
[Sponsors] 
July 7, 2008, 20:50 
Hi everyone,
I am trying to

#1 
New Member
Patrice Castonguay
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
Hi everyone,
I am trying to simulate steady flow over a NACA0012 airfoil at Mach number 0.2 and AOA 2 degrees and I'm having problems converging to the solution with icoFoam. I'm using a structured Cmesh of dimensions (384x64) which can be seen here: www.stanford.edu/~pcasto2/naca0012_visc/mesh.pdf The utility checkMesh outputs the following:  Checking geometry... Domain bounding box: (14.5446 16.6068 0) (18 16.6068 1) Boundary openness (1.78119e18 1.88139e17 4.27264e16) OK. ***High aspect ratio cells found, Max aspect ratio: 74554.3, number of cells 7232 <<Writing 7232 cells with high aspect ratio to set highAspectRatioCells Minumum face area = 1.5362e08. Maximum face area = 3.57128. Face area magnitudes OK. Min volume = 1.5362e08. Max volume = 3.57128. Total volume = 938.87. Cell volumes OK. Mesh nonorthogonality Max: 88.216 average: 9.60062 *Number of severely nonorthogonal faces: 252. Nonorthogonality check OK. <<Writing 252 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 0.186059 OK. *Edges too small, min/max edge length = 1.90263e05 2.79354, number too small: 3244 <<Writing 3884 points on short edges to set shortEdges All angles in faces OK. Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1 All face flatness OK. Failed 1 mesh checks.  So it seems to complain about the HAR cells but I would really like to be able to obtain a solution on this mesh... Now my problem is the following: I can't get icoFoam to convergence properly. The pressure residual goes down to 4e04 but stops decreasing after. (see convergence history at: www.stanford.edu/~pcasto2/naca0012_visc/p0_conv.pdf) The Cp distribution I obtain for this convergence level does not agree with results obtained with our flow solver. (www.stanford.edu/~pcasto2/naca0012_visc/cp_plot.pdf). My boundary conditions are as follows: INLET p: zeroGradient, U: fixedValue (69.383 2.422 0) OUTLET p: fixedValue 100000, U: zeroGradient WALL p: zeroGradient, U: fixedValue (0 0 0) I'm using the same schemes used with the cavity tutorial except that I set nNonOrthogonalCorrectors to 2. I also reduced my time step to 2e07. I'm fairly new to OpenFOAM so maybe I missed something really obvious but I would really appreciate if you could help me in getting a converged solution. 

July 8, 2008, 16:03 
Hello Patrice,
As I can see

#2 
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
Hello Patrice,
As I can see, the value of the velocities that you are using lead to a turbulent flow (if the fluid is air), and icoFoam is destinated to laminar problems, as far as I know. Use simpleFoam instead. Regards, Paulo. 

July 9, 2008, 17:59 
Hey Paulo,
I understand th

#3 
New Member
Patrice Castonguay
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
Hey Paulo,
I understand that at this Reynolds number, the flow should transition to turbulent flow over the airfoil. However, the algorithm should still be able to converge even though it might not give the real physical solution. The velocity components seems to converge but I don't understand why pressure doesn't converge. Any idea what values for the parameters in fvSchemes or fvSolution would help improve the pressure convergence? Thanx Patrice 

July 12, 2008, 15:16 
Hello Patrice,
In my experi

#4 
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
Hello Patrice,
In my experience, high Reynolds number always lead to numerical instabilities. The model must have something to dissipate the turbulent energy (like epsilon or omega). That is my understanding, it might be not right. Any comments are apreciated. Regards, Paulo. PS: Sorry for the late reply. 

July 12, 2008, 18:24 
Hey Paulo,
Thanx for your r

#5 
New Member
Patrice Castonguay
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
Hey Paulo,
Thanx for your reply. I finally managed to have icoFoam converged. I also tried using simpleFoam and you are right, switching turbulence on (I used kepsilon) helps in improving the convergence. Also, I didn't have any problem converging when I reduced the Reynolds number. For those of you who are having convergence problem with simpleFoam or icoFoam, here are the setting I used. When using simpleFoam, if the pressure residual stalls, you can try increasing the relaxation factor for pressure to 0.5 or 0.6 after a few outer iterations, it might help to reach a lower pressure residual. Patrice  IcoFOAM: gradSchemes { default Gauss linear; grad(p) Gauss linear; } divSchemes { default Gauss upwind; div(phi,U) Gauss upwind; } laplacianSchemes { default none; laplacian(nu,U) Gauss linear limited 0.7; laplacian((1A(U)),p) Gauss linear limited 1.; } interpolationSchemes { default linear; interpolate(HbyA) linear; } solvers { p PCG { preconditioner DIC; tolerance 1e08; relTol 0; }; U PBiCG { preconditioner DILU; tolerance 1e08; relTol 0; }; } PISO { nCorrectors 1; nNonOrthogonalCorrectors 1; } SIMPLEFOAM Same fvSchemes as with IcoFOAM fvSolution: p PCG { preconditioner DIC; tolerance 1e08; relTol 0; }; U PBiCG { preconditioner DILU; tolerance 1e08; relTol 0; }; k BICCG 1e06 0; epsilon BICCG 1e06 0; R BICCG 1e06 0; nuTilda BICCG 1e06 0; } SIMPLE { nNonOrthogonalCorrectors 1; pRefCell 0; pRefValue 0; } relaxationFactors { p 0.3; U 0.7; k 0.5; epsilon 0.5; } 

July 16, 2008, 14:24 
Very nice Patrice!
And than

#6 
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
Very nice Patrice!
And thanks for posting your solution. Btw, do you have any Cd / Cl results? I'm interested in validation of the turbulent code. Regards, Paulo. 

July 16, 2008, 15:16 
Hey Paulo,
No I haven't cal

#7 
New Member
Patrice Castonguay
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
Hey Paulo,
No I haven't calculated Cl and Cd yet. I will probably do that soon. I'll let you know what are my results. I am now trying to simulate the flow at higher angle of attach but I'm having problems with my boundary conditions (see the thread named: Boundary conditions  Cmesh, high AOA ). If you have any suggestions on how to resolve my problems, I would really appreciate your help. Again thanks for your help Patrice 

July 24, 2008, 23:56 
For anyone interested in analy

#8 
New Member
Patrice Castonguay
Join Date: Mar 2009
Posts: 7
Rep Power: 10 
For anyone interested in analyzing an airfoil with simpleFoam or rhoSimpleFoam, I posted my case folders for a Naca0012 at 2 degrees AOA. Hope this can be useful to people reading this thread. I used the SA model as it proved to improve the convergence significantly.
NACA 0012, Mach 0.2, AOA 2, simpleFoam NACA 0012, Mach 0.5, AOA 2, rhoSimpleFoam 

July 25, 2008, 13:05 
Hi Patrice,
since I'm strug

#9 
Member
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 10 
Hi Patrice,
since I'm struggling with the same kind of problems (although my Ma is 0.75 and the mesh is an ogrid in a square domain) I would like to try your settings. Anyway I'd like to know if you are solving the boundary layer or using wall functions?? thank you in advance dino 

July 25, 2008, 13:07 
ps:
I can't see your mesh o

#10 
Member
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 10 
ps:
I can't see your mesh on this link: "www.stanford.edu/~pcasto2/naca0012_visc/mesh.pdf " the message I get is something like: object not found bye 

August 18, 2008, 08:27 
hI All,
I am working on an

#11 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 10 
hI All,
I am working on an airfoil myself. I am having problems with running the solver icoFoam. I get the following error This mesh contains patches of type empty but is not 1D or 2D by virtue of the fact that the number of faces of this empty patch is not divisible by the number of cells. From function emptyFvPatchField<type>::updateCoeffs() in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 148. But if I execute refineMesh with this file, it shows the mesh as 2D mesh. I have checked my patches individually and they are all correct without any errors. Also, I have not defined any internal face as boundary face. Still I get this error. My checkMesh also, does not give me any error. It is only when I execute icoFoam, I get this error. I cant understand why so? Can anyone suggest any help? Thanks 

August 18, 2008, 16:24 
Have a look at the cavity tuto

#12 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 18 
Have a look at the cavity tutorial  every cell has two faces which are in the empty patch. Count the number of cells and the size of your empty patch. Perhaps you have more than one cell in the third direction?


August 18, 2008, 17:24 
Hi Mattijs
Yeah I have alre

#13 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 10 
Hi Mattijs
Yeah I have already done that. I have 13 blocks or cells as u want to call them. So it should be 26 faces in the empty patch I believe which is also correct in the blockMeshDict file. Also, there are no faces repeated in the empty Patch or any other patch. I am attaching the file, if u can, then please take a look. Thanks blockMeshDict 

August 18, 2008, 18:31 
The problem is due to your mes

#14 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,754
Rep Power: 29 
The problem is due to your mesh generation. As can be seen from the attached picture of your mesh, there are several black lines, which are default faces generated by blockMesh.
The default faces are given empty, but as they are perpendicular to the xy plane, the mesh looks like being 3D for any solver in OF. My guess is that the problem lies within the fact, that you do not have the same number of cells in all the blocks, thus blockMesh does not know how to connect across these nonmatching interfaces and makes it a seperate region. Further in your checkMesh, you are informed that your mesh consists of multiple regions which are not interconnected, but this is merely a warning. / Niels
__________________
Please note that I do not use the Friendfeature, so do not be offended, if I do not accept a request. 

August 19, 2008, 13:51 
hi niels,
first off i cant

#15 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 10 
hi niels,
first off i cant c the black lines in my paraview. my colleague showed them to be discontinuties which i dont think should arise because everypatch is beginning from the vertex of the preceding patches so it should be a continuous faces and should not contain defaultFaces added by OpenFOAM. These defaultFaces are being added at the connection of 2 patches. i do not understand the error for this discontinuity or is it incorrect to define a common vertex in 2 patches. 

August 19, 2008, 13:58 
and yeah i also tried to remov

#16 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 10 
and yeah i also tried to remove the discontinuity by making a successive patch from the penultimate point in the previous patch but it does not seem to help.


August 19, 2008, 15:13 
1. See the attached picture in

#17 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,754
Rep Power: 29 
1. See the attached picture in my previous post for the black lines.
2. If you zoom onto the mesh in paraView, then you will see that the interface between the different blocks have nonmatching nodal points, even though the entire interface patch are perfectly matching. 3. I have been wondering that it actually was succesfully generated by blockMesh, but in the blockMeshfile you will find that you have multiple definition of the points, thus as (point N) = (point M) but you use N in one block and M in the the neighboring block me guess is that they are considered to be noninterconnected. Discard all multiple defined points and make your blocks based on unique point definitions. See the UserGuide for questions on mesh generation using blockMesh. / Niels
__________________
Please note that I do not use the Friendfeature, so do not be offended, if I do not accept a request. 

August 19, 2008, 16:59 
yeah Niels,
I can see the d

#18 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 10 
yeah Niels,
I can see the discontinuity in ur image and the image sent by my colleague. And yes regarding the individual point method, i tried that in the morning, it was good for the airfoil upper chord and lower chord patch but when i tried to attach the gap between the slot and airfoil, i had the same problem of no connectivity. Anyways I can try again tomorrow as the blockMesh is in the office. 

August 20, 2008, 17:23 
HI all,
I tried the unique

#19 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 10 
HI all,
I tried the unique point method but it does not work. The problem is in meshing the gaps arising due to the deflection of the slot. is there anyway to mesh the following in OpenFOAM. i have an edge ABC. from this edge, BC has to form a different patch and AC a different one. i have read the users guide and seen examples in icoFoam and simpleFoam but I cant find anything similar to this. Can some one suggest another software for meshing this. Thanks 

November 6, 2008, 17:46 
I tried the NACA0012 airfoil f

#20 
New Member
Peter Lian
Join Date: Mar 2009
Posts: 12
Rep Power: 10 
I tried the NACA0012 airfoil for incompressible flow using kepsilon model with minor changes on the solver. It seems work for me.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
2D SST Simulation Airfoil  Convergence Problem  Kraemer  CFX  10  April 16, 2011 07:22 
Convergence Criteria  airfoil sim.  Andres Bernal  CFX  2  December 18, 2006 19:57 
3d Airfoil Modelling Problems  Olly  FLUENT  7  March 19, 2006 16:10 
Help! Convergence of Separated Flow on 2D airfoil.  Daniel  FLUENT  2  September 25, 2005 00:24 
when,Ma=0.95,problems of airfoil compution in cfx  zuozicheng  CFX  2  May 25, 2005 07:18 