|
[Sponsors] |
March 24, 2011, 05:42 |
Test-case NLF-414 airfoil
|
#1 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
Hi,
i'm making a study of a nlf-414 airfoil with simpleFoam, k-omegaSST turbulence model. I have a problem with convergence of results. after a low number of iteration steps my solution diverges. i've tried a lot of possibilities for fvschemes and fvsolution, but nothing!!!! this is my case please help me!!!!fvSchemes.txt fvSolution.txt controlDict.txt checkMesh.txt log.txt |
|
March 24, 2011, 06:58 |
|
#2 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 555
Rep Power: 27 |
Hi just to make it easier a plot of the residuals. And it really does not look right.
Could you post a plot of your mesh? According to the checkMesh you have some nonOrthogonal faces, these are usually not an issue for aerofoil simulations since the mesh near surface can be very elongated. One issue I see is that the mesh is very big ~60 by ~60 meters and Max aspect ratio = 818.404. This seems quite extreme for only 73728 cells. I think this could be the cause. Also try switching U to upwind in the fvSchemes file just to eliminate that also.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
March 24, 2011, 07:20 |
|
#3 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
hi linnemann.
may i reduce the dimensions of my grid?? and how can i do it?? i need to resolve this problem. i use this gird also in fluent but i have no problem! p.s. how can you make the story of convergence?? |
|
March 24, 2011, 07:27 |
|
#4 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 555
Rep Power: 27 |
You can only scale the mesh but I do not know the dimensions of your geometry. If is is a Boing 747 wing you are simulating 60x60meters makes sense but if the wing is only 1m long 60x60 seems a bit excessive.
So give us some geometry dimensions for the wing, and a closeup of the mesh near the wing, this will make it easier to help you. convergence http://www.cfd-online.com/Forums/ope...residuals.html
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
March 24, 2011, 07:39 |
|
#5 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Quote:
My advice is to find a setup that guarantees solution stability with a smaller airfoil domain (20 chords is ok) and then improve accuracy increasing domain dimension. mad |
||
March 24, 2011, 08:11 |
|
#6 | |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 555
Rep Power: 27 |
Quote:
Then take a look at the mesh in that area. Possibly make a the nonOrthogonal faceset into a VTK file you can open in paraview and see where these cells are located in the mesh. (foamToVTK -faceSet nonOrthoFaces) EDIT: Arhhh it is a 2D mesh :-), then 70k seems about right.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
||
March 24, 2011, 08:26 |
|
#7 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
is there anyone interested to study my mesh?? i can bring it by email. this could be resolve the problem faster, because i have no idea for resolve it
|
|
March 24, 2011, 08:40 |
|
#8 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 555
Rep Power: 27 |
Do you have a dropbox account then you can have the files public available only providing a download link and you get 2Gb for free.
Otherwise pm me and I will give you my mail.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
March 24, 2011, 08:48 |
|
#9 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Quote:
as suggested here why do not you try simpleFoamResiduals? mad Last edited by maddalena; March 25, 2011 at 07:30. Reason: added link |
||
March 25, 2011, 06:44 |
|
#10 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 555
Rep Power: 27 |
Hi
Had a first look on the case and after just 10 itterations the flowfield looks like this. Also you have an initial guess on U, what is the inlet velocity for the case?
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
March 25, 2011, 06:52 |
|
#11 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
hi, linnemann. i was just sending you an email!!
maybe i resolved the problem. i changed my mesh, using gambit. now i have better results with the same conditions of the other case. i thinked that this would be the faster way to resolve the problem . thank you very very much to you and to maddalena |
|
March 25, 2011, 07:13 |
|
#12 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 555
Rep Power: 27 |
Hi
Yes my conclusion is also the mesh. The first picture shows a thin stretch of cells which is the nonorthofaces and the next picture is where the case start diverging. And this just happens to be next to these nonorthofaces.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
March 25, 2011, 07:28 |
|
#13 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
that's very interestring!!! but the other thing is that in Fluent i haven't these problem. so we may say that OF is more "sensible" with the mesh quality
|
|
March 25, 2011, 17:27 |
|
#14 |
Senior Member
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 18 |
Could be a conversion error. Did you already set writeFormat to binary when converting the fluent mesh to polyMesh format?
I had similar issues with airfoil simulations using a fluent mesh which worked flawlessly in fluent. Setting writeFormat to binary solved the problem. Greetings, Felix. |
|
March 26, 2011, 05:55 |
|
#15 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
Hello world!! I have a question for you. I'm studying the case of my airfoil with a Mach Number=0.12. So I have in the controlDict magUinf=41.651 and a value of nu in transportProperties of 0.000004171 (to put the Reynolds Number to 10*10^6). Now my question is: which value of nut (kOmegaSST turbulence model) i have to put???In other word is there a ralation between the value of nu(the "laminar" viscosity) and nut???
thank you very much, in this forum i'm learnig a lot of things!!! |
|
March 30, 2011, 08:49 |
|
#16 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
Hi i have a question.
if i have m=0.12 e re=10*10^6 wich value of nut,k and omega i have to put?? could you give me an example??? |
|
April 1, 2011, 02:04 |
|
#17 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
hi. i have a problem. when i plot the cp of my airfoil with the sampleDict, i have a strange behavior on the trailing edge.
could you help me??? it seems that it is not respected the equal pressure coefficient on the T.E. |
|
April 1, 2011, 10:19 |
|
#18 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
1st foto of the airfoil
|
|
April 1, 2011, 10:20 |
|
#19 |
Member
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 15 |
the other 2 foto of the TE
|
|
November 14, 2012, 19:28 |
|
#20 |
Member
Zifei Yin
Join Date: Sep 2012
Location: Shanghai & Ames
Posts: 33
Rep Power: 13 |
Hi, linnemann how can I visualize the nonorthofaces?
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Large test case for running OpenFoam in parallel | fhy | OpenFOAM Running, Solving & CFD | 23 | April 6, 2019 09:55 |
Example subsonic airfoil case | doug | OpenFOAM Running, Solving & CFD | 1 | September 9, 2010 17:24 |
oscillating airfoil test case | Akbar | FLUENT | 0 | July 15, 2005 06:49 |
Durham test case | SAM | FLUENT | 0 | August 16, 2004 05:01 |
c1 body test case | Eric Lenormand | Main CFD Forum | 0 | March 2, 2000 06:54 |