried without it?

Caelan

[lebc]

Which version of OF are you using?

I had issues with mapFields some time ago and I found out that the version I compiled had a bug that was corrected right after the release, I fixed it and it worked!

I can share with you the command I use, I have the same domain, but different mesh sizes.

Best Regards,
Luis

[Loekatoni]

Dear Luis,


Could you share the command? I'm having the same problem as OP and possibly your command will also fix my problem.


Sincerely,
Loek

[lebc]

Hi Loek,


The issue I had was in the file calculateMeshToMesh0Addressing.C, in the path /src/sampling/meshToMesh0, line 159.


It was like this:

            if (fromPatch.empty())
            {
                WarningInFunction
                    << "Source patch " << fromPatch.name()
                    << " has no faces. Not performing mapping for it."
                    << endl;
                boundaryAddressing_[patchi] = -1;

After the fix, it is like this:

            if (fromPatch.empty())
            {
                WarningInFunction
                    << "Source patch " << fromPatch.name()
                    << " has no faces. Not performing mapping for it."
                    << endl;
                boundaryAddressing_[patchi].setSize(toPatch.size());
                boundaryAddressing_[patchi] = -1;

Check this file, if it is not like the second code I put here, this is your issue, you will have to make this again. I can help you if you don know how to do it, just don't do it in the original OF installation folder.


In case your file is correct, go to your target folder and run the command:

mapFields path/to/source -sourceTime latestTime -parallelSource -parallelTarget -consistent >map_log

If you are not running a parallel case, just remove the options parallellSource and parallelTarget. If you don want to save a log file, remove >map_log


You may need to create some dummy files in the target folder, give it a try and tell me if it doesn't work.


Best Regards,
Luis

[Loekatoni]

Dear Luis,


Thanks for your quick reply. I checked the file and the line you added was already there. So I will need to look for another fix.


Thanks for the help.


Best regards,
Loek

[lebc]

Hi,

Have you tried the command I suggested you? Did it give you the same result?

BR,
Luis

[Loekatoni]

Hi Luis,


I have tried it and I also already responded to your message thanks for the interest.


Sincerely,
Loek

[yambanshee]

I am using openFoam 5 and I need to make use of the consistent flag, as my two meshes are the same domain with only a different cell count: which is what the consistent flag deals with.


What fixed my problem was to make use of the utility mapFieldsPar, which works the exact same as the normal mapFields utility, but with some extra functionality and less instability.

[calf.Z]

Originally Posted by lebc

Hi,

Have you tried the command I suggested you? Did it give you the same result?

BR,
Luis

Hi,

I use the command mapFields path / to / source -sourceTime latestTime -parallelSource -parallelTarget -consistent and it's running without errors.

But I cannot see any changes in my target case. These fields should be mapped into the target case, but I did not see it. When I run it , the error is :cannot find file "/home/dyfluid/OpenFOAM/dyfluid5.x/run/cavity_mapfieldtest/processor0/0.5/p"

Thank you.

[lebc]

You have to create the folders corresponding to the time step you are mapping on each target processor folder, and you also need to create a dummy file for each field you are mapping.


What you can do is copy the fields from time 0 to a folder with the latestTimeStep in each processor.