CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

interDyMFoam- Floating point exception Error

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   December 5, 2012, 07:46
Default interDyMFoam- Floating point exception Error
  #1
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi All,
for simulating my case using with interDymFoam solver I just changed the mesh of sloshingTank2D case, I attached my case here. ( please do blockMesh before starting).
before running the case I initialized the velocity by running the case with potentialFoam solver.

but when I want to start the run with interDyMFoam I get the below strange error.


Create time

Create mesh for time = 0

Selecting dynamicFvMesh solidBodyMotionFvMesh
Selecting solid-body motion function SDA
Applying solid body motion to entire mesh
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 = 2.85057e-06, global = 7.14331e-23, cumulative = 7.14331e-23
GAMGPCG: Solving for pcorr, Initial residual = 1, Final residual = 2.78369e-08, No Iterations 1
time step continuity errors : sum local = 1.51316e-07, global = -1.36584e-23, cumulative = 5.77747e-23
Courant Number mean: 1.35576e-06 max: 1.55603e-05

Starting time loop

Interface Courant Number mean: 0 max: 0
Courant Number mean: 1.32918e-06 max: 1.52551e-05
deltaT = 0.00116279
Time = 0.00116279

solidBodyMotionFunctions::SDA::transformation(): Time = 0.00116279 transformation: ((0 0 0) (1 (0.000363523 0 0)))
Execution time for mesh.update() = 0.01 s
MULES: Solving for alpha1
Phase-1 volume fraction = 0.0790278 Min(alpha1) = 0 Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.0790278 Min(alpha1) = -2.86237e-29 Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.0790278 Min(alpha1) = -1.71602e-28 Max(alpha1) = 1
GAMG: Solving for p_rgh, Initial residual = 1, Final residual = 0.00420348, No Iterations 2
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::inv(Foam::Field<Foam::SymmTensor<double> >&, Foam::UList<Foam::SymmTensor<double> > const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
#5
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
#6
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
#7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interDyMFoam"
Floating point exception


could anybody explain the reason?
Regards,
Marhamat
Attached Files
File Type: gz boxSolidOscillation.tar.gz (34.8 KB, 11 views)
marhamat is offline   Reply With Quote

Old   December 24, 2012, 09:49
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Marhamat,

All I could figure out was:
  • The gravity is wrongly oriented. It's set on the Z axis, when it should be on the Y axis.
  • The "setFieldsDict" should have this:
    Code:
    box ( -0.5 -5 -5 ) ( 0.5 5 5 );
    The only difference is the last 5 was a 0.
I'd suggest you check the "multiphase/interDyMFoam/ras/testTubeMixer" tutorial for ideas as well.

Another suggestion is to do gradual modifications of the original case. From the attached case, it looks like you've tried to do all modifications in a single go, which for someone not experienced with OpenFOAM this is simply a bad idea

I think you should do the steps somewhat like this (also know as divide-and-conquer):
  1. Change the form of the original geometry, but only the outer shell. Preserve the scale, mesh resolution and "setFieldsDict", so that you don't trigger other problems.
  2. Run with this new shape and check if anything needs to be calibrated, such as the initial step and so on.
  3. After this is dominated, add the hole in the middle and run with the new geometry. Calibrate as necessary.
  4. Change the "setFieldsDict" to the ones you want. Run with the new initial field. Calibrate as necessary.
  5. You can now try initializing with potentialFoam or any other application and run again... but I don't think it's necessary.
  6. Once all of the above have been dominated, change the scale of the geometry to the size you need. Changing mesh resolution might be necessary at this point...
After you've done these steps, it'll be easier to help you! And if you share the steps in between, it will make it easier easier!

Best regards,
Bruno
marhamat likes this.
wyldckat is online now   Reply With Quote

Old   December 26, 2012, 14:40
Default
  #3
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hi Bruno
Perfect reply.Tanks a lot for devoting time to my problem.

Regards & merry Christmas,
Marhamat
marhamat is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Compile calcMassFlowC aurore OpenFOAM Programming & Development 12 March 18, 2014 05:22
OpenFOAM on MinGW crosscompiler hosted on Linux allenzhao OpenFOAM Installation 127 January 30, 2009 20:08
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50
Compiling problems with hello worldC fw407 OpenFOAM Installation 21 January 6, 2008 18:38
Gmsh and samplesurface touf Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 December 10, 2007 03:27


All times are GMT -4. The time now is 15:05.