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

What's wrong with the patch / p...?

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

Like Tree2Likes
  • 2 Post By danishdude

Reply
 
LinkBack Thread Tools Display Modes
Old   January 4, 2012, 17:39
Default What's wrong with the patch / p...?
  #1
Member
 
Klaus
Join Date: Mar 2009
Posts: 70
Rep Power: 8
klausb is on a distinguished road
Hello,

I want to test a hydrofoil (symmetry case based on motorBike case) and keep getting error messages from potentialFoam and simpleFoam.

What's wrong?

Find attached the error messages and the case (without the foil, as the file exceeds 97kB).

E.g. potentialFoam log:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.0.1-5ae28021cd90
Exec : potentialFoam -noFunctionObjects -writep
Date : Jan 04 2012
Time : 22:25:53
Host : tenno-EP45-UD3R
PID : 7255
Case : /home/tenno/OpenFOAM/tenno-2.0.1/run/tutorials/incompressible/simpleFoam/wing
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 mesh for time = 0

Reading field p



--> FOAM FATAL IO ERROR:

patch type 'patch' not constraint type 'symmetryPlane'
for patch maxY_domain_upper_wall of field p in file "/home/tenno/OpenFOAM/tenno-2.0.1/run/tutorials/incompressible/simpleFoam/wing/0/p"

file: /home/tenno/OpenFOAM/tenno-2.0.1/run/tutorials/incompressible/simpleFoam/wing/0/p::boundaryField::maxY_domain_upper_wall from line 27 to line 27.

From function symmetryFvPatchField<Type>::symmetryFvPatchField
(
const fvPatch& p,
const Field<Type>& field,
const dictionary& dict
)

in file fields/fvPatchFields/constraint/symmetry/symmetryFvPatchField.C at line 99.

FOAM exiting
Attached Files
File Type: txt log.blockMesh.txt (2.7 KB, 12 views)
File Type: txt log.potentialFoam.txt (1.8 KB, 2 views)
File Type: txt log.simpleFoam.txt (1.7 KB, 2 views)
File Type: txt log.snappyHexMesh.txt (57.3 KB, 0 views)
File Type: gz wing.tar.gz (38.9 KB, 12 views)
klausb is offline   Reply With Quote

Old   January 4, 2012, 18:57
Default
  #2
New Member
 
Michael Ahlmann
Join Date: Feb 2010
Posts: 27
Rep Power: 7
danishdude is on a distinguished road
Your symmetry planes are defined as patches in:

/constant/polyMesh/boundary

You need to change those to symmetry plane. The error message is telling you that you are trying to apply a symmetry condition to a patch.
lth and nisha like this.
danishdude is offline   Reply With Quote

Old   January 5, 2012, 08:01
Default Now I am running into the next problem - patch name .stl ...
  #3
Member
 
Klaus
Join Date: Mar 2009
Posts: 70
Rep Power: 8
klausb is on a distinguished road
Thank you!

But now I am running into the next patch problem.

SimpleFoam doesn't get the patch name of the wing. The wing is represented through wing.stl and the name defined in that file is also wing (first line is: solid wing).

Error: Cannot find any patch names matching wing_wing

SimpleFoam is looking for a patch name wing_wing which is to my knowledge made up internaly: name of wing.stl defined in sHMDict+ _name defined in the wing.stl file.

My trial & error approach didn't work.

Any idea, what needs to be changed? Find attached the simpleFoam log file.

Klaus
Attached Files
File Type: txt log.simpleFoam.txt (85.9 KB, 6 views)
klausb is offline   Reply With Quote

Old   January 5, 2012, 14:33
Default Case file - I am still not able to define the patch name
  #4
Member
 
Klaus
Join Date: Mar 2009
Posts: 70
Rep Power: 8
klausb is on a distinguished road
Hello,

find attached my case file - I am still not able to define the patchname for my wing (wing.stl).

I need to fix the following SimpleFoam error:

Reading surface description:
yNormal

--> FOAM Warning :
From function polyBoundaryMesh::patchSet(const wordReList&, const bool) const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 573
Cannot find any patch names matching wing_wing
--> FOAM Warning :
From function polyBoundaryMesh::patchSet(const wordReList&, const bool) const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 573
Cannot find any patch names matching wing_wing

Any ideas how to do that?

Klaus
Attached Files
File Type: txt log (Kopie).simpleFoam.txt (53.4 KB, 1 views)
File Type: gz wing (Kopie).tar.gz (88.6 KB, 11 views)
klausb is offline   Reply With Quote

Old   January 7, 2012, 14:24
Default
  #5
New Member
 
Michael Ahlmann
Join Date: Feb 2010
Posts: 27
Rep Power: 7
danishdude is on a distinguished road
Sorry for the slow response. The error message I get when running your case is:

Code:
--> FOAM FATAL ERROR: 
Invalid wall function specification
    Patch type for patch minX_inlet must be wall
    Current patch type is patch
This is because you specified the following in your /0/nu file:

Code:
    minX_inlet
    {
        type            nutkWallFunction;
        value           uniform 0;
    }
I'm assuming that your "minX_inlet" is in fact an inlet, as such, the /0/nut file should have the following instead:

Code:
    minX_inlet
    {
        type            calculated;
    }
Once that is fixed, the code issues the same error for maxX_outlet. So this one should also be changed to 'type calculated;" in the 0/nut

Additionally, the case also complains about use of deprecated syntax. This is not a big deal (and does not cause the code to stop); however, I recommend reviewing the messages and adjusting your input files per the instructions. The case will run without doing so.

With the above two modifications, the case successfully ran the first iteration on my machine. I did not check your boundary condition types in any level of detail as there are several examples on the forums of people modeling airfoils, and personally, I do not have much experience doing so, but I would recommend reviewing your wing boundary condition. Wouldn't it be more common to use a wall function than a fixed value for an object in the flow?

Best of luck!
danishdude 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
Using starToFoam clo OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 33 September 26, 2012 04:04
CheckMeshbs errors ivanyao OpenFOAM Running, Solving & CFD 2 March 11, 2009 03:34
udf error srihari FLUENT 0 February 9, 2009 10:00
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 08:29.