Negative courant number

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

February 3, 2015, 14:55
Negative courant number
#1
Senior Member

Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 493
Rep Power: 11
Dear All,

I am running a simulation using pimplefoam and something strange happens: I get a negativa courant number, from the very first iteration.

Code:
```Create time

Create mesh for time = 0

--> FOAM Warning :
From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
in file /home/szampini/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude/Field.C at line 318
Reading "/home/szampini/Documenti/Afros/CFDSimulations/testRTM/0/U.boundaryField.inlet" from line 29 to line 9
expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.

Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar
No finite volume options present

PIMPLE: Operating solver in PISO mode

Starting time loop

Courant Number mean: -1.68919e-06 max: -0
deltaT = 0.000111111
Time = 0.000111111

smoothSolver:  Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.0219292, No Iterations 1000
smoothSolver:  Solving for Uz, Initial```
And after few iteration the courant number becomes smaller and smaller (negative and bigger in magnitude) and the simulation diverges.

Could you have a look at the attached case?

Thanks a lot,
Samuele
Attached Files
 testRTM.tar.gz (9.3 KB, 7 views)

 February 3, 2015, 16:01 #2 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 9,860 Blog Entries: 39 Rep Power: 108 Quick answer: Incorrect usage of a transient solver, see file "system/fvSchemes": Code: ```ddtSchemes { default steadyState; }``` This is why the Courant Number cannot evolve over time, since there is no such thing as "time" in a steady state solver samiam1000 likes this.

 February 4, 2015, 07:03 #3 Senior Member   Samuele Z Join Date: Oct 2009 Location: Mozzate - Co - Italy Posts: 493 Rep Power: 11 This was for sure an error, but not the only one. I changed the time scheme, but nothing happened. Any other idea? Thanks, Samuele

 February 4, 2015, 13:29 #4 Senior Member   Tom Fahner Join Date: Mar 2009 Location: Delft, Netherlands Posts: 358 Rep Power: 14 Hi Samuele, I ran your Allrun script except for the pimpleFoam part and after that I ran checkMesh. During blockMesh there is already a warning for negative volumes, which is later confirmed by checkMesh output. I copied that output for you here: Code: ```Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 452403 faces: 1041592 internal faces: 734408 cells: 296000 faces per cell: 6 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 296000 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. *Number of regions: 5 The mesh has multiple regions which are not connected by any face. <

 February 5, 2015, 07:11 #5 Senior Member   Samuele Z Join Date: Oct 2009 Location: Mozzate - Co - Italy Posts: 493 Rep Power: 11 Got it: solved! Thanks a lot, Samuele. This was a problem in the blockMeshDict! Samuele

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 42 January 8, 2017 13:55 danny123 OpenFOAM 19 October 24, 2012 07:44 hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58 liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07

All times are GMT -4. The time now is 09:54.