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

Is it possible to obtain wallY%23601 for an airfoil

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 26, 2008, 12:35
Default Hi foamers, in the last wee
  #1
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
Hi foamers,

in the last weeks I'm struggling with a rae airfoil for which I would like to obtain wall y+ <1. Unfortunately since this requirement is very strong for the mesh generation (the first cell near the wall should be very small) this gave me a lot of problems to get the convergence. Actually in all my trials the continuity error tends to explode, probably driven by the pressure residuals. On the other side when I've tried to modify the mesh in order to using the wall functions, so increasing the wall-adiacent cell size, I got no problems!!
Therefore now I'm asking myself if it possible to reach this objective!
If somebody did something concerning this issue, please help me!
thanks a lot

dino
dinonettis is offline   Reply With Quote

Old   May 26, 2008, 12:56
Default Yes, it should be possible. Wh
  #2
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
Yes, it should be possible. What are you using for mesh generation? To assure you've resolved the boundary layer, you want your first cell distance to be between 10^-5 - 10^-6 of the aerofoil chord with a stretching ratio no greater than 1.2-1.3. Using wall functions is an easy problem since boundary layer resolution is no longer required and your cell quality will be improved. Don't waste your time with wall functions if you can afford to. All major research in wings, rotors, and aircraft has the boundary layer resolved. Anything less than 10 points in there and you can expect to face a lot of scrutiny.

So, can you tell us what solver, turbulence model you were using? What is your cell skewness and general quality like? Has your aerofoil got a blunt trailing edge or does it meet at a point? What mach number are you working at? What angle of attack? We need more information, please.
madad2005 is offline   Reply With Quote

Old   May 26, 2008, 13:35
Default These are the info you require
  #3
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
These are the info you required:


solver: simpleFoam
turbulenceModel: LaunderSharmaKE
near wall cell size: 1e-5
Ma=0.1
Re=1e6
trailing edge: blunt (lenght: 3e-4 m)
angle of attack:2.8

checkMesh
----------------------
Mesh stats
points: 212020
edges: 528678
faces: 421982
internal faces: 209962
cells: 105324
boundary patches: 8
point zones: 0
face zones: 0
cell zones: 1

Number of cells of each type:
hexahedra: 105324
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Topological cell zip-up check OK.
Face vertices OK.
Face-face connectivity OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface
empty1 105324 106010 ok (not multiply connected)
trailing 31 64 ok (not multiply connected)
outlet 229 460 ok (not multiply connected)
bottom 312 626 ok (not multiply connected)
top 312 626 ok (not multiply connected)
wing 259 520 ok (not multiply connected)
inlet 229 460 ok (not multiply connected)
empty2 105324 106010 ok (not multiply connected)

Checking geometry...
Domain bounding box: (-20 -20 0) (20 20 0.001)
Boundary openness (3.98952e-20 -1.72053e-23 1.83245e-14) OK.
Max cell openness = 4.4418e-14 OK.
Max aspect ratio = 992.012 OK.
Minumum face area = 1.00474e-10. Maximum face area = 0.182054. Face area magnitudes OK.
Min volume = 1.00474e-13. Max volume = 0.000182054. Total volume = 1.59992. Cell volumes OK.
Mesh non-orthogonality Max: 89.6288 average: 35.0138
*Number of severely non-orthogonal faces: 32206.
Non-orthogonality check OK.
<<Writing 32206 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 2.4549 OK.
*Edges too small, min/max edge length = 1.1e-06 0.4924, number too small: 20938
<<Writing 20078 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.

Mesh OK.
-----------------------------

Iteration Trend
--------------------
Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.82607e-07, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.78752e-07, No Iterations 1
GAMG: Solving for p, Initial residual = 1, Final residual = 0.00956934, No Iterations 65
GAMG: Solving for p, Initial residual = 0.0961131, Final residual = 0.000860428, No Iterations 29
GAMG: Solving for p, Initial residual = 0.171639, Final residual = 0.00170798, No Iterations 21
time step continuity errors : sum local = 0.000365398, global = -0.000104773, cumulative = -0.000104773
DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 1.38442e-06, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 1.46551e-06, No Iterations 1
ExecutionTime = 7.3 s ClockTime = 7 s

Time = 2

DILUPBiCG: Solving for Ux, Initial residual = 0.0437159, Final residual = 1.27017e-05, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.104176, Final residual = 2.99386e-05, No Iterations 1
GAMG: Solving for p, Initial residual = 0.748567, Final residual = 0.00722813, No Iterations 34
GAMG: Solving for p, Initial residual = 0.331249, Final residual = 0.00324074, No Iterations 20
GAMG: Solving for p, Initial residual = 0.497473, Final residual = 0.00428006, No Iterations 21
time step continuity errors : sum local = 0.00220773, global = 0.00049871, cumulative = 0.000393937
DILUPBiCG: Solving for epsilon, Initial residual = 0.0525692, Final residual = 2.73007e-14, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.300619, Final residual = 1.4153e-06, No Iterations 1
ExecutionTime = 10.98 s ClockTime = 11 s

-
-
-
-

Time = 29

DILUPBiCG: Solving for Ux, Initial residual = 0.966284, Final residual = 2.5783e-08, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.929986, Final residual = 2.1638e-08, No Iterations 1
GAMG: Solving for p, Initial residual = 0.999977, Final residual = 0.00487312, No Iterations 4
GAMG: Solving for p, Initial residual = 2.33007e-23, Final residual = 2.33007e-23, No Iterations 0
GAMG: Solving for p, Initial residual = 2.33007e-23, Final residual = 2.33007e-23, No Iterations 0
time step continuity errors : sum local = 5.45356e+64, global = 1.3964e+48, cumulative = 1.3964e+48
DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 0.000757565, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.000583767, No Iterations 1
ExecutionTime = 46.32 s ClockTime = 47 s

Time = 30

DILUPBiCG: Solving for Ux, Initial residual = 0.12179, Final residual = 1.03215e-09, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.119747, Final residual = 2.03625e-10, No Iterations 1
GAMG: Solving for p, Initial residual = 4.51096e-12, Final residual = 4.51096e-12, No Iterations 0
GAMG: Solving for p, Initial residual = 3.99327e-12, Final residual = 3.99327e-12, No Iterations 0
GAMG: Solving for p, Initial residual = 3.99327e-12, Final residual = 3.99327e-12, No Iterations 0
time step continuity errors : sum local = 4.86914e+49, global = -7.4534e+36, cumulative = 1.3964e+48
#0 Foam::error::printStack(Foam:stream&) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::multiply(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::tmp<foam::geometricfield<double,> > Foam::operator*<foam::fvpatchfield,>(Foam::tmp<foa m::geometricfield<double,> > const&, Foam::GeometricField<double,> const&) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libincompressibleTurbu lenceModels.so"
#5 Foam::turbulenceModels::LaunderSharmaKE::correct() in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libincompressibleTurbu lenceModels.so"
#6 main in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoa m"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 Foam::regIOobject::readIfModified() in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoa m"
Errore di virgola mobile
-------------------------------------
If you need any other detail, please tell me!
thanks

dino
dinonettis is offline   Reply With Quote

Old   May 28, 2008, 04:25
Default Hi Dino, Did you manage to
  #4
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
Hi Dino,

Did you manage to get this working? Sorry for taking so long to reply. I looked at your output and a couple of things caught my eye. Firstly, why is your AMG residuals appearing three times? I thought this was only required once? Have you tried using the k-w (Wilcox or SST) and seeing if you have the same problem? Try it inviscid and see if the same problem persists.

Secondly, I notice you are running at a very low Mach number. I'm not sure what type of preconditioning is used, but maybe that could be a problem. Try upping your Mach number to 0.3 and see if the problem still occurs. Thirdly, what is your mesh quality like close to the wall, especially at the trailing-edge? High skewness at the leading edge and trailing-edge can cause you a world of problems. The blunt trailing-edge can also give some issues with convergence. It might be an idea to retry it with your trailing-edge defined at a point.

Let me know how you get on.
madad2005 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
How to obtain forces Karimu FLUENT 2 August 22, 2005 17:26
Compressible flow with inlet velocity Ma%23601 klaus OpenFOAM Running, Solving & CFD 2 July 3, 2005 15:43
HELP - How to obtain numerical values Ravi FLUENT 3 February 16, 2003 11:18
How to obtain.... Sharad Dugad FLUENT 6 February 13, 2002 13:14
how to obtain a profile ... olivier FLUENT 2 December 13, 2001 07:21


All times are GMT -4. The time now is 06:53.