CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM

Foam::error::printStack(Foam::Ostream&) at ??:? ///// pimpleDyMFoam

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

Like Tree7Likes
  • 4 Post By chegdan
  • 2 Post By chegdan
  • 1 Post By j_moulton

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 7, 2016, 08:54
Default Foam::error::printStack(Foam::Ostream&) at ??:? ///// pimpleDyMFoam
  #1
Member
 
bye bye my blue
Join Date: Sep 2016
Posts: 37
Rep Power: 6
bye bye my blue is an unknown quantity at this point
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam:ow3(Foam::Field<double>&, Foam::UList<double> const&) at ??:?
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:ow3<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#5 Foam::RASModels::SpalartAllmaras<Foam::Incompressi bleTurbulenceModel<Foam::transportModel> >::fv1(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const at ??:?
#6 Foam::RASModels::SpalartAllmaras<Foam::Incompressi bleTurbulenceModel<Foam::transportModel> >::correct() at ??:?
#7 ? at ??:?
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9 ? at ??:?
Floating point exception (core dumped)

///////

I don't know how to solve it .....

and I attached B.C , checkMesh output and etc..

please help me ToT

thanks.
Attached Files
File Type: c epsilon.c (1.5 KB, 22 views)
File Type: c k.c (1.5 KB, 10 views)
File Type: c nut.c (1.5 KB, 12 views)
File Type: c nuTilda.c (1.5 KB, 13 views)
File Type: c p.c (1.5 KB, 21 views)
bye bye my blue is offline   Reply With Quote

Old   December 7, 2016, 08:59
Default + other files..
  #2
Member
 
bye bye my blue
Join Date: Sep 2016
Posts: 37
Rep Power: 6
bye bye my blue is an unknown quantity at this point
log.pimpledymfoam has big size, so i modified it
Attached Files
File Type: c log.checkMesh.c (25.5 KB, 15 views)
File Type: c log.pimpleDyMFoam.c (12.2 KB, 16 views)
File Type: c controlDict.c (1.2 KB, 6 views)
File Type: c fvSchemes.c (1.6 KB, 7 views)
File Type: c fvSolution.c (2.8 KB, 9 views)
bye bye my blue is offline   Reply With Quote

Old   December 13, 2016, 19:01
Default
  #3
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 26
chegdan will become famous soon enoughchegdan will become famous soon enough
First of all, this is a very common error (i.e. the divide by zero) and is not necessarily easy to figure out. I did notice that you fix all the values of nuTilda in your simulation so you might want to go back and look through the tutorials or search the forum on how to correctly set the nutilda boundary conditions. As for how to proceed, i would start first with a much simpler strategy. Though your ultimate goal may be a turbulent, transient, dynamic mesh case i would:
  • Start with a steady simulation. Lower the flow rate to a laminar level and turn off turbulence all together to make sure that you have pressure and velocity BCs setup correctly (i have not looked at yours to confirm yet). Use upwind on everything (because it is bounded and first order).
  • Try a higher flow rate (still steady) with turbulence to get your turbulence model BCs setup correctly (still first order schemes)
  • Try a higher flowrate, but transient case with no dynamic mesh to see how the time stepping influences/changes during the simulation (still first order schemes)
  • Try the dynamic mesh case with very conservative settings (ie. if it rotates, make it rotate slow), as this will help you see if your ami (as it rotates) is causing issues (e.g. overlapping faces).
  • Try at a real condition with first order schemes, then try to move to higher order schemes. use function objects and in-situ probes to evaluate your solution as it is running to see if you are within acceptable ranges.
  • Say something nice to your computer or cluster to make it not crash so often.

Overall, start simple and build up. Good luck and I would also look at

How to give enough info to get help

and provide a bit more information next time e.g. a complete zipped case or a link to a dropbox so others can download it and help.
__________________
Dan

Find me on
Twitter @dancombest
LinkedIn
WordPress
chegdan is offline   Reply With Quote

Old   December 14, 2016, 06:24
Default
  #4
Senior Member
 
Join Date: Jan 2014
Posts: 178
Rep Power: 9
hxaxtma is on a distinguished road
Without knowing your case I can just assume what happened, anyway here are some hints

0) Everything what chegdan said

1): Check your BCs for p and U if they are set up properly.
- in your p File you set the pressure for inlet and oulet to 0! Is this by purpose?
Normally you use for U inlet: fixedValue and outlet zeroGradient and for pressure inlet zeroGrdianet and outlet fixedValue

2) Next: your checkMesh shows up with 207 cells < 0.001 determinant. Check were these cells are situated

3) Observe what happens in your flow field for pressure and velocity with paraview.
hxaxtma is offline   Reply With Quote

Old   February 17, 2017, 17:31
Default
  #5
New Member
 
Jeremy
Join Date: May 2016
Posts: 17
Rep Power: 7
j_moulton is on a distinguished road
Hi everyone, receiving a similar message for what I think is a simple case (attempting incompressible, laminar flow in a pipe):

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#5 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#6 Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#7 ? at ??:?
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9 ? at ??:?
Floating point exception

I have been Frankensteining together some code and I thought I was close. Most of the case files are attached as .zips. Please help me out with some feedback! Thanks.
Attached Files
File Type: zip 0.zip (1.4 KB, 13 views)
File Type: zip blockMeshDict_boundary.zip (1.5 KB, 5 views)
File Type: zip system.zip (6.3 KB, 7 views)
j_moulton is offline   Reply With Quote

Old   February 17, 2017, 17:48
Default
  #6
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 26
chegdan will become famous soon enoughchegdan will become famous soon enough
Jeremy,

After a quick look at your files, I can try suggest a few things. I'm assuming that you are using icoFoam, pisoFoam, pimpleFoam, or simpleFoam to perform your simulations. If so, this error can be caused by an incorrectly specified set of boundary conditions for p and U. For implicit methods (like the ones used in the above solvers), you need something like

fixed value velocity inlet
zerogradient pressure inlet

zeroGradient velocity outlet
fixedValue pressure outlet

fixedValue (0 0 0) velocity on the walls
zeroGradient pressure on the walls.

these should be stable boundary conditions for laminar pipe flow, assuming your mesh is fine.
jylee4 and piu58 like this.
__________________
Dan

Find me on
Twitter @dancombest
LinkedIn
WordPress
chegdan is offline   Reply With Quote

Old   February 23, 2017, 11:49
Default
  #7
New Member
 
Jeremy
Join Date: May 2016
Posts: 17
Rep Power: 7
j_moulton is on a distinguished road
Quote:
Originally Posted by chegdan View Post
Jeremy,

After a quick look at your files, I can try suggest a few things. I'm assuming that you are using icoFoam, pisoFoam, pimpleFoam, or simpleFoam to perform your simulations. If so, this error can be caused by an incorrectly specified set of boundary conditions for p and U. For implicit methods (like the ones used in the above solvers), you need something like

fixed value velocity inlet
zerogradient pressure inlet

zeroGradient velocity outlet
fixedValue pressure outlet

fixedValue (0 0 0) velocity on the walls
zeroGradient pressure on the walls.

these should be stable boundary conditions for laminar pipe flow, assuming your mesh is fine.
Thank you for the feedback, Dan. I implemented your changes but now I'm playing host to a new cast of problems. The Courant number blows up in just a few iterations and I'm not seeing any flow in Paraview. I adjusted my deltat in the controlDict but I'm not sure what else to do. Any thoughts? I think it could be a scaling issue when I exported from AutoCAD, but the documentation on that whole process is pretty scant.
j_moulton is offline   Reply With Quote

Old   February 23, 2017, 11:59
Default
  #8
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 26
chegdan will become famous soon enoughchegdan will become famous soon enough
It can be complex, and courant number issues are often resolved with smaller time steps, so you're on the right track. There is a great post

How to give enough info to get help

That will make good suggestions on how to get help as sometimes it is difficult to assess the issue with sparse information. A new thread may get more traction.
__________________
Dan

Find me on
Twitter @dancombest
LinkedIn
WordPress
chegdan is offline   Reply With Quote

Old   February 23, 2017, 12:02
Default
  #9
New Member
 
Jeremy
Join Date: May 2016
Posts: 17
Rep Power: 7
j_moulton is on a distinguished road
Quote:
Originally Posted by chegdan View Post
It can be complex, and courant number issues are often resolved with smaller time steps, so you're on the right track. There is a great post

How to give enough info to get help

That will make good suggestions on how to get help as sometimes it is difficult to assess the issue with sparse information. A new thread may get more traction.
Thanks, Dan!
chegdan likes this.
j_moulton is offline   Reply With Quote

Old   February 13, 2018, 21:36
Default
  #10
Member
 
Join Date: Jan 2018
Location: Malaysia
Posts: 58
Rep Power: 5
jiahui_93 is on a distinguished road
Hi, i faced the similar problem but with extra different problems so i started a new post. i am sorry if causing any inconvenience. This is my problem shown

Code:
Courant Number mean: 0.04994512 max: 5.830545
Time = 0.005

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::surfaceInterpolation::makeWeights() const at ??:?
#4  Foam::surfaceInterpolation::weights() const at ??:?
#5  Foam::surfaceInterpolation::makeDeltaCoeffs() const at ??:?
#6  Foam::surfaceInterpolation::deltaCoeffs() const at ??:?
#7  Foam::fvPatch::deltaCoeffs() const at ??:?
#8  Foam::mixedFvPatchField<Foam::Vector<double> >::evaluate(Foam::UPstream::commsTypes) at ??:?
#9  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::Boundary::evaluate() in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/pimpleDyMFoam"
#10  Foam::solidBodyMotionFvMesh::update() at ??:?
#11  ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/pimpleDyMFoam"
#12  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13  ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/pimpleDyMFoam"
Floating point exception (core dumped)
this is the link to my post
PimpleDyMFoam errors- Foam::error::printStack(Foam::Ostream&) at

I will very appreciate and grateful if there's some advice or suggestion for me to solve this. Thanks a lot for your time
jiahui_93 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Savonius pimpleDyMFoam vitokad OpenFOAM Pre-Processing 10 September 16, 2014 10:30
From simpleFoam to pimpleDyMFoam gregjunqua OpenFOAM Running, Solving & CFD 0 May 6, 2014 21:48
pimpleDyMFoam issue giovanidiniz OpenFOAM Running, Solving & CFD 1 July 5, 2013 08:25
pimpleDyMFoam samiam1000 OpenFOAM 2 September 19, 2012 11:11
Error with pimpleDyMFoam samiam1000 OpenFOAM 2 June 11, 2012 07:21


All times are GMT -4. The time now is 03:45.