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

NACA 0012 Case Will Not Converge

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 22, 2011, 00:00
Default NACA 0012 Case Will Not Converge
  #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 great difficulty trying to set up a case for a NACA 0012 airfoil that will converge. I have taken great pains to get a structured C-grid with y+ of ~30 (for k-omega SST), and edgeGrading to overcome the problem of high aspect ratio cells in the wake. This case has converged with meshes that I do not trust (first cell at y+ ~ 30, second at y+ ~ 200), but I have tried tweaking the mesh and the case but could not get it to work.

I feel like the NACA 0012 is a pretty straightforward example, which makes it all the more frustrating that I cannot get it to work. My case is attached - I would appreciate if someone could have a look and suggest where I might be going wrong.

Thanks,

Dan
Attached Files
File Type: zip VISN021a.zip (20.6 KB, 58 views)
dancfd is offline   Reply With Quote

Old   July 22, 2011, 00:53
Default
  #2
Senior Member
 
Daniel
Join Date: Jul 2009
Location: Montreal, Canada
Posts: 151
Rep Power: 8
dancfd is on a distinguished road
On a related note, has anyone successfully run a 2-D airfoil simulation that converged and produced results that compared well to experimental data?

Thanks,
Dan
dancfd is offline   Reply With Quote

Old   July 22, 2011, 01:25
Default
  #3
Senior Member
 
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 9
FelixL is on a distinguished road
Good morning, Dan,


I was looking into your case a bit and I think the first thing to have a look at should be the mesh.

First of all, I get a few warnings when running blockMesh:

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: -8.5e-09 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: -0.00049768 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 blockMesh/blockMeshTopology.C at line 255
    negative volume block : 3, probably defined inside-out
The case works and checkMesh doesn't complain, though, but you probably might want to fix that, just to be sure.

Secondly, at the regions of your domain far away from the airfoil you have huge differences in cell sizes! The size ratio of adjacant cells should not overcome 2, otherwise the stability of the simulation could be critically affected.


You should also think about a proper initialization. I ran potentialFoam before I started simpleFoam and the simulation seemed to converge. After 500 steps the fields were looking pretty good, I havent checked the accuracy, though.


I hope I could help you!

Greetings,
Felix.
FelixL is offline   Reply With Quote

Old   July 27, 2011, 00:31
Default
  #4
Senior Member
 
Daniel
Join Date: Jul 2009
Location: Montreal, Canada
Posts: 151
Rep Power: 8
dancfd is on a distinguished road
Hi Felix,

Thanks for your advice! I have changed the mesh grading to reduce the difference between the cell sizes at the interface between the "leading edge" blocks of the mesh and the "upper/lower surface" blocks of the mesh (I believe this is the area you were referring to - pic attached).

I ran potentialFoam prior to running simpleFoam this time around, and I am waiting on the results as the case runs...

Regarding the blockMesh errors, I was able to reduce these by changing the order of the block 3 vertices to "( 3 9 11 1 2 8 10 0)". However, this introduced a host of errors with checkMesh:

Code:
Checking geometry...
    Overall domain bounding box (-9.899 -10 0) (10 10 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 (0.0055776 -8.3664e-07 -7.39573e-16) possible hole in boundary description.
 ***Open cells found, max cell openness: 1, number of open cells 300
  <<Writing 300 non closed cells to set nonClosedCells
  <<Writing 9900 cells with high aspect ratio to set highAspectRatioCells
    Minumum face area = 3.81788e-07. Maximum face area = 0.586083.  Face area magnitudes OK.
    Min volume = 2e-300. Max volume = 0.0146634.  Total volume = 19.7899.  Cell volumes OK.
    Mesh non-orthogonality Max: 180 average: 55.3971
   *Number of severely non-orthogonal faces: 2.
 ***Number of non-orthogonality errors: 20000.
  <<Writing 20002 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 60100 faces are incorrectly oriented.
  <<Writing 40100 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 0.506229 OK.

Failed 4 mesh checks.
This leads to two questions:
1) How do I address the blockMesh errors that are of the following nature? Is it possible to visualize the discrepant faces?
Code:
--> 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: -8.5e-09 for face 0
2) How do I get blockMesh and checkMesh to like the same mesh?

Thanks,
Dan
Attached Images
File Type: jpg mesh.jpg (99.1 KB, 71 views)
dancfd is offline   Reply With Quote

Old   July 27, 2011, 02:02
Default
  #5
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Hi

The best thing you can do is go through each block in blockMesh

uncomment all but the first one and methodically enable a block at a time until you get the negative volumes.

You probably have a block which you have gone around the points in the wrong direction and the cells get "inverted" even though it looks ok.
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   November 14, 2011, 07:55
Default Results?
  #6
New Member
 
Felipe
Join Date: Apr 2010
Posts: 13
Rep Power: 7
fippo_dk is on a distinguished road
Hi Dan

I'm also running a simulation of 2D airfoil with k-omega SST.

I would like to know whether we could compare results.

I have other airfoils (NACA) until now, but I could mesh the naca0015 in order to compare.

Regards,

Felipe
fippo_dk is offline   Reply With Quote

Old   November 14, 2011, 20:09
Default
  #7
Senior Member
 
Daniel
Join Date: Jul 2009
Location: Montreal, Canada
Posts: 151
Rep Power: 8
dancfd is on a distinguished road
Hello Felipe,

I finally got the mesh to converge, and the results are reasonable. My residuals are higher than I would like, but that is probably due to the high mesh resolution. Let me know what you would like by message and I would be happy to 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
NACA 0012 Simulation in CFX Satheesh CFX 1 March 22, 2011 22:18
Solving naca 0012 airfoil naveen OpenFOAM Pre-Processing 3 February 17, 2009 10:25
NACA 0012 Mesh Alex FLUENT 4 March 28, 2006 23:34
flow over naca 0012 Frederic Felten Main CFD Forum 6 May 23, 2001 11:45
naca 0012 press distribution huong FLUENT 2 March 27, 2001 22:27


All times are GMT -4. The time now is 13:54.