[WhiteW]

Dear all,
I'm using OpenFOAM v2012 on a computer with the Ubuntu 20.04 OS.
Now I also installed it (v2012) on a new computer with a more recent hardware, the new operative system is Ubuntu 21.10.

I'm doing some test to check the performances; however I'm registering different behaviours between the two computers.
The sequece of operations involves:
surfaceFeatureExtract
blockMesh
snappyHexMesh
decomposePar
extrudeMesh
createPatch
potentialFoam
changeDictionary
buoyantBoussinesqSimpleFoam

The resulting meshes are identical, indeed the two checkMesh logs give the same output.
All the logfiles are identical (as expected with different execution times) until the execution of potentialFoam.
The first difference I noticed is in potentialFoam: the Interpolated velocity error is 1.46919e-06 for PC1 and 0.00893802 for PC2

Finaly the buoyantBoussinesqSimpleFoam of PC2 diverges after few iterations, the maximum velocity is very high since iteration 1.
The buoyantBoussinesqSimpleFoam results in PC2 diverges also skipping the potentialFoam.

Why the results are different?
Attached are the potentialFoam and buoyantBoussinesqSimpleFoam log files.
comparison.zip

Thanks!
WhiteW

[WhiteW]

The Problem also appears running the tutorial
heatTransfer/buoyantBoussinesqSimpleFoam/iglooWithFridges

On PC1 everything is ok.
On PC2 the solution diverges after 12 iterations.

I tried also to use the simpleFoam solver on PC2 and the solution runs without problems. It seems something related to the buoyantBoussinesqSimpleFoam solver and the new operative system/hardware...

Any Idea on how to solve it?
Thanks,

WhiteW

[WhiteW]

I can confirm that the problem is the solver buoyantBoussinesqSimpleFoam running in the new Operative System.
I tested both the openFoam versions v2012 and v2112 on both Ubuntu 20.04 and 21.10 versions.
The setting is the same, Im now running the iglooWithFridges tutorial.

These are the results:

of2012 - Ubuntu 20.04 - ok
of2012 - Ubuntu 21.10 - diverge
of2112 - Ubuntu 20.04 - ok
of2112 - Ubuntu 21.10 - diverge

I also tested the diverging configurations with Ubuntu 21.10 in a different hardware. It is not hardware dependent; the problem is the operative system.
I think Ubuntu 21.10 does not support the buoyantBoussinesqSimpleFoam solver, the cases always diverges after 10-15 iterations (continuity is not respected).
Where can I report the bug?

WhiteW

[ffran]

Hi,
Have you ever managed to fix this issue or trace where the different behaviour comes from?


Thank you very much!

[JM92]

Hi,

I found this thread while searching for solutions to a similar problem, so I just want to summarize my solution here for others.

One case showed diverging solutions running a new installation of OFv2106 on a workstation, while it ran perfectly on a Linux server and another workstation.
Similarly, the multiphase/interFoam/RAS/floatingObject tutorial was diverging as well on the new installation.

The core of the problem were the compilers (gcc, g++, gfortran), since I had to change the version from 11 to 9 to compile waves2Foam on Ubuntu 22.04 (Compilation on Ubuntu 22.04).
I installed OFv2106 using the pre-compiled package initially. I could imagine that the difference between the default compilers of the OS (which the pre-compiled package depends on) and the actual compilers currently activated on my OS led to the problems.
Hence, switching back to the default compilers could be a solution which might work. However, I have not tested this.

I was able to solve this by not using the pre-compiled Ubuntu/Debian package, but compiling OFv2106 myself. The compiled version then fits to the compiler settings of the system and runs without diverging.

Regards,
JM92

[mllokloks]

Originally Posted by WhiteW

I can confirm that the problem is the solver buoyantBoussinesqSimpleFoam running in the new Operative System.
I tested both the openFoam versions v2012 and v2112 on both Ubuntu 20.04 and 21.10 versions.
The setting is the same, Im now running the iglooWithFridges tutorial.

These are the results:

of2012 - Ubuntu 20.04 - ok
of2012 - Ubuntu 21.10 - diverge
of2112 - Ubuntu 20.04 - ok
of2112 - Ubuntu 21.10 - diverge

I also tested the diverging configurations with Ubuntu 21.10 in a different hardware. It is not hardware dependent; the problem is the operative system.
I think Ubuntu 21.10 does not support the buoyantBoussinesqSimpleFoam solver, the cases always diverges after 10-15 iterations (continuity is not respected).
Where can I report the bug?

WhiteW

I got a similar issue. But, interestingly, after switching off snap and addLayers in snappyHexMeshDict, the issue has gone.

[slavaVM]

I have similar problem. After upgrading to Ubuntu 22.04 OF-v2006 gives wrong results. The reason is the incorrect calculation in fvc::reconstruct(). For the same p_rghEqn.flux() field the reconstruction gives utterly "chequerboarded" velocity correction, this spoils the final velocity field. With Ubuntu 18 everything worked.

[slavaVM]

Update: the dot product of a tensor and a vector in the fvc::reconstruct() is calculated incorrectly, the z component gives strange value. The solution is to replace few lines in
OpenFOAM/primitives/Tensor/TensorI.H before operator&(const Tensor<Cmpt>& t, const Vector<Cmpt>& v) (see e.g. OF-v2312).


In this way OF-v2006 is compiled properly with gcc 11 and runs like with the previous version of Ubuntu.