CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   simpleFoam simulation with mesh from Pointwise crashes immediately (https://www.cfd-online.com/Forums/openfoam-solving/143770-simplefoam-simulation-mesh-pointwise-crashes-immediately.html)

Artur November 2, 2014 10:14
simpleFoam simulation with mesh from Pointwise crashes immediately
 
Hi Foamers!

I'm trying to learn how to use Pointwise for OpenFOAM simulations. I'm trying to create a 2D C-grid of an airfoil following the official tutorials:

https://www.youtube.com/watch?v=qifDBLbKvwM

https://www.youtube.com/watch?v=SwLkbrZMYMo

When I try to run my case it works fine with potentialFoam but then throws a FP exception at the first velocity loop. I have used the same numerical setup as for grids created using native blockMesh and so I am quite certain the BCs, schemes and linear solvers are chosen correctly. I'm attaching the case and the Pointwise project (inside the .zip archive).

Here's a checkMesh log:

Code:
/*---------------------------------------------------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.2                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
Build  : 2.2.2-9240f8b967db
Exec  : checkMesh -allTopology -allGeometry
Date  : Nov 02 2014
Time  : 15:06:09
Host  : "artur-Aspire-V3-571G"
PID    : 3624
Case  : /home/artur/Dropbox/myOpenFoamStuff/run/bladelessPropeller/wing2D
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Enabling all (cell, face, edge, point) topology checks.

Enabling all geometry checks.

Time = 0

Mesh stats
    points:          19600
    internal points:  0
    edges:            48608
    internal edges:  9408
    internal edges using one boundary point:  0
    internal edges using two boundary points:  9408
    faces:            38612
    internal faces:  19012
    cells:            9604
    faces per cell:  6
    boundary patches: 5
    point zones:      0
    face zones:      0
    cell zones:      0

Overall number of cells of each type:
    hexahedra:    9604
    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.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
  <<Writing 2 cells with two non-boundary faces to set twoInternalFacesCells
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch              Faces    Points  Surface topology                  Bounding box
    frontAndBack        19208    19600    ok (non-closed singly connected)  (-0.95 -1 0) (1 1 0.1)
    inlet              98      198      ok (non-closed singly connected)  (-0.95 -1 0) (0.0499997 1 0.1)
    outlet              98      198      ok (non-closed singly connected)  (1 -1 0) (1 1 0.1)
    topAndBottom        98      200      ok (non-closed singly connected)  (0.0499997 -1 0) (1 1 0.1)
    wing                98      196      ok (non-closed singly connected)  (-0.0500302 -0.0105422 0) (0.0499997 0.00287132 0.1)

Checking geometry...
    Overall domain bounding box (-0.95 -1 0) (1 1 0.1)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (9.51962e-18 1.66799e-18 -8.27013e-16) OK.
    Max cell openness = 3.04422e-16 OK.
    Max aspect ratio = 612.418 OK.
    Minimum face area = 9.51948e-08. Maximum face area = 0.0143194.  Face area magnitudes OK.
    Min volume = 9.51948e-09. Max volume = 0.00140263.  Total volume = 0.346866.  Cell volumes OK.
    Mesh non-orthogonality Max: 56.1806 average: 9.47516
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.841906 OK.
    Coupled point location match (average 0) OK.
    Face tets OK.
    Min/max edge length = 0.000144024 0.143194 OK.
    All angles in faces OK.
    Face flatness (1 = flat, 0 = butterfly) : average = 1  min = 1
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 2.6908e-05 average: 1.60367
 ***Cells with small determinant (< 0.001) found, number of cells: 150
  <<Writing 150 under-determined cells to set underdeterminedCells
    Concave cell check OK.

Failed 1 mesh checks.

End
Small determinant cells are in the wake, I've had them there before with other grids and they never caused me any problems.

In more details, here are the steps I've taken:
1. create airfoil sketch in Autodesk Inventor and exported as an iges file
2. imported the database to Pointwise, created connectors
3. assembled domains and extruded them by translation of 0.1 units in 1 step
4. exported as CAE for OpenFOAM having defined the BCs
5. ran the case to find it doesn't work

I really want to use Pointwise for more complex geometries which I cannot mesh using Python and blockMesh as I normally do. So I really need to get past this initial stage, any help will be much appreciated.

https://www.dropbox.com/s/l7p7e9ra0d...ing2D.zip?dl=0

Have a nice Sunday,

Artur

mdeaves March 31, 2015 06:10
3 Attachment(s)
Hey Artur,

I think I am having the same problem with my 2D NACA0012 O-Mesh. I was given a working mesh from a colleague, and when I try to replicate the mesh in Pointwise the simulation fails on the first time step.

I have narrowed down the problem to the faces, neighbor, and owner files created by Pointwise. When I use the ones from the working mesh, all is good, but when I use those exported from Pointwise it crashes.

I guess somehow the ordering of the faces or the assignment of owner and neighboring faces is messed up in Pointwise, or effects the fvSchemes or fvSolution settings I'm using.

I have attached these files for you and others to see.

Have you made any progress on this issue?

Artur March 31, 2015 06:51
Apologies, I was sure I had posted my solution (took me a long time to figure out!), here it is:

For some reason the Pointwise grid works OK with some linear solvers but doesn't with others, I'm sure it has something to do with the ordering of cells/faces, as you've pointed out as well. To overcome this I use these solvers:

pressure:
Code:
        solver          PCG;
        preconditioner  DIC;
velocity/turbulence
Code:
        solver          PBiCG;
        preconditioner  DILU;
For some reason neither the smoothSolver (which you are using) and GAMG (which I used to use) work.

Let me know if this helps,

A

mdeaves March 31, 2015 07:37
Excellent, excellent, excellent! This worked like a charm.

If you are ever in Delft, Netherlands send me a message and I'll take you for a beer.

Thank you.

-Michael

Artur March 31, 2015 08:05
Perfect, glad it worked OK. I was in Wageningen last week, too bad we only got to this point now. Maybe next time :)

A

Artur September 4, 2015 10:50
I just noticed something on a different simulation using Pointwise and OpenFOAM: it seems like running the "renumberMesh" utility helps in overcoming the initial problem in this thread, probably there is something about mesh ordering the multi-grid solver needs which it doesn't get from Pointwise by default.

Maybe someone will find this hint useful.

A


All times are GMT -4. The time now is 04:03.