CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Test-case NLF-414 airfoil (http://www.cfd-online.com/Forums/openfoam/86506-test-case-nlf-414-airfoil.html)

salvoblack March 24, 2011 06:42

Test-case NLF-414 airfoil
 
5 Attachment(s)
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!!!!Attachment 7009

Attachment 7010

Attachment 7011

Attachment 7012

Attachment 7013

linnemann March 24, 2011 07:58

1 Attachment(s)
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.

salvoblack March 24, 2011 08:20

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?? :)

linnemann March 24, 2011 08:27

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

maddalena March 24, 2011 08:39

Quote:

Originally Posted by linnemann (Post 300872)
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 http://www.cfd-online.com/Forums/ope...gh-drag-2.html (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

linnemann March 24, 2011 09:11

Quote:

Originally Posted by maddalena (Post 300873)
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 http://www.cfd-online.com/Forums/ope...gh-drag-2.html (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.

salvoblack March 24, 2011 09:26

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

linnemann March 24, 2011 09:40

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.

maddalena March 24, 2011 09:48

Quote:

Originally Posted by linnemann (Post 300877)
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

linnemann March 25, 2011 07:44

1 Attachment(s)
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?

salvoblack March 25, 2011 07:52

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 :) :)

linnemann March 25, 2011 08:13

2 Attachment(s)
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.

salvoblack March 25, 2011 08:28

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

FelixL March 25, 2011 18:27

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.

salvoblack March 26, 2011 06:55

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 March 30, 2011 08:49

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 April 1, 2011 02:04

1 Attachment(s)
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.

salvoblack April 1, 2011 10:19

1 Attachment(s)
1st foto of the airfoil

salvoblack April 1, 2011 10:20

2 Attachment(s)
the other 2 foto of the TE

yzf1215 November 14, 2012 20:28

Hi, linnemann how can I visualize the nonorthofaces?


All times are GMT -4. The time now is 16:35.