OpenFoam.1.7.x floatingObject tutorial case & MULES:alpha1 greater than 1
Hello,
I have installed the OF.1.7.0 and the new OF1.7.x but I still continues trying to run the floating tutorial case without any success. I always obtain the following error. Anybody know what it is possible that alpha start to increase and produce simulation crash? Interface Courant Number mean: 0.00868469717822 max: 3.07048076829 Courant Number mean: 0.0214761703961 max: 3.07048076829 deltaT = 0.000368438312644 Time = 1.2731 Centre of mass: (0.373595449653 0.351882909424 0.482406400186) Linear velocity: (0.357961120598 0.419740647472 0.322074163028) Angular velocity: (1.07106504184 0.903173170713 0.0110838047329) GAMG: Solving for cellDisplacementx, Initial residual = 0.0056044966347, Final residual = 5.8395571122e06, No Iterations 5 GAMG: Solving for cellDisplacementy, Initial residual = 0.00549399203972, Final residual = 5.71456061284e06, No Iterations 5 GAMG: Solving for cellDisplacementz, Initial residual = 0.00997063228984, Final residual = 3.85256246304e06, No Iterations 6 Execution time for mesh.update() = 1.15 s time step continuity errors : sum local = 3.84344042594e10, global = 2.49126712936e11, cumulative = 0.000105905828067 GAMGPCG: Solving for pcorr, Initial residual = 1, Final residual = 2.81917055336e06, No Iterations 7 time step continuity errors : sum local = 1.08353248665e15, global = 2.55464254723e16, cumulative = 0.000105905828067 MULES: Solving for alpha1 Liquid phase volume fraction = 0.533377598497 Min(alpha1) = 3.16898215629e+294 Max(alpha1) = 2.40723995432 #0 Foam::error::printStack(Foam::Ostream&) in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so" #2 in "/lib/libc.so.6" #3 Foam::fv::gaussGrad<double>::grad(Foam::GeometricF ield<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/home/aml/OpenFOAM/OpenFOAM1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam" #4 Foam::fv::gaussGrad<double>::grad(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so" #5 Foam::tmp<Foam::GeometricField<Foam::outerProduct< Foam::Vector<double>, double>::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::grad<double>(Foam::GeometricField<doubl e, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&) in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so" #6 Foam::tmp<Foam::GeometricField<Foam::outerProduct< Foam::Vector<double>, double>::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::grad<double>(Foam::GeometricField<doubl e, Foam::fvPatchField, Foam::volMesh> const&) in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so" #7 Foam::LimitedScheme<double, Foam::vanLeerLimiter<Foam::NVDTVD>, Foam::limitFuncs::magSqr>::limiter(Foam::Geometric Field<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so" #8 Foam::limitedSurfaceInterpolationScheme<double>::w eights(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so" #9 Foam::surfaceInterpolationScheme<double>::interpol ate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libinterfaceProperties.so" #10 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/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so" #11 Foam::fv::gaussConvectionScheme<double>::flux(Foam ::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/aml/OpenFOAM/OpenFOAM1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so" #12 in "/home/aml/OpenFOAM/OpenFOAM1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam" #13 in "/home/aml/OpenFOAM/OpenFOAM1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam" #14 in "/home/aml/OpenFOAM/OpenFOAM1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam" #15 __libc_start_main in "/lib/libc.so.6" #16 in "/home/aml/OpenFOAM/OpenFOAM1.7.x/applications/bin/linux64GccDPOpt/interDyMFoam" Floating point exception I will be very grateful if somebody help me with this error 
My guess:
Interface Courant Number mean: 0.00868469717822 max: 3.07048076829 Courant Number mean: 0.0214761703961 max: 3.07048076829 
Hello,
Yes I know it but I have tried to limit the maxCo to 0.25 but it still continuous with the problem, at certain time (1.27), Co start to increase beyond 0.25 and stop the simulation. I have tried to increase timePrecision but the problem persist, and I don't know what can I do. Best regards, 
This is an issue with the initialization (or lack of it) of the pressure (p_rgh) which imparts an unphysical impulse on the object which then moves further than the meshmotion can cope with. We are reworking this tutorial to initialize the pressure correctly and will push the new version into 1.7.x when it is ready.
H 
ok thank you very much,
I look forward to the update Thank you very much for your wonderful work Angel 
I found the problem and fixed it. Please pull the latest OpenFOAM1.7.x and try it out.
H 
3 Attachment(s)
Hi,
I have just recently downloaded and installed OpenFOAM1.7.x and pulled the latest update, but I am still getting an error very similar to the one described above and at about the same timestep (1.28s). Does the latest floatingObject case need to be downloaded from somewhere particular or is it just included in OF1.7.x updates? Also, out of interest, what was the problem that was resolved with this case? When I look at the solution I get up to 1.2s, following some water getting trapped above the floatingObject (as it resurfaces) there appears to be a shockwave in alpha (starting from this 'trapped' bit of water) through the entire solution volume (attached are 3 screenshots). Is it this shockwave reaching the mesh edge that causes the instability or is it a coincedence that's when my solution fails to converge? Woops! henry  I just realised your post was dated last night so it's likely that my OF1.7.x is out of date  I read the 'march' bit of your join date and thought it was an old post. Will get the update and let you know how I get on. 
Did you recompile after downloading?
H 
Have now pulled the latest version and recompiled and run the case without any problems. Many thanks for all the work you must've put into this. Out of interest what was 'wrong' with the old case that was causing the instability?
 Khalid. 
Many thanks,
Now i can run the tutorial example without any problem. Best regards 
Quote:
I'm also interested in the problem with the pressure and also how to make it work. I had no problems with running the mentioned tutorial (I have OF 1.7.1) but when using another floating object I see a sudden rise of Min(alpha1) from somewhere 1E5 to 1E+295 in one iteration. The Courant number is normal and slightly higher than the maximum given value in the ControlDict. Making this limit larger doesn't result in a converged result. Another remarkable thing is that the angular velocity along the yaxis is becoming bigger. Tweaking the CoG result in a smaller velocity but the code explodes at the same timestep with the same sudden rise of Min(alpha1) as above. Anyone any suggestions how to solve this problem? FYI: I'm trying to model the sinkage and trim of a boat. Cheers, Ralph 
has anyone figured out what was the problem and how was solutioned?? I have almost the same... after a certain number of timesteps, alpha1 becomes much greater than 1, so courant number increase and simulation stops...

To Ralph/All,
I noticed the same behavior on a hull set only to heave (the constraint moment goes through the roof) and alpha goes well above 1, time steps start shrinking while the courant number goes up and the simulation goes from perfectly normal to floating point error in two time steps of increasingly small size. It always occurs at the same time despite numerous attempts to make the solvers more robust. I am also using 1.7.1 and the simulation works fine without mesh motion. Regards, Dave 
I know I am couple of years late, but did anyone find solution to this problem?

Greetings Hrushi,
The latest talk I know of this topic is at this thread: http://www.cfdonline.com/Forums/ope...tutorial.html You can jump to the post #9 on that thread, if you want a very quick summary. Best regards, Bruno 
Hello, Hrushi!
Did you manage to solve the problem? I have read all the threads about this, but all my attempts to get a good converged solution failed. So I still wonder if someone was cleverer than me and found smth special) Regards, Olga 
Hi Olga,
I am still trying. I tried doing it manually. I tried using alpha1=alpha1>1?(1:(alpha1<0?0:alpha1)); But I am running into some logical model error now, unable to verify if this actually works. You can try and let me know. Thanks Hrushi 
Hi Hrushi!
This seems to be a kind of ignoring problems inside solving alpha1 equation or somewhere around.(anyway, I tried to use this, but got no results) As I understand, alpha1 equation is solved by MULES, but can't find how. And are there any other shemes that can be used here? Regards, Olga 
Hi Olga,
I tried using shorter time step and it worked for me. I converted MULES equation into solve equation but I found the same result. Then I reduced the timestep, now I get max alpha1 as 1. I think you can try it in your problem too. Regards, Hrushi 
All times are GMT 4. The time now is 04:20. 