|
[Sponsors] |
April 16, 2012, 06:08 |
pimpleDyMfoam simulation keeps blowing up
|
#1 |
Senior Member
|
Hi all;
I'm running a pimpleDyMFoam simulation and it keeps blowing up. Even reducing the time step down to 1e-5 does not solve the problem. Code:
Courant Number mean: 5.46684e+95 max: 8.98336e+97 Time = 0.02416 solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 0.02416 transformation: ((0 0 0) (0.997121 (0 0 0.075828))) PIMPLE: iteration 1 smoothSolver: Solving for Ux, Initial residual = 0.790411, Final residual = 0.0773137, No Iterations 13 smoothSolver: Solving for Uy, Initial residual = 0.736195, Final residual = 0.0664809, No Iterations 15 GAMG: Solving for p, Initial residual = 0.991861, Final residual = 0.00944463, No Iterations 3 time step continuity errors : sum local = 1.18585e+93, global = -2.66584e+77, cumulative = 1.75555e+77 PIMPLE: iteration 2 smoothSolver: Solving for Ux, Initial residual = 0.763113, Final residual = 0.07555, No Iterations 53 smoothSolver: Solving for Uy, Initial residual = 0.721429, Final residual = 0.0720906, No Iterations 255 GAMG: Solving for p, Initial residual = 0.930911, Final residual = 0.00681328, No Iterations 5 time step continuity errors : sum local = 3.0917e+94, global = 8.06608e+78, cumulative = 8.24164e+78 PIMPLE: iteration 3 DILUPBiCG: Solving for Ux, Initial residual = 0.763528, Final residual = 7.71705e-07, No Iterations 75 DILUPBiCG: Solving for Uy, Initial residual = 0.750098, Final residual = 8.75581e-07, No Iterations 74 GAMG: Solving for p, Initial residual = 0.982765, Final residual = 6.63145e-07, No Iterations 19 time step continuity errors : sum local = 1.39295e+91, global = -2.71812e+80, cumulative = -2.6357e+80 #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libfiniteVolume.so" #5 Foam::fvMatrix<double>::solve() in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libincompressibleRASModels.so" #6 Foam::incompressible::RASModels::kOmegaSST::correct() in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libincompressibleRASModels.so" #7 in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/pimpleDyMFoam" #8 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6" #9 in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/pimpleDyMFoam" Any help would be greatly appreciated. |
|
April 16, 2012, 06:26 |
|
#2 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
Hi
I would suggest doing the following until it stops blowing up. Change to upwind on U. And relax the components by 0.5. If it stops blowing up you can then try to switch to higher order schemes and decrease the relaxation.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
April 16, 2012, 06:32 |
|
#3 |
Senior Member
|
Thank you Linnemann.
Relax the components by 0.5 means that I need this in my fvSolutions: Code:
relaxationFactors { "(U|k|epsilon).*" 1; } About the rest, what do you mean with change to upwind on U and switch to hig order schemes? Thank you again for your help! |
|
April 16, 2012, 06:58 |
|
#4 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
yes
relaxationFactors { "(p|U|k|epsilon).*" 0.5; } in fvSolutions and div(phi,U) Gauss upwind;// in fvSchemes you are using linearUpwind which is a higher order scheme and thus inherently more unstable.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
April 16, 2012, 09:42 |
|
#5 |
Senior Member
|
Thank you linnemann, unfortunately had no luck with your tips…
First of all I increased the time step from 1e-5 to 1e-4 and my simulation blew up at time 0.0266. So I changed this line I had in my fvSolution: Code:
"(U|k|epsilon).*" 1; Code:
"(p|U|k|omega).*" 1; So I changed the line to this: Code:
"(p|U|k|omega).*" 0.5; So I changed these lines in my fvSchemes: Code:
divSchemes { default none; // div(phi,U) Gauss upwind; div(phi,U) Gauss linearUpwind grad(U); div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } Code:
divSchemes { default none; div(phi,U) Gauss upwind; // div(phi,U) Gauss linearUpwind grad(U); div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } At this time I moved back to a time step of 1e-5 to reduce the Courant Number but the simulation blew up at 0.026… What do you think? Thank again. |
|
April 16, 2012, 09:58 |
|
#6 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
Try with transientSimpleDyMFoam
with this fvSolution file.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
April 16, 2012, 10:21 |
|
#7 |
Senior Member
|
Thank you. Do I need to compile it?
|
|
April 16, 2012, 10:25 |
|
#8 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
Yes you have to
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
April 16, 2012, 10:26 |
|
#9 |
Senior Member
|
Thank you!
I'll see what I can do! |
|
April 16, 2012, 10:50 |
|
#10 |
Senior Member
|
By the way, what's the difference between this and the one that comes with openFoam?
|
|
April 16, 2012, 19:08 |
|
#11 |
Senior Member
|
Actually, my geometry is quite a simple one: just a 2D cube… How comes it cannot be solved? I mean, what can you solve with the original pimpleDyMFoam then?
|
|
April 17, 2012, 02:37 |
|
#12 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
Hi
If it is that simple I suggest you upload it so we can have a look at your setup. If its too big to fit here use Dropbox with a public link or a similar file sharing method.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
April 17, 2012, 05:46 |
|
#13 |
Senior Member
|
Thank you linnemann.
Here's my case. Regards |
|
April 17, 2012, 13:03 |
|
#14 |
Member
Jason Eason
Join Date: Jan 2010
Location: Portage, Michigan
Posts: 45
Rep Power: 16 |
Excuse me Linnemann, could you please explain the differences between pimpleDyMFoam and transientSimpleDyMFoam?
__________________
Debian Squeeze - OpenFOAM-2.1.x, Paraview-3.12.0 |
|
April 17, 2012, 16:26 |
|
#15 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Greetings to all!
In case Linnemann doesn't see the question about the differences between the two solvers, here's what I know:
Best regards, Bruno
__________________
|
|
April 17, 2012, 16:49 |
|
#16 |
Senior Member
mauricio
Join Date: Jun 2011
Posts: 172
Rep Power: 18 |
just a thought... you know your running an incompressible solver and your using a reference pressure of 1atm
Code:
pRefPoint (0.1 0.1 -0.005); pRefValue 1e5;
__________________
Best Regards /calim "Elune will grant us the strength" |
|
April 17, 2012, 16:58 |
|
#17 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
Hi lovecraft
Had a look at your case and it looks like you haven't (not to be rude) understood the setup involving rotating stuff. If you follow the tutorial /tutorials/incompressible/pimpleDyMFoam/mixerVesselAMI2D I think you will get a better understanding of the whole setup involving rotating parts. Back to your case. I had to split it up into two meshes and then merge them back together and attach them using AMI's. You cant have a moving mesh where you only have one mesh and a zone. If you want to do it this way you should use the steady MRF approach. Also a lot of your BC's where wrong for such a case. Here is a nice little animation of it running. http://dl.dropbox.com/u/15968063/output.avi and also a link to the case that works. http://dl.dropbox.com/u/15968063/cubo.tar.gz And to follow up on the difference transientSimpleDyMFoam has some hard-coded stuff that makes it more stable, but it should be able to tweak pimpleDyMFoam to have a similar stability.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
April 17, 2012, 18:10 |
|
#18 |
Senior Member
|
Thank you a lot linnemann, that's really great! I'll have a look at the setup tomorrow. Could you also explain me what commands you ran?
Thanks again! |
|
April 17, 2012, 19:07 |
|
#19 |
Senior Member
|
I did some digging around and also looking at the case you uploaded I think I understood this:
1. You need to create an interface between the rotating and the stationary meshes. In my case it was a cylinder. This is the AMI (Arbitrary - btw, why "arbitrary??" - Mesh Interface); 2. You need to mesh the two regions separately, making sure you have the same cell dimensions on the AMI; 3. Merge the two meshes using mergeMesh on the running case and then run it. I'll dig deeply on the propeller tutorial tomorrow. What I did wrong (and I'm sorry for having posted here and on another discussion my wrong conclusions about that…) was that I only set the rotating region as a zone. This is what I usually do for the MRF and, at this point, I hope that at least is correct… Looking forward to try an run it as I'm getting really excited about that! Anyway thanks anybody for you help and sorry for my mistakes… |
|
April 18, 2012, 06:59 |
|
#20 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
@linnemann @lore
http://dl.dropbox.com/u/70019943/roCube.tar.gz Hello linnemann, appreciate your effort on pimpleDyFoam above. plz find my case folder with implementation of rotating cube. * I have only done the meshing of rotor stator inside rocube/Mesh folder. * the next step would be to merge rotor-Mesh and stator-Mesh!!! How to go about it? Note: Still the case is not fully modeled, so most of the BC files are missing. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Solar Radiation in OpenFOAM | plainstyle | OpenFOAM Running, Solving & CFD | 15 | July 8, 2014 05:43 |
Simulation of a complex wing in solidworks flow simulation | niels1900 | FloEFD, FloWorks & FloTHERM | 6 | April 20, 2011 11:44 |
pimpleDyMFoam stability problems | cnsidero | OpenFOAM Running, Solving & CFD | 3 | January 29, 2011 13:36 |
Continuous vs interrupted simulation | sega | OpenFOAM Running, Solving & CFD | 4 | November 3, 2008 15:29 |
strange simulation error | Ralf Schmidt | FLUENT | 2 | May 4, 2007 14:02 |