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

SimpleFoam solver issue

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 3, 2017, 11:31
Default SimpleFoam solver issue
  #1
New Member
 
Join Date: Mar 2017
Posts: 7
Rep Power: 5
isaacOF is on a distinguished road
Hi all,

I'm new to OpenFoam and I would like to learn it because I think it is a "must have" knowledge for an engineer.
I started with a simple geometry in order to understand the flow path inside a rectangular duct with two honeycomb filters inside it.
The mesh of the fluid domain was made with SALOME (v 7.8.0) and imported the .unv file in OpenFoam with the ideasUnvToFoam.
To prepare the simulation I started from the incompressible/pitzDaily tutorial, and applide it to a 3D domain.
However, an error occurred, but I really don't know what it belongs to and how to debug it. You can find attached the log of error.

I really hope in your help!!
many thanks in advantage,
isaacOF
Attached Files
File Type: txt error.txt (3.7 KB, 16 views)
isaacOF is offline   Reply With Quote

Old   March 3, 2017, 15:40
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,922
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

Since the error happens during solution of pressure equation, could you post checkMesh command output?
alexeym is offline   Reply With Quote

Old   March 6, 2017, 03:02
Default
  #3
New Member
 
Join Date: Mar 2017
Posts: 7
Rep Power: 5
isaacOF is on a distinguished road
Hi alexeym,

thank you for the answer. Here it is the checkMesh output.

Attached Files
File Type: txt checkMesh.txt (6.6 KB, 6 views)
isaacOF is offline   Reply With Quote

Old   March 6, 2017, 05:46
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,922
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Does your domain really consist of 63 disjoint parts? I think there is a problem with mesh conversion. Is UNV the only option for mesh export?
alexeym is offline   Reply With Quote

Old   March 6, 2017, 08:00
Default
  #5
New Member
 
Join Date: Mar 2017
Posts: 7
Rep Power: 5
isaacOF is on a distinguished road
I guess disjoint parts are mesh parts that are not connected together: how can I avoid them during the mesh creation?
UNV is not the only format, SALOME allows the following ones: DAT, MED, UNV, STL, CGNF, SAUV, GMF.
isaacOF is offline   Reply With Quote

Old   March 6, 2017, 11:06
Default
  #6
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,922
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Since amount of information about mesh and geometry is rather limited, I guess, the problem happens not during mesh creation but during mesh export/import.

There is https://github.com/nicolasedh/salomeToOpenFOAM, it can help to avoid UNV as intermediate format.
alexeym is offline   Reply With Quote

Old   March 9, 2017, 02:26
Default
  #7
New Member
 
Join Date: Mar 2017
Posts: 7
Rep Power: 5
isaacOF is on a distinguished road
It worked fine and the simulation started.
You were right, it was an export/import issue!
However, after a few time steps, the simulation crashes and the following error:

Time = 17

smoothSolver: Solving for Ux, Initial residual = 0.999619, Final residual = 0.0772869, No Iterations 10
smoothSolver: Solving for Uy, Initial residual = 0.999906, Final residual = 0.0994966, No Iterations 9
smoothSolver: Solving for Uz, Initial residual = 0.999473, Final residual = 0.0911458, No Iterations 9
#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::GAMGSolver::solveCoarsestLevel(Foam::Field<d ouble>&, Foam::Field<double> const&) const at ??:?
#6 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:?
#7 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#8 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#9 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#10 Foam::fvMatrix<double>::solve() in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#11 ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#12 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13 ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
Floating point exception (core dumped)

How can i manage this?
isaacOF is offline   Reply With Quote

Old   March 9, 2017, 03:45
Default
  #8
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,922
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Since your mesh has changed, let's start again with checkMesh output.
alexeym is offline   Reply With Quote

Old   March 10, 2017, 03:11
Default
  #9
New Member
 
Join Date: Mar 2017
Posts: 7
Rep Power: 5
isaacOF is on a distinguished road
Here it is!
Attached Files
File Type: txt checkMesh_1.txt (3.0 KB, 2 views)
isaacOF is offline   Reply With Quote

Old   March 10, 2017, 03:40
Default
  #10
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,922
Rep Power: 35
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Here is main points of the output:

Code:
Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    300225
    polyhedra:     0
and

Code:
    Mesh non-orthogonality Max: 84.9448 average: 19.4851
   *Number of severely non-orthogonal (> 70 degrees) faces: 620.
    Non-orthogonality check OK.
  <<Writing 620 non-orthogonal faces to set nonOrthoFaces
pitzDaily has hexagonal mesh with 5 degree of maximum non-orthogonality, so fvSchemes and fvSolution from this tutorial is not quite applicable to your situation.

So, you have several choices:

0. Go to tutorials folder and search to cases, where nNonOrthogonalCorrectors in SIMPLE sub-dictionary is non-zero (heatTransfer/buoyantBoussinesqSimpleFoam/iglooWithFridges for example).
1. Get yourself new mesh
2. Set nNonOrthogonalCorrectors in fvSolution to, let's say, 2.
3. Change gradSchemes to leastSquares. Or even to cellLimited leastSquares.
4. Use "limited corrected" schemes.
5. Google "OpenFOAM highly non-orthogonal meshes"
alexeym is offline   Reply With Quote

Old   March 30, 2017, 04:37
Default
  #11
New Member
 
Join Date: Mar 2017
Posts: 7
Rep Power: 5
isaacOF is on a distinguished road
Thank you Alexey for all these hints. I've tried some of them, but without any success. Surely it depends on my limited knowledge of OpenFOAM
So I decided to strongly simplify the geometrical model by mantaining the main characteristics (shapes, discontinuities, ecc.). Then I made a better mesh and got the incompressible/pitzDaily tutorial settings again: however, the only way I found to carry out the full simulation without any errors is by modifying the following fvSchemes setting:

divSchemes
{
default none;
div(phi,U) bounded Gauss upwind;
div(phi,k) bounded Gauss upwind;
div(phi,epsilon) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind;
div(phi,v2) bounded Gauss upwind;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
div(nonlinearStress) Gauss linear;
}

I'd like to improve my knowledge of the solver settings, do you know a good documentation (in addition to the official one) where I can find useful information about the relationship between settings and simulation solutions?

Thanks again for your help
isaacOF is offline   Reply With Quote

Old   March 30, 2017, 05:07
Default
  #12
Member
 
Ricky
Join Date: Jul 2014
Location: Germany
Posts: 77
Rep Power: 8
kera is on a distinguished road
Quote:
Originally Posted by isaacOF View Post
I'd like to improve my knowledge of the solver settings, do you know a good documentation (in addition to the official one) where I can find useful information about the relationship between settings and simulation solutions?
have a look at this one Tips and triks in OF

Regards,
Ricky
__________________
If it is easy, then something is fishy!
kera is offline   Reply With Quote

Old   April 12, 2017, 08:48
Default
  #13
New Member
 
Join Date: Mar 2017
Posts: 7
Rep Power: 5
isaacOF is on a distinguished road
Thank you very much Ricky, it's a very useful document: by following the tricks that it suggests, I could run the whole simulation.
Howeveer, I'm still interested in improving my knowledge of the theory that is behind these settings, do you have any other documentation to suggest?

Thanks in advance!
isaacOF is offline   Reply With Quote

Reply

Tags
3d steadystate, salome mesh, simplefoam

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
OpenFoam profiling the solver simpleFoam andre OpenFOAM Programming & Development 9 April 29, 2017 08:51
Density issue in simpleFoam mqsim OpenFOAM Running, Solving & CFD 0 April 25, 2016 09:52
simpleFoam parallel solver & Fluent polyhedral mesh Zlatko OpenFOAM Running, Solving & CFD 3 September 26, 2014 06:53
Working directory via command line Luiz CFX 4 March 6, 2011 20:02
snappyMesh Motor Bike case for simpleFoam solver s.sivakumar OpenFOAM Pre-Processing 0 July 23, 2009 00:51


All times are GMT -4. The time now is 20:06.