[knalldi]

I try to simulate an small Object with a certain speed crashing into water. For this problem I mesh a .stl object into a small 1x1x2mm domain filled with 3/4 water and 1/4 air where the object starts its journey. The simulation is aborted when the mesh exceeds a certain amount of max skewness. This is how the first run looks like when its aborted due to skewness :

After a short remeshing and mapping of the Domain the mesh looks like this:


After remeshing the information of the solidBody is copied and the simulation restarted. Here is where following error occurs.

Create time

Create mesh for time = 2.6e-05

Selecting dynamicFvMesh dynamicMotionSolverFvMesh
Selecting motion solver: displacementLaplacian
Selecting motion diffusion: inverseDistance
Reading field p_rgh

Reading field alpha1

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar

Reading g
Calculating field g.h


PIMPLE: Operating solver in PISO mode

time step continuity errors : sum local = 5.30289168164e-08, global = -1.3992586985e-09, cumulative = -1.3992586985e-09
GAMGPCG: Solving for pcorr, Initial residual = 1, Final residual = 6.14812798455e-06, No Iterations 7
time step continuity errors : sum local = 3.26028567482e-13, global = -3.61267749522e-14, cumulative = -1.39929482527e-09
Courant Number mean: 1.12667262724e-06 max: 0.000467558744663

Starting time loop

Interface Courant Number mean: 1.31070161191e-07 max: 0.000280808963944
Courant Number mean: 1.12655997124e-06 max: 0.000467511993463
deltaT = 1.19976004799e-10
Time = 2.600011998e-05

Skewness = 0.997089357123

Centre of mass: (0.000499999983277 0.000499999993449 0.00049003915428)
Linear velocity: (-4.49427041303e-06 -2.08718626458e-06 -9.9930235812)
Angular velocity: (-6.28014492619e-13 1.77778371316e-12 -1.01698680087e-12)
DICPCG: Solving for cellDisplacementx, Initial residual = 1, Final residual = 0.0431477016736, No Iterations 6
DICPCG: Solving for cellDisplacementy, Initial residual = 1, Final residual = 0.0431477016736, No Iterations 6
DICPCG: Solving for cellDisplacementz, Initial residual = 1, Final residual = 0.0431477016736, No Iterations 6
Execution time for mesh.update() = 1.26 s
time step continuity errors : sum local = 3.90302363497e-13, global = -4.32488654546e-14, cumulative = -1.39933807414e-09
GAMGPCG: Solving for pcorr, Initial residual = 1, Final residual = 2.71383892696e-06, No Iterations 8
time step continuity errors : sum local = 0.00781073811174, global = -1.19171409414e-09, cumulative = -2.59105216828e-09
MULES: Solving for alpha1
Phase-1 volume fraction = -8.97767166817e+280 Min(alpha1) = -3.11246990095e+284 Max(alpha1) = 3.97785319942e+282
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/libc.so.6"
#3 Foam::PhiScheme<double, Foam::interfaceCompressionLimiter>::limiter(Foam:: GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/lib/libinterfaceProperties.so"
#4 Foam::limitedSurfaceInterpolationScheme<double>::w eights(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5 Foam::surfaceInterpolationScheme<double>::interpol ate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#6 Foam::fv::gaussConvectionScheme<double>::interpola te(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7 Foam::fv::gaussConvectionScheme<double>::flux(Foam ::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8
in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
#9
in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
#10
in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
#11 __libc_start_main in "/lib/libc.so.6"
#12
in "/home/knalldi/myFOAM/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
Floating point exception

I am not quite sure why it has says it has such a high skewness ( I abort old simulation at 0.7) and why the timestep is not e-10 out of the controlDict entry. I tired several matrix solvers and I am really clueless why alpha explodes. Anyone any hint son what i can try to makes this run?

[danvica]

Hi Waldemar,
Can you upload your case ?

[knalldi]

http://depositfiles.com/files/u5kz10e56
Here it is. its already meshed, but I deleted the files of the run in Casefirst. When you run the second case with interDyMFoam you get said error. I typically stop the run at skewness 0.7 , start a remesh with the topology and run the rest in a second, respective third etc case. I hope someone can help me. Stuck with this problem for too long now

[maxof]

Hi Waldemar,
I got similar error messages. In my simulation, I did moveMesh and then run interDyMFoam on the moved/deformed mesh. It has been a bit trial and error, but what I figured out is that setting initialOrientation in the pointdisplacementDict is somehow screwing up things. In an earlier post, (http://www.cfd-online.com/Forums/ope...mapfields.html) I said that this is the way to go, but somehow that was not the final answer to this problem. Try your case without initialOrientation (and maybe w/o initialCentreOfMass).
Honestly, I dont know why you need to state the initial* and whats the purpose of it. If anyone can bring some light into this issue, please let us know!
Let me know how you go.
Cheers, Max

[knalldi]

Hallo Max,
I honestly did not think about this entry, I just copied the whole one. But it works like a charm now when I delete those 2 initialentries.
Greetings, a very thankful Waldemar

[Olam]

Originally Posted by knalldi

http://depositfiles.com/files/u5kz10e56
Here it is. its already meshed, but I deleted the files of the run in Casefirst. When you run the second case with interDyMFoam you get said error. I typically stop the run at skewness 0.7 , start a remesh with the topology and run the rest in a second, respective third etc case. I hope someone can help me. Stuck with this problem for too long now

Hi Waldemar,

I'm sorry to bother you about a case you ran almost three years ago, but I find myself in a rather similar situation to yours (an interDyMFoam sixDoF simulation which needs remeshing every once in a while to keep the skewness to reasonable levels). I Have tried a whole variety of remeshing options (dynamicTopoFvMesh, dynamicRefineFvMesh, etc...) But none seemed to work for me. Hence I have a few questions about your solution to this problem.

I was wondering how you managed to stop your simulation, remesh it and continue running it in a separate case.

Did you stop the simulation manually? Or did you modify the solver to do it for you?

Also how did you perform your remeshing and mapping of the topology once you had stopped your simulation? What tools did you use?

I was also wondering what modifications you had to do to the case to run it again once the remeshing had been done.

Finally, i was wondering if maybe you could re-upload your case (as the link seems to be broken) as I hope it might hold some of the answers to my questions.

I'm sorry to harass you with questions like this on an old case, and hope you still remember it enough to help me.

Thank you for your consideration.
Malo