
[Sponsors] 
August 24, 2007, 06:27 
ooops.. it seems we was writin

#21 
Member
Rosario Russo
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 56
Rep Power: 8 
ooops.. it seems we was writing at the same time :)
Just another question: at the solid face what kind of cell elements do you have? It would be recommendable to have prisms there, particularly if you are trying to model boundary layer. Try also in laplacian schemes to use linear limited (0.5 for instance), or not to correct laplacian term at all and see what happen; this is useful if your grid doesn't have good orthogonality (you should be able to achieve convergence at least). Yes it would be interesting to look at your case, but you should post also the mesh... Good luck. Rosario 

August 24, 2007, 08:27 
Hmmm, very interesting, Rosari

#22 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hmmm, very interesting, Rosario you made me find something.
I have two computers here, one with OpenFoam 1.4 and one with openfoam 1.4.1. My mesh is generated with GridPro (so hexa multiblock). Then to use OpenFOAM I create three meshes with GridPro2FOAM, one coarse, one medium and one fine. When I run OpenFOAM either 1.4 or 1.4.1 on the coarse mesh, well everything's fine. Running the medium mesh (with starting conditions mapped from coarse mesh) my computation is blowing up with 1.4.1 and not with 1.4!!! Strange... So I was wondering whether something would have changed between those two versions? Unfortunately I can't post my case since it weights few hundreds of Mo. Vincent 

August 24, 2007, 10:34 
I have been using Fluent for r

#23 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
I have been using Fluent for racing car (NASCAR) applications for past several years. Steady state RANS solver (simpleFoam type algorithm) seems to give reasonable predictions for drag. Lift is not as good. Speeds are similar to the ones you are trying. Few details of process:
1. Prism layers on exterior surfaces 2. Realizable KE turbulence model 3. Refinement in the wake area and other interesting regions. PS: I have also recently started playing with OpenFoam and currently setting it up for 20 deg Ahmad model. 

August 24, 2007, 10:53 
This is very interesting Rajne

#24 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
This is very interesting Rajneesh since my model has also a 20deg angle.
Would be great if you could tell me what kind of results you obtain with simpleFoam and eventually settings you are using. With these informations I'll be able to see if my problems come from my mesh or something else. Vincent 

September 5, 2007, 02:59 
Hi Rajneesh,
What kind of m

#25 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi Rajneesh,
What kind of mesh generator are you using your race cars? Are you going to use the same in OpenFOAM? And did you get some results on the ahmed bluff body? Thanks in advance. Vincent 

September 5, 2007, 22:01 
I use Fluent/Tgrid/Ansa at my

#26 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
I use Fluent/Tgrid/Ansa at my work for CFD simulations.
I have used Tgrid ( Prism layers on body + Tetra) to create symmetric half and full models of Ahmed body of 12.5 and 30 deg. I came across the original paper of Ahmed and the paper has some flow viz data for these two shapes. So I am going to focus on these two models. I have got some numbers for ~0.5 mill elements model (looks reasonable) but I will be upgrading my computer next week to run ~2Mill models. I will compare Fluent/OF/test after that. thanks  Rajneesh 

September 6, 2007, 23:34 
12.5 Deg Half model results wi

#27 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
12.5 Deg Half model results with openFoam (model size ~0.6 Mill)
Pressure Drag: 0.189 Viscous Drag: 0.006!! Pressure drag is very close to the experimental numbers and the Fluent's prediction with ~3 Mill elements full model. (BTW Fluent got exactly same number as the Ahmed's test after applying continuity correction. Test section had a blockage of ~4%. I was really shocked/surprised at this perfect match. I will know tomorrow on what happens for 30deg Ahmed model.) OpenFoam's Viscous drag is definitely incorrect. It should of order of ~0.04. I need to double check the LiftDrag utility (thanks Srini & Bos) and my model to make sure there are no errors in computing viscous drag. If anyone needs this mesh to play for external Aero simulations, let me know. 

September 7, 2007, 00:02 
looks like contribution from t

#28 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
looks like contribution from the turbulence are not
added to the viscous drag. I think I need to compute turbDragCoefficient as well. If this correct, can anyone please explain the first argument of this function? turbDragCoefficient ( const autoPtr<foam::turbulencemodel>& turbulence, const volVectorField& U, const volScalarField& p, const dimensionedScalar& mu, const word& patchName, const vector& Uinf, const scalar& Aref ); thanks  Rajneesh 

September 7, 2007, 00:19 
Rajneesh,
I have performed

#29 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 700
Rep Power: 12 
Rajneesh,
I have performed validations with Fluent for incompressible laminar unsteady/steady flow using the adapted version of the liftDrag utility originally compiled by Frank Bos. It works very nicely and gives accurate results. A few weeks ago, Frank raised a concern on how accurate the pressure and viscous contributions are when calculated using the adapted liftDrag routines. To answer that question, I started a validation test with a journal article. Preliminary observations show that OpenFOAM does give the correct lift/Drag coefficients. I will post the results shortly. 

September 7, 2007, 02:41 
Hi everybody,
Rajneesh, you

#30 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi everybody,
Rajneesh, your results look great, at least for the pressure drag. That's a good begening. Could I know a bit more about your configuration:  which solver are you using?  which turbulence model?  do you check the mesh convergence? I mean, doing coarse, medium and fine mesh computations or you only use one mesh? The best to understantd the differences between your computation and mine would be to have access to your mesh or even better the test case implementation. I don't know if it's possible for you? I think it's a good thing if we succeed in getting results on this test case, it would be one more validation of OpenFOAM capacities. Vincent 

September 7, 2007, 10:38 
Hi Rajneesh,
I would be int

#31 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 473
Rep Power: 11 
Hi Rajneesh,
I would be interested in that mesh or better the OF model to play around with it. Could you send it to me, please? The differences in viscous drag are strange, maybe I can take a look at it. Thanks Basti 

September 7, 2007, 16:26 
Srini,
As far as I could fi

#32 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
Srini,
As far as I could figure out from liftDrag.C, viscous drag is computed separately from laminar and turbulent viscosity. I am not getting the contributions from the turbulent viscosity as yet. I hope case you are trying out is for turbulent flow case. Vincent, BastiL I will tar/zip files over this weekend and upload it here or on the website mentioned in my profile. I am using simpleFoam at conditions similar to the Ahmed's experiment.  Rajneesh 

September 7, 2007, 16:30 
You are correct. However my co

#33 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 700
Rep Power: 12 
You are correct. However my computations are for laminar flows. For turbulent flows you need to include the contribution from turbulent viscosity.


September 10, 2007, 08:52 
Hi everybody,
It looks like

#34 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi everybody,
It looks like the liftDrag tool I'm using is not computing my turbulent viscosity part neither. On a rotating wheel I get lower values for turbulent case with respect to laminar case, which is a bit strange. Which is currently the best (taking everything into account) liftDrag tool available for OF 1.4? Thanks in advance. 

September 11, 2007, 05:20 
Hi all,
I a mdoing simular

#35 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 473
Rep Power: 11 
Hi all,
I a mdoing simular tests on a more realistic body. I am struggling how to setup BC for simpleFoam. How can I define the rotating wheels? In my eyes this is a rotating wall BC? Thanks 

September 11, 2007, 05:37 
Hi BastiL,
I am using a too

#36 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi BastiL,
I am using a tool name rotationBC posted on this message board by a foam user. Actually, you set up a wall condition on your wheel, and rotationBC is going to compute a non uniform field to put in the bc file for U. You can find the code in this thread: http://www.cfdonline.com/OpenFOAM_D...es/1/4473.html Which software are you going to use for the mesh? Which reference are you going to take to compare with? I would be really interested in comparing our results if you want. Regards, Vincent Vincent 

September 11, 2007, 11:26 
This is a mesh converted from

#37 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 473
Rep Power: 11 
This is a mesh converted from proSTAR using ccm26ToFoam. This went fine. I skipped rotating boundaries and started with simple walls. I can not get simpleFoam running. After few iterations residuals get very low but continutiy errors are very high. Foam struggles with an floating point error afterwards. I tried to play with nonothoganal correctors an relaxation but without success so far. Checkmesh reports few nonortoganals and skews. What can I do next?
I am going to compare with STAR which runs without problems on this mesh. Comparing results is difficult for me, sorry. I guess I am doing something wrong with simplefoam, please help. Thanks. 

September 11, 2007, 16:28 
Hi Bastil,
Looks like OpenF

#38 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi Bastil,
Looks like OpenFOAM really doesn't like skewed or non orthogonal meshes. For the ahmed body, I have two different meshes, one passing checkMesh without problem and one reporting some bugs like yours, and simpleFoam fails on the last one with the same results as you have on the wheel. I guess this is comming from some cell skewness. Your problem may be the same. However I also noticed differences in stability between OpenFOAM 1.4 and 1.4.1, version 1.4 being suprisingly the more stable. I still don't have any answer on this differences but if you are using OF 1.4.1 so far, you may try OF 1.4 just to check if it's going better. However I'm not an OpenFOAM specialist, and other people may know beeter solutions to your problem. Hope that helped, let me know. Vincent 

September 11, 2007, 18:37 
Rajneesh and Vincent
I' m a

#39 
New Member
marco
Join Date: Mar 2009
Posts: 3
Rep Power: 8 
Rajneesh and Vincent
I' m able to calculate turbDragCoefficient only modifying the simpleFoam code as the example posted in this forum for turbFoam (search "turbFoam_1"), but with two adds: 1 adding to the local liftDrag.H file the definition and the code of turbDragCoefficient from the original OpenFoam liftDrag.C and liftDrag.H files 2 adding to the local computeForces.H also the call to turbDragCoefficient, adding as first argument simply turbulence (before U). I needed also to change in createFields.H the word PISO to SIMPLE, bur only because I apply these modification to simpleFoam and not to turbFoam. Surely should be possible to modify the original liftDrag utility, but I'm not expert of C++ and I' m not be able to find which is the error if I apply the modification 2 directly to the original liftDrag utility. The drag and lift with turbulent contribution seem to me reasonables, but I've not yet verify the results with some test case. Regards 

September 11, 2007, 23:42 
Vincent, BastiL,
I have not

#40 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
Vincent, BastiL,
I have not been able to upload the whole Ahmad mesh model to my googlepage site. Its about 20Mb after gzipping. I am not sure if uploading such a huge file to this forum is possible or considered polite Here is rest of stuff from openFoam setup for this problem for simpleFoam solver http://aertheos.googlepages.com/ahma...efoamsetup.gz thanks  Rajneesh 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
3d test case  Hassan Raiesi  Main CFD Forum  1  August 19, 2006 12:33 
Test Case  ganesh  Main CFD Forum  0  March 16, 2006 13:34 
Looking for test case  William M.  Main CFD Forum  2  May 26, 2005 03:45 
test case?  lsm  Main CFD Forum  0  June 14, 2004 11:39 
test case  Follet  Main CFD Forum  0  July 8, 2002 04:07 