CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Native Meshers: blockMesh

No-win situation?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 4, 2011, 17:42
Default No-win situation?
  #1
Senior Member
 
Daniel
Join Date: Jul 2009
Location: Montreal, Canada
Posts: 151
Rep Power: 8
dancfd is on a distinguished road
Hello all,

I am having trouble running the case /simpleFoam/airfoil2D when I replace the default mesh with mine, a NACA 0012 in a C-grid (blockMeshDict attached). The problem is that the results show pressure/velocity fluctuations in the far field, and no characteristic pressure field around the airfoil. I thought this might be due to the mesh, since blockMesh gives me the following warnings:


Code:
Creating block mesh topology
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -0.000497689 for face 0
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.26062e-08 for face 2
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.26063e-08 for face 3
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.26063e-08 for face 4
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.26063e-08 for face 5
--> FOAM Warning : 
    From function blockMesh::createTopology(IOdictionary&)
    in file createTopology.C at line 397
    negative volume block : 0, probably defined inside-out
I tried to resolve the issue by changing the order of the vertex numbering in block 0 from hex (2 4 6 0 3 5 7 1) to hex (3 5 7 1 2 4 6 0), and that yielded only the following:

Code:
Creating block mesh topology
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -0.000497664 for face 1
The problem is that now simpleFoam will not even run! (log attached) I am not surprised, because the interface between two of the blocks clearly looks inside out. CheckMesh was not kind either (see checkMeshAdjusted). However, checkMesh had no problem with the first mesh (log.checkMesh).

In a nutshell, the problem is this: blockMesh gives me several warnings when building my mesh that runs; blockMesh only gives one error (which I do not know how to fix) when building the mesh that will not run. CheckMesh gives a worse report to the mesh that blockMesh liked best, and simpleFoam will not run the mesh checkMesh does not like, but will run the other one with poor results.

Can anyone tell me what is wrong with this mesh? I would appreciate any advice.

Thank you,

Dan
Attached Files
File Type: zip thesis.zip (8.9 KB, 14 views)
dancfd is offline   Reply With Quote

Old   June 5, 2011, 02:04
Default
  #2
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 11
MartinB is on a distinguished road
Hi Dan,

I just tested you mesh and although I do get the same warnings the simulation runs fine.

There could be a problem with the polyLine definition: for example in lines 540 and 541 there is the same point defined two times. May be there are other doubles, too... If you want to get rid of the warnings you can try to split the front block (block 0) into two blocks.

In the attachment you can find the running case, tested with OpenFOAM-1.7.x. The only modification to the original airfoil2D case are reduced relaxation factors and a faster solver.

Martin
Attached Files
File Type: gz dan.tar.gz (7.9 KB, 12 views)
MartinB is offline   Reply With Quote

Old   June 5, 2011, 16:43
Default
  #3
Senior Member
 
Daniel
Join Date: Jul 2009
Location: Montreal, Canada
Posts: 151
Rep Power: 8
dancfd is on a distinguished road
Hi Martin,

Thank you for taking the time to look at the problem I am having. I ran the case, and it looks like one issue was that the simulation was not running long enough to reach steady-state. There were two instances where polyLines had two identical points (as you pointed out), but commenting them had no effect. I might try splitting block 0 into two, but I do not understand why this would address the warnings.

Thanks for your help,

Dan
dancfd 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
[GAMBIT] Gambit GUI slow response in Win 7 Peter023 ANSYS Meshing & Geometry 5 October 30, 2011 07:00
how nozzle's inlet flow speed change in an ocean situation sogolf FLOW-3D 1 August 3, 2009 15:41
GAMBIT and win xp Philip FLUENT 10 January 1, 2007 14:33
Exceed 7.0 on Win 2000 Yoshi CFX 8 October 11, 2001 06:09
Fluent on PC, Win 2000 or Linux Thorsten Rauch FLUENT 2 February 23, 2001 11:05


All times are GMT -4. The time now is 15:00.