[sita]

Hi Jon,

Just wondering: did you ever get RBFMeshMotionSolver to work with fsiFoam? I'm trying to use it with solids4foam (foam-extend-4.1, Ubuntu 18.04), and got the same error message you got (Problem with fluid mesh motion solver selection), both for RBFMeshMotionSolver and RBFMotionSolver.

I came across a presentation by Željko Tuković, in which he uses RBFMeshMotionSolver with solids4foam, even combined with overset grid, so apparently it's possible to get it working, but it clearly doesn't work straight out of the box.

Did you find a solution?

Many thanks,
Sita

Originally Posted by jcappola

Hi All,

I'm using the foam-extend 4.0 bazaar to do FSI on flexible airfoils and I am having some trouble with mesh motion. It seems that the fsiFoam solver has only been implemented with RBF point interpolation and while RBFMeshMotionSolver is in the library, fsiFoam refuses to use it when I patch it into the dynamicMeshDict.

After the first time step's solid predictor I get the following error when the cell motion step occurs:

--> FOAM FATAL ERROR: 
Problem with fluid mesh motion solver selection

    From function fluidSolidInterface::moveFluidMesh()
    in file fluidSolidInterface/fluidSolidInterface.C at line 1922.

FOAM aborting

I am wondering if someone has been able to patch in the RBFMeshMotionSolver for fsiFoam and could give some hints on how to move forward as the .moveFluidMesh() call only allows for fe/fv motionSolvers to be used and is hard coded.

Thanks,

Jon

[bigphil]

Hi,

See commit bc08236 to the development branch of solids4foam: I added the following code to fluidSolidInterface.C:

        // Check for RBF motion solver                                                                                    
        const bool rbfMotionSolver =
            isA<RBFMeshMotionSolver>
     	    (
                fluidMesh().lookupObject<motionSolver>("dynamicMeshDict")
            );

	// Set motion on FSI interface                                                                                    
        if (feMotionSolver)
        {
 
...

        }
        else if (rbfMotionSolver)
        {
            // Prepare list of patch motions                                                                              
            Field<vectorField> motion(fluidMesh().boundaryMesh().size());

            // Initialise all fields to zero                                                                              
            forAll(fluidMesh().boundaryMesh(), patchI)
            {
                motion[patchI] = vectorField
	        (
                    fluidMesh().boundaryMesh()[patchI].size(), vector::zero
	        );
            }

     	    // Loop through all FSI interfaces                                                                            
            forAll(fluid().globalPatches(), interfaceI)
            {
		// Interpolate the FSI interface point motion to the faces                                                
		const vectorField interfacePatchMotion =
		    fluidPatchesPointsDispls[interfaceI]
                  - fluidPatchesPointsDisplsPrev[interfaceI];

                // Create interpolator                                                                                    
                primitivePatchInterpolation interp
                (
                    fluidMesh().boundaryMesh()[fluidPatchIndices()[interfaceI]]
                );

                // Set motion of FSI interface                                                                            
                motion[fluidPatchIndices()[interfaceI]] =
                    interp.pointToFaceInterpolate(interfacePatchMotion);
            }

            // Set motion field in RBF motion solver                                                                      
            // Note: take displacement as opposed to velocity                                                             
            const_cast<RBFMeshMotionSolver&>
            (
                fluidMesh().lookupObject<RBFMeshMotionSolver>("dynamicMeshDict")
            ).setMotion(motion);
        }
        else
        {

...

Then constant/fluid/dynamicMeshDict can be set as (for example):

dynamicFvMesh dynamicMotionSolverFvMesh;

solver RBFMeshMotionSolver;

diffusivity quadratic inverseDistance (interface);

// Settings for the RBF solver                                                                                            
staticPatches    (top bottom left);
movingPatches    (interface);
fixedPatches     (inlet outlet);
interpolation
{
    function     TPS;
}
coarsening
{
    enabled      no;
}

I haven't looked into the "best" settings but the beamInCrossFlow/linearGeometryElasticBeam tutorial runs in serial with these settings. I am not sure what the difference between fixed and static patches are. Parallel does not seem to work yet, so I will have to dig further to find out why (feel free to!).

Philip

[sita]

Hi Philip,

Perfect, I'll have a look a that, thanks!

Sita

[sita]

Hi Philip,

Sorry, just a quick question: can I build this development branch version next to the version that I already built from the master branch, or should I replace everything? Or would adding the code you mentioned to my master branch version, and re-building, work as well (i.e. without messing up my git clone)?

Many thanks,
Sita

[bigphil]

Hi Sita,

There are at least three ways you can do this:

1. Use "git checkout development" to change to the development branch, and you can then use "git checkout master" to change back
2. Create a second clone of the entire repo and change this repo to the development branch
3. Copy the code segment into the relevant file in the master branch

All three of these are fine. Personally, I prefer option 1.

Once I have checked all tutorial still run I will merge the change into the master branch anyway.

Philip

[sita]

Hi Philip,

Thanks a lot for your quick reply, I'll go for the first option so.

Sita

[bigphil]

Originally Posted by sita

Hi Philip,

Thanks a lot for your quick reply, I'll go for the first option so.

Sita

No problem. By the way, after changing branch, you can run "git pull" to pull the latest changes from that branch ("git pull" may update all branches if your git settings are configured using the old approach).

[sita]

Hi Philip,

Great, that worked, the error "Problem with fluid mesh motion solver selection" is gone now. Unfortunately a new error popped up:

Time = 0.001, iteration: 1
Modes before clean-up (plate): 0, modes after clean-up (plate): 0
Current fsi under-relaxation factor (plate): 0.05
Maximal accumulated displacement of interface 0: 2.40967e-05
solids4Foam: fluidModels/finiteVolume/RBFMeshMotionSolver/RBFMeshMotionSolver.C:662: virtual void Fo
am::RBFMeshMotionSolver::solve(): Assertion `index == nbGlobalStaticFaceCenters[Pstream::myProcNo()]
' failed.
Aborted (core dumped)

Does this look familiar to you?

I'll try to run this beamInCrossFlow/linearGeometryElasticBeam tutorial first, see if I can work out how things work from there.

Thanks,
Sita


EDIT: Woops, the beamInCrossFlow/linearGeometryElasticBeam tutorial gives me the exact same error...
EDIT 2: Strange, the line of code that failed (the one with Pstream::myProcNo() ) should only be used in a parallel case (if ( Pstream::nProcs() > 1 ) ). I'm fairly sure I'm running the case in serial mode, as I haven't decomposed anything etc.

[bigphil]

Hi Sita,

Are you running the case in serial or in parallel?

As noted in my previous post, parallel is currently not working: there is something wrong in the RBFMeshMotionSolver.

Philip

EDIT: I have checked the linearGeometryElasticBeam case in parallel on my Ubuntu box and it does work. I have realised there is a problem with openmpi on my mac (unrelated to solids4foam).
Can you try clean and re-compile solids4foam (run "wclean lib && wmake libso" in src/solids4FoamModels)? And update to development commit 699223c first, where I included some example RBF settings. You need to enable the RBF motion in linearGeometryElasticBeam tutorial by changing the following lines in the fluid/dynamicMeshDict:

solver velocityLaplacian;
//solver RBFMeshMotionSolver;

to

//solver velocityLaplacian;
solver RBFMeshMotionSolver;

[sita]

Hi Phil,

That's the thing, I actually am running the case in serial (on Ubuntu 18.04, with foam-extend-4.1), so I was really surprised that I got an error related to this "if nProc > 1" block. I already changed the dynamicMeshDict like you suggested in post #483, I'll try the cleaning and re-compiling too, tomorrow. Thanks for your help so far!

Sita

[sita]

Hi Philip,

I just tried cleaning and re-compiling solids4foam, after updating to commit 699223, but I'm still getting the same error. As you wrote that for you the tutorial case now also works in parallel on Ubuntu, I'm starting to think that something might be wrong with my foam-extend-4.1 install (I had a good deal of trouble installing that, see also here (last page), and I'm still not sure whether everything's working as it should now).

For now I'll try installing the pre-built binary of foam-extend-4.1, see if that helps. I read that the pre-built binary has some trouble with parallel cases in combination with the GAMG solver, but in fairness I'd be happy enough with just serial runs by now.

Thanks,
Sita


EDIT: Too bad, with the foam-extend-4.1 pre-built binary it doesn't work either, still the same error...

EDIT 2: Ah wait, sorry, the error isn't in this if-block; I missed a closing parenthesis. Still, can't figure out why exactly it failed; it seems the index in this for-loop (lines 653-660) doesn't reach nbGlobalStaticFaceCenters


EDIT 3: Hm, commenting out those assert commands "solves" my problems for now. The results of the beamInCrossFlow/linearGeometryElasticBeam tutorial look alright, but this is not a permanent solution of course...

[sita]

Hi everyone,

I've two quick questions about solids4foam/RBFMeshMotion (foam-extend-4.1, Ubuntu 18.04.3):

1. Does anyone know how I'm supposed to add gravity to a solids4foam computation with RBFMeshMotion? There's a dictionary g in constant/solid, which works fine with other mesh motion solvers, such as velocityLaplacian, but when I use RBFMeshMotion, gravity seems to be ignored.

Looking through the solver log file, I noticed:

g field not found in constant directory: initialising to zero

but that line is also there when I use velocityLaplacian, and in that case gravity is picked up alright. Just to be sure I copied g into constant, but that didn't have any noticeable effect.

2. Whenever I'm postprocessing solids4foam results in ParaView, it's complaining about duplicated entries:

ERROR: In /build/paraview-lH8wFv/paraview-5.4.1+dfsg3/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 7484
vtkOpenFOAMReaderPrivate (0x555867625480): Error reading line 490 of /home/openfoam/foam/openfoam-4.1/tutorials/solids4foam/fluidSolidInteraction/beamInCrossFlow/overset/elasticBeam/4/solid/D_0_0: Found duplicated entries with keyword value

I'm using a system installed ParaView 5.4, because I didn't manage to get the Third Party version installed. As also the PVFoamReader wouldn't build somehow, I'm using paraFoam -builtin (or just "touch case.foam && paraview case.foam"). Could that be causing these errors?

Thanks in advance,
Sita

[bigphil]

Originally Posted by sita

Hi Philip,

I just tried cleaning and re-compiling solids4foam, after updating to commit 699223, but I'm still getting the same error. As you wrote that for you the tutorial case now also works in parallel on Ubuntu, I'm starting to think that something might be wrong with my foam-extend-4.1 install (I had a good deal of trouble installing that, see also here (last page), and I'm still not sure whether everything's working as it should now).

For now I'll try installing the pre-built binary of foam-extend-4.1, see if that helps. I read that the pre-built binary has some trouble with parallel cases in combination with the GAMG solver, but in fairness I'd be happy enough with just serial runs by now.

Thanks,
Sita


EDIT: Too bad, with the foam-extend-4.1 pre-built binary it doesn't work either, still the same error...

EDIT 2: Ah wait, sorry, the error isn't in this if-block; I missed a closing parenthesis. Still, can't figure out why exactly it failed; it seems the index in this for-loop (lines 653-660) doesn't reach nbGlobalStaticFaceCenters


EDIT 3: Hm, commenting out those assert commands "solves" my problems for now. The results of the beamInCrossFlow/linearGeometryElasticBeam tutorial look alright, but this is not a permanent solution of course...

Glad to made progress.

One other point to mention: I checked this case only with foam-extend-4.0; I did not check foam-extend-4.1. Maybe this may be the reason for the different behaviour. I can check with fe41 too.

Philip

[bigphil]

Originally Posted by sita

Hi everyone,

I've two quick questions about solids4foam/RBFMeshMotion (foam-extend-4.1, Ubuntu 18.04.3):

1. Does anyone know how I'm supposed to add gravity to a solids4foam computation with RBFMeshMotion? There's a dictionary g in constant/solid, which works fine with other mesh motion solvers, such as velocityLaplacian, but when I use RBFMeshMotion, gravity seems to be ignored.

Looking through the solver log file, I noticed:

g field not found in constant directory: initialising to zero

but that line is also there when I use velocityLaplacian, and in that case gravity is picked up alright. Just to be sure I copied g into constant, but that didn't have any noticeable effect.

Some of the solidModel implementations may not include gravity (most do but some may not) so you may need to check for the one you are using. The choice of fluid mesh motion solver "should" not affect solid in any way.

Feel free to upload a small test case here demonstrating the problem.

Originally Posted by sita

2. Whenever I'm postprocessing solids4foam results in ParaView, it's complaining about duplicated entries:

ERROR: In /build/paraview-lH8wFv/paraview-5.4.1+dfsg3/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 7484
vtkOpenFOAMReaderPrivate (0x555867625480): Error reading line 490 of /home/openfoam/foam/openfoam-4.1/tutorials/solids4foam/fluidSolidInteraction/beamInCrossFlow/overset/elasticBeam/4/solid/D_0_0: Found duplicated entries with keyword value

I'm using a system installed ParaView 5.4, because I didn't manage to get the Third Party version installed. As also the PVFoamReader wouldn't build somehow, I'm using paraFoam -builtin (or just "touch case.foam && paraview case.foam"). Could that be causing these errors?

Thanks in advance,
Sita

I also use the ParaView binaries from the ParaView website. This warning can be ignored but I have not looked into what is causing it.

[sita]

Hi Philip,

Thanks for getting back, sorry for the delay on my side. About the RBFMeshMotionSolver: I took another look at the results, and it looks like gravity is indeed included, but the fluid and the solid seem to be decoupled.

I was messing around with the HronTurek tutorial as a testcase, changed the parameters to get the FSI1 case, and later on added gravity. When I use the velocityLaplacian solver, the results look alright (see attached plot, uA.png), but when I change to RBFMeshMotion, the solid seems to be deforming without affecting the flow (see attached image, RBF_seems_decoupled.png, and plot, uA_RBF.png). I'm also attaching my testcase, so if you have time you can take a look. I don't know, it's probably something really silly that I'm missing here, but I haven't found it yet.


And about the ParaView warnings/errors: in my case the variables that cause those errors aren't loaded, I only get pointD0 etc. Is there a way to load these variables anyway?

Many thanks,
Sita

[Flowkersma]

Hi Sita,

Can you try removing the "frontAndBackPlanes" patch from the dynamicMeshDict/staticPatches dictionary?

Best, Mikko

[sita]

Hi Mikko,

Sure, I can give that a try. Do you want me to remove it altogether, or to move it to e.g. fixedPatches? Do you happen to know the difference between staticPatches and fixedPatches, by the way? Is there a reason that removing frontAndBackPlanes from staticPatches should fix the fluid-solid coupling?

I'll let you know how I get on,
Sita


EDIT: Cool, that actually seems to work! Thanks for the tip, can you explain it?

[Flowkersma]

Hi Sita,

To be honest, I do not know what is the difference between a static and a fixed patch. If a patch is either fixed or static then the nodes/cellCenters on that patch are not moving and therefore you were not getting any deformations for the 2D case. If you look at the example dynamicMeshDictionaries by the authors of the mesh deformation library, they seem to be also using both static and fixed patches for the 2D cases:
cylinderFlap_FSI3
beamInCrossFlow2D

Best, Mikko

[sita]

Hi Mikko,

Yeah, I noticed those tutorials, couldn't figure out the difference either though. I still don't quite get how my flexible plate was able to bend straight through the lower wall of my domain, but I'm glad everything is working as it should now.

Thanks again,
Sita

[sita]

Hi everyone,

I seem to be running into the same issue as Mike in post #436: as the deformation in my toy case (HronTurek FSI1 with gravity) is too large to be considered linear, I switched the solidModel in solidProperties from linearGeometryTotalDisplacement to unsNonLinearGeometryTotalLagrangian. This model wouldn't combine with the linearElastic material type in mechanicalProperties (as is indicated in Philip Cardiff's solids4foam training slides, but I tried anyway...), so I switched that to neoHookeanElastic.

And so now I'm getting these warnings

--> FOAM Warning : 
    From function void Foam::neoHookeanElastic::correct(surfaceSymmTensorField& sigma)
    in file materialModels/mechanicalModel/mechanicalLaws/nonLinearGeometryLaws/neoHookeanElastic/neoHookeanElastic.C at line 401
     Material linearity enforced for stability!

indicating that the solver is struggling to converge. And indeed a little while later the simulation crashes. As Philip suggested, I tried under-relaxation of D (and Deqn, and DD, and DDeqn) in system/solid/fvSolution, but so far the warnings keep coming up, and the simulation keeps crashing. Does anyone have any tips to improve things?

Many thanks,
Sita