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

an sigFpe error on Turbulence

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   May 29, 2013, 16:10
Default
  #21
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
yes.it should be for that reason.
could you please have a look into the main case also?
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   May 29, 2013, 16:28
Default
  #22
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Uhm... I have the case running in serial (sequential mode) for over 600 seconds already and it hasn't crashed yet.

At which time step is it meant to crash?
wyldckat is offline   Reply With Quote

Old   May 29, 2013, 16:41
Default
  #23
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
this simple case doesn't crash,although the values of turbulence variales increase constantly.which value is suitable to be used in internal field and enterance?are the current values proper?
And crashing occurs in the case with groovyBC.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   May 29, 2013, 17:48
Default
  #24
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Ehsan,

As tired as I am, I'm trying to figure out what to suggest. This is unfortunately waaaay beyond my level of experience.

From what I can figure out, "omega" shoots up to very high values at the walls, due to the sudden pressure/mass flow intake. I think that injecting higher values of k-omega won't affect the results... the pressure difference is simply too high. Either that, or the initial pressure is already too high inside the domain, leading "omega" to increase so much!?

OK, there are several layers of complexity at work here and you'll have to isolate one at a time:
  1. Pressure: it's too high at the inlet. Start the simulation with a very small difference in pressure intake. Examine how things simulate.
    • Use atmospheric pressure levels as reference, instead of using the high pressure levels right away.
  2. As you gradually increase pressure, you should begin to notice two effects:
    1. The mesh resolution starts to seem insufficient (if it was coarse to begin with).
    2. k-omega or k-epsilon start to become less functional.
    The mesh should be adapted, if it seems to need to be. And perhaps looking for other turbulence models would be a good idea, if these models start to loose their effectiveness.
  3. And as I said in the past in other threads: you need simple cases where you can analytically calculate what the end result should be. I think you've already found several papers/thesis that should be able to give you some examples.
  4. Pressure driven simulations can be harder to simulate. Sometimes it's easier to first do some approximate tests by injecting speed, rather than pressure. This strategy can help figure out if there is something wrong with the chosen pressure boundary conditions... or at least, this usually works on incompressible cases.

And that's pretty much all I can figure out to suggest

Good luck!
Bruno
wyldckat is offline   Reply With Quote

Old   May 29, 2013, 18:19
Default
  #25
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
thanks Bruno for your time and effort
Did you do tests on simple case with constant entrance height?
Please have a look into the case with groovyBC to see wich values are appropriate.
Feel free to change turbulence and other values to make it work.
you have a more well ordered way to investigate things than me.
Thanks
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   April 19, 2014, 00:06
Default
  #26
Member
 
Lucas Mutti
Join Date: Aug 2013
Posts: 47
Rep Power: 4
lramutti is on a distinguished road
Hi Bruno,

At the moment I have no zero parameters in my boundary conditions nor initial conditions. I am trying to implement the SST k-omega solver for the conjugate heat transfer problem and I get this error which I don't quite understand. I was able to get the case working for a k-epsilon; however, for some strange reason when I change the solver and add values for kappat, nut, and omega the solver crashes. I was wondering if you could please help me understand what is this message exactly saying. Where is the equation being divided by zero and what is causing it?

Cheers!

Code:
Selecting turbulence model type RASModel
Selecting RAS turbulence model kOmegaSST
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#5  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#6  Foam::compressible::RASModels::kOmegaSST::F2() const in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#7  Foam::compressible::RASModels::kOmegaSST::F23() const in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#8  Foam::compressible::RASModels::kOmegaSST::kOmegaSST(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#9  Foam::compressible::RASModel::adddictionaryConstructorToTable<Foam::compressible::RASModels::kOmegaSST>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#10  Foam::compressible::RASModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#11  Foam::compressible::turbulenceModel::addturbulenceModelConstructorToTable<Foam::compressible::RASModel>::NewturbulenceModel(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#12  Foam::compressible::turbulenceModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so"
#13  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#14  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
Floating point exception (core dumped)

Last edited by wyldckat; April 19, 2014 at 06:52. Reason: Added [CODE][/CODE]
lramutti is offline   Reply With Quote

Old   April 19, 2014, 00:32
Default
  #27
Member
 
CFDUser
Join Date: Mar 2014
Posts: 55
Rep Power: 4
CFDUser_ is on a distinguished road
Dear Lucas,

I guess there is something wrong with your mesh.
Please run below code and post the result.
Code:
checkMesh -allGeometry -allTopology
Regards,
CFDUser_

Last edited by wyldckat; April 19, 2014 at 07:59. Reason: removed quote to a post that had been removed, as it was a duplicate question
CFDUser_ is offline   Reply With Quote

Old   April 19, 2014, 07:01
Default
  #28
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Lucas,

Quote:
Originally Posted by lramutti View Post
Where is the equation being divided by zero and what is causing it?
Code:
#6  Foam::compressible::RASModels::kOmegaSST::F2() const in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
As shown above, the problem is in the method "F2()": https://github.com/OpenFOAM/OpenFOAM...OmegaSST.C#L72
To know better which exact division is giving the problem, you would have to build the Debug version: http://openfoamwiki.net/index.php/HowTo_debugging

But my guess is that the new fields you've added, there were some that you initialized with 0, which as stated in post #2, is wrong.

Best regards,
Bruno

PS: Please wrap code output with the "[CODE]" markers, as explained in my signature link: Posting code and output with [CODE]
immortality likes this.
wyldckat is offline   Reply With Quote

Old   April 20, 2014, 18:53
Default
  #29
Member
 
Lucas Mutti
Join Date: Aug 2013
Posts: 47
Rep Power: 4
lramutti is on a distinguished road
Hey Bruno,

Thanks for the help! I got it working. The F2() parameter depends on the inverse of the velocity field. Initially I left it set as (0 0 0) but I made a minor change and it worked. Sorry about the code, I was not aware about the link you posted. Thanks for letting me know!

Cheers!
immortality likes this.
lramutti 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
Question on Turbulence Intensity Eric FLUENT 1 March 7, 2012 05:30
Turbulence postprocessing Mohsin FLUENT 0 September 19, 2011 21:05
Discussion: Reason of Turbulence!! Wen Long Main CFD Forum 3 May 15, 2009 09:52
Code release: Flow Transition and Turbulence Chaoqun Liu Main CFD Forum 0 September 26, 2008 17:15


All times are GMT -4. The time now is 07:09.