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

Test-case NLF-414 airfoil

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 24, 2011, 06:42
Default Test-case NLF-414 airfoil
  #1
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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
salvoblack is offline   Reply With Quote

Old   March 24, 2011, 07:58
Default
  #2
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 439
Rep Power: 13
linnemann will become famous soon enough
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.
Attached Images
File Type: jpg residu.jpg (28.5 KB, 40 views)
__________________
Linnemann

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

Old   March 24, 2011, 08:20
Default
  #3
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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??
salvoblack is offline   Reply With Quote

Old   March 24, 2011, 08:27
Default
  #4
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 439
Rep Power: 13
linnemann will become famous soon enough
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 Tutorial of how to plot residuals !
__________________
Linnemann

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

Old   March 24, 2011, 08:39
Default
  #5
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 11
maddalena is on a distinguished road
Quote:
Originally Posted by linnemann View Post
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.
How long is your chord? 1 meter? if so, 60x60 is not eccessive. I experienced that cl and cd may vary if the domain is as far as 100 chords, see post 33 on Naca airfoil with too high drag (read everything, there are some nice observations for you). In any case, this did not change the solution convergence.
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
maddalena is offline   Reply With Quote

Old   March 24, 2011, 09:11
Default
  #6
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 439
Rep Power: 13
linnemann will become famous soon enough
Quote:
Originally Posted by maddalena View Post
How long is your chord? 1 meter? if so, 60x60 is not eccessive. I experienced that cl and cd may vary if the domain is as far as 100 chords, see post 33 on Naca airfoil with too high drag (read everything, there are some nice observations for you). In any case, this did not change the solution convergence.
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
I agree that it is not excessive but for 70k cells this seems like a rather big domain. I propose that you write out the results for each iteration and then try and locate where in the mesh the simulation blows up in paraview.
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.
linnemann is offline   Reply With Quote

Old   March 24, 2011, 09:26
Default
  #7
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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
salvoblack is offline   Reply With Quote

Old   March 24, 2011, 09:40
Default
  #8
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 439
Rep Power: 13
linnemann will become famous soon enough
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.
linnemann is offline   Reply With Quote

Old   March 24, 2011, 09:48
Default
  #9
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 11
maddalena is on a distinguished road
Quote:
Originally Posted by linnemann View Post
propose that you write out the results for each iteration and then try and locate where in the mesh the simulation blows up in paraview.
Salvo,
as suggested here why do not you try simpleFoamResiduals?

mad

Last edited by maddalena; March 25, 2011 at 08:30. Reason: added link
maddalena is offline   Reply With Quote

Old   March 25, 2011, 07:44
Default
  #10
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 439
Rep Power: 13
linnemann will become famous soon enough
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?
Attached Images
File Type: png weird.png (11.2 KB, 53 views)
__________________
Linnemann

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

Old   March 25, 2011, 07:52
Default
  #11
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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
salvoblack is offline   Reply With Quote

Old   March 25, 2011, 08:13
Default
  #12
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 439
Rep Power: 13
linnemann will become famous soon enough
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.
Attached Images
File Type: jpg nonortho.jpg (12.7 KB, 52 views)
File Type: jpg nonortho2.jpg (15.5 KB, 47 views)
__________________
Linnemann

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

Old   March 25, 2011, 08:28
Default
  #13
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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
salvoblack is offline   Reply With Quote

Old   March 25, 2011, 18:27
Default
  #14
Senior Member
 
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 8
FelixL is on a distinguished road
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.
FelixL is offline   Reply With Quote

Old   March 26, 2011, 06:55
Default
  #15
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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!!!
salvoblack is offline   Reply With Quote

Old   March 30, 2011, 08:49
Default
  #16
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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???
salvoblack is offline   Reply With Quote

Old   April 1, 2011, 02:04
Default
  #17
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
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.
Attached Images
File Type: jpg cpalfaturb.jpg (50.2 KB, 29 views)
salvoblack is offline   Reply With Quote

Old   April 1, 2011, 10:19
Default
  #18
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
1st foto of the airfoil
Attached Images
File Type: jpg Schermata-1.jpg (45.4 KB, 32 views)
salvoblack is offline   Reply With Quote

Old   April 1, 2011, 10:20
Default
  #19
Member
 
Join Date: Oct 2010
Location: Naples
Posts: 50
Rep Power: 6
salvoblack is on a distinguished road
the other 2 foto of the TE
Attached Images
File Type: jpg Schermata.jpg (37.7 KB, 31 views)
File Type: jpg Schermata-2.jpg (34.4 KB, 22 views)
salvoblack is offline   Reply With Quote

Old   November 14, 2012, 19:28
Default
  #20
Member
 
Zifei Yin
Join Date: Sep 2012
Location: Shanghai & Ames
Posts: 31
Rep Power: 4
yzf1215 is on a distinguished road
Hi, linnemann how can I visualize the nonorthofaces?
yzf1215 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
Example subsonic airfoil case doug OpenFOAM Running, Solving & CFD 1 September 9, 2010 17:24
Large test case for running OpenFoam in parallel fhy OpenFOAM Running, Solving & CFD 22 September 22, 2009 11:13
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


All times are GMT -4. The time now is 14:39.