[samiam1000]

Dear All,

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

Create time

Create mesh for time = 0

Reading field p

Reading field U

--> 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.
Reading/calculating face flux field phi

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

[wyldckat]

Quick answer: Incorrect usage of a transient solver, see file "system/fvSchemes":

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]

This was for sure an error, but not the only one. I changed the time scheme, but nothing happened.

Any other idea?

Thanks,
Samuele

[tomf]

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:

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.
  <<Writing region information to "0/cellToRegion"
  <<Writing region 0 with 18000 cells to cellSet region0
  <<Writing region 1 with 30000 cells to cellSet region1
  <<Writing region 2 with 200000 cells to cellSet region2
  <<Writing region 3 with 30000 cells to cellSet region3
  <<Writing region 4 with 18000 cells to cellSet region4

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    outlet1             592      903      ok (non-closed singly connected)  
    outlet2             592      903      ok (non-closed singly connected)  
    top                 101900   103626   ok (non-closed singly connected)  
    walls               204000   205911   ok (non-closed singly connected)  
    inlet               100      121      ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-0.12 0 -0.25) (0.12 0.03 0.25)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (8.43768e-19 1.05278e-17 -3.86038e-20) OK.
 ***High aspect ratio cells found, Max aspect ratio: 1e+194, number of cells 296000
  <<Writing 296000 cells with high aspect ratio to set highAspectRatioCells
    Minimum face area = 1e-06. Maximum face area = 1e-06.  Face area magnitudes OK.
 ***Zero or negative cell volume detected.  Minimum negative volume: -1e-09, Number of negative volume cells: 296000
  <<Writing 296000 zero volume cells to set zeroVolumeCells
    Mesh non-orthogonality Max: 180 average: 180
 ***Number of non-orthogonality errors: 734408.
  <<Writing 734408 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 1776000 faces are incorrectly oriented.
  <<Writing 1041592 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 2.5e-06 OK.
    Coupled point location match (average 0) OK.

Failed 4 mesh checks.

End

So it tells you it finds negative volumes, which would explain a negative courant number.

Please check your blockMesh setup and make sure you have a valid mesh before running pimpleFoam.

Regards,
Tom

[samiam1000]

Got it: solved!

Thanks a lot,
Samuele.

This was a problem in the blockMeshDict!

Samuele