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

XiFoam simulation error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 11, 2013, 15:50
Default XiFoam simulation error
  #1
New Member
 
Efstratios Mavrogiannis
Join Date: Dec 2012
Posts: 20
Rep Power: 4
raysark is on a distinguished road
Hi everyone,

I am trying to run a simulation in XiFoam with an object from snappyHexMesh.

After running blockMesh, snappyHexMesh -overwrite and XiFoam in time step 0.00158 I get this error.

Code:
#0  Foam::error::printStack(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::sqrt(Foam::Field<double>&, Foam::UList<double> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  
 at XiFoam.C:0
#5  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/XiFoam"
#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/XiFoam"
Floating point exception(core dumped)
Paraview runs normally the simulation until 0.0015 where of course stops.
I suspect that somewhere XiFoam divides with 0 as it is a common problem with Floating Point error.

I would really appreciate any help that you could provide as this will help progress my dissertation.

The following link has the case file
https://www.dropbox.com/sh/ou5inoou5ie42rx/JYshJ8DMlg
Please take a look.

Thank you
Stratos
raysark is offline   Reply With Quote

Old   March 11, 2013, 19:07
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,503
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Stratos,

That error message is indicating that a square root has gone very wrong

But you could have posted what truly lead to this crash:
Code:
Courant Number mean: 0.016017 max: 8.74872
Time = 0.00158

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG:  Solving for Ux, Initial residual = 0.0333502, Final residual = 0.00140485, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.0460333, Final residual = 0.00297582, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 0.0450505, Final residual = 0.00291196, No Iterations 2
StCorr = 1
Max St-Courant Number = 0.0022791
Igniting cell 22118 state : 0.442633 1.31785 0.431142 9.95666
DILUPBiCG:  Solving for b, Initial residual = 0.00147667, Final residual = 7.13629e-08, No Iterations 1
min(b) = 0.441463
DILUPBiCG:  Solving for Xi, Initial residual = 0.00251158, Final residual = 3.12975e-05, No Iterations 1
max(Xi) = 1.51737
max(XiEq) = 5.24266
Combustion progress = 0.00442978%
DILUPBiCG:  Solving for hu, Initial residual = 0.115582, Final residual = 0.00124521, No Iterations 3
DILUPBiCG:  Solving for h, Initial residual = 0.118145, Final residual = 0.00128932, No Iterations 3
--> FOAM Warning : 
    From function janafThermo<EquationOfState>::limit(const scalar T) const
    in file /home/user/OpenFOAM/OpenFOAM-2.1.x/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 108
    attempt to use janafThermo<EquationOfState> out of temperature range 200 -> 5000;  T = 5.78718
The first warning sign is that the Courant number is really high:
Code:
Courant Number mean: 0.016017 max: 8.74872
After changing in "system/controlDict" the entry "adjustTimeStep" to "yes" instead of "no", it seemed to be more stable, at least when it comes to the Courant number...
although, around "Time=0.001523", it dropped "deltaT" to "9.26622e-12", making it rather impractical to simulate.

Oh, and the "sqrt" problem was due to the temperature being out of range and leading to one of the calculations after that to use bad values.


After taking a look at the geometry, I suggest the following:
  • Do a simpler mesh, using a parallelepiped shaped object, meshed solely with blockMesh. I say this because the mesh you've got is far from perfect, specially for combustion
  • So it would be best that you first sort out how to perform a good combustion simulation and only after that should you work on having a good mesh for your desired case.
  • Because if you still can't do a good combustion case with mesh created with only blockMesh, then upgrade to OpenFOAM 2.2.x, because it has got better combustion solvers (or at least it should), as well as a better meshing capabilities in snappyHexMesh.
Good luck! Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   March 11, 2013, 19:28
Default
  #3
New Member
 
Efstratios Mavrogiannis
Join Date: Dec 2012
Posts: 20
Rep Power: 4
raysark is on a distinguished road
Hi Bruno,

Thanks a lot for the comments.

I know the simulation wasn't good as I started working with XiFoam this Friday and this was a first trial but I wanted to see what was wrong.

Do you have any suggestions for mesh in combustion? Actually at the end I want simulate a transition from subsonic combustion to supersonic combustion (detonation).

Thanks again.
Stratos
raysark is offline   Reply With Quote

Old   March 13, 2013, 14:32
Default
  #4
New Member
 
Efstratios Mavrogiannis
Join Date: Dec 2012
Posts: 20
Rep Power: 4
raysark is on a distinguished road
Hey Bruno,

I changed the geometry a bit and the endTime of the simulation.

I left the mesh coarse as I want to run very quick simulations and I dont want to spend time waiting (I am not looking for results at this stage).

From paraView I can see the movement of the gas and the combustion which seems quite logical but after a certain time the temperature reaches weird numbers. I uploaded this case on the link above. Could you tell me what's the problem with the temperatures?

PS: Do you know anyone that could set up an accurate combustion with good mesh in case I need it? (with a payment of course for his time)

Thanks a lot
Stratos
raysark is offline   Reply With Quote

Old   March 18, 2013, 18:02
Default
  #5
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,503
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Stratos,

I'm really short for time. Only around the 28th will I be able to try and look into this .

As for someone to help you, right now I can only remember the freelancers forum: http://www.cfd-online.com/Forums/cfd-freelancers/
Now that I think a bit more about it... you can also try contacting Tobi: http://www.cfd-online.com/Forums/members/tobi.html

Best regards,
Bruno
wyldckat 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
Problem running perturbUCyl sen.1986 OpenFOAM 14 March 23, 2012 05:12
Saving ParaFoam views and case sail OpenFOAM Paraview & paraFoam 9 November 25, 2011 16:46
UDF: DEFINE_CG_MOTION for vertical jump motion of an electrode! alban Fluent UDF and Scheme Programming 2 June 8, 2010 18:54
groovyBC sega OpenFOAM Running, Solving & CFD 12 February 17, 2010 10:30
POSDAT problem piotka STAR-CD 4 June 12, 2009 08:43


All times are GMT -4. The time now is 14:52.