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

simpleFoam simulation with mesh from Pointwise crashes immediately

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 2, 2014, 11:14
Default simpleFoam simulation with mesh from Pointwise crashes immediately
  #1
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
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
Artur is offline   Reply With Quote

Old   March 31, 2015, 06:10
Default
  #2
New Member
 
Michael Deaves
Join Date: Dec 2013
Posts: 5
Rep Power: 3
mdeaves is on a distinguished road
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?
Attached Files
File Type: c controlDict.c (1.9 KB, 4 views)
File Type: c fvSolution.c (1.7 KB, 4 views)
File Type: c fvSchemes.c (1.4 KB, 4 views)
mdeaves is offline   Reply With Quote

Old   March 31, 2015, 06:51
Default
  #3
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
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
Artur is offline   Reply With Quote

Old   March 31, 2015, 07:37
Default
  #4
New Member
 
Michael Deaves
Join Date: Dec 2013
Posts: 5
Rep Power: 3
mdeaves is on a distinguished road
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
mdeaves is offline   Reply With Quote

Old   March 31, 2015, 08:05
Default
  #5
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
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 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem in initializing transient simulation with a finer mesh sidd CFX 6 April 1, 2015 16:41
Airfoil simulation solution interfered by mesh Dvergr OpenFOAM Running, Solving & CFD 1 September 28, 2014 02:05
simpleFoam parallel solver & Fluent polyhedral mesh Zlatko OpenFOAM Running, Solving & CFD 3 September 26, 2014 06:53
Improve Mesh quality - airfoil simulation Lukas84 STAR-CCM+ 4 July 6, 2010 10:07
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09


All times are GMT -4. The time now is 09:12.