
[Sponsors] 
February 25, 2008, 16:31 
It's a grid I made some time a

#41 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 9 
It's a grid I made some time ago because at the moment I don't have a good software. Howerver the geometry is very simple.
Tonight I'm iterating with HRV's settings, tomorrow I'll check if the solution is more realistic of that I got with the other settings. 

February 27, 2008, 12:46 
Would any of you have access t

#42 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 82
Rep Power: 9 
Would any of you have access to 3dmodels of real cars you could spare? Something I could find Cd and Cl figures on?
I'd like to compare results to experimental data. 

February 29, 2008, 18:34 
Hallo,
I made 2000 iteration

#43 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 9 
Hallo,
I made 2000 iteration with HRV's settings, starting from the previous solution. Now the flow field is realistic, completely different from what I had obteined with the other settings. But the CD I calculated with liftDrag is 0.367: too high! Has anyone obtained a better result? What schemes and solvers could I try? 

March 1, 2008, 03:08 
Hi,
In my not quite converg

#44 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 82
Rep Power: 9 
Hi,
In my not quite converged but Cd and Cl quite stable results realizableKE give a Cd of 0.45 and Cl 0.3. kOmegaSST gives Cd 0.36 and Cl 0.28. As the car is imaginary I don't have anything to compare it to but the realizableKE seems high. kOmegaSST might be in the ballpark, or close enough not to be able to tell if it's wrong. I'm using prisms 120mm from the surface and tetras elsewhere. I've tried to use V2F but I'm having great trouble with my y+ ~ 1 mesh. Not least due to memory limitations of my computer's memory but also lacking any convergence. The pressure problem was solved by increasing the size of the domain. I'm now using a volume of about 25x5x5m which gives a blockage ratio of 4%. 

March 1, 2008, 07:52 
Added turbulent drag to the so

#45 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 82
Rep Power: 9 
Added turbulent drag to the solver and iterated some more with the kOmegaSST:
pressureDragCoefficient = 0.357712 viscDragCoefficient = 0.00803725 turbCoefficient = 0.021208 turbDragCoefficient = 0.386957 LiftCoefficient = 0.2582 

March 25, 2008, 06:27 
Dear users,
we are going to

#46 
Member
Tommaso Lucchini
Join Date: Mar 2009
Posts: 83
Rep Power: 9 
Dear users,
we are going to organize a session about OpenFOAM developments and applications in the Automotive field at the next OpenFOAM workshop (www.openfoamworkshop.org), which will be held in Milano, 1011 July 2008. Among the possible subjects, we encourage presentations in the area of car aerodynamics, since there is a lot of interest for it. In the typical "workshop spirit", also presentations on open problems and/or with preliminary results are welcome. People interested to make a presentation can send an abstract by email to me or to the other session organizers of the Automotive session. The deadline is on the 31st March. Best Regards, Tommaso 

April 8, 2008, 05:26 
Hi everybody,
Still working

#47 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 10 
Hi everybody,
Still working on the topic I'd like to know if other people are getting result with the ahmed body for instance. If it's the case, would it be possible to know the schemes and turbulence models you are using? Tommaso, is it possible to have access to the abstract of people presenting at the workshop? Titles on the website look interesting and I would like to know a bit more about some of them. Regards, Vincent 

February 18, 2009, 10:36 
Dear all,
Like many on the

#48 
Senior Member

Dear all,
Like many on the forum, I am investigating the flow for the Ahmed body. Currently investigating various turbulence models for the 35 degree slant angle case. With the kOmegaSST I am getting results which look reasonable, however I am questioning the amount of iterations I need for convergence. Using simpleFoam I start with 300 iterations using Gauss upwind as suggested on the forum for my convective terms. I then switch to second order (limitedUpwind for turbulence, Gamma 0.2 for velocity). After 6000 iterations, my forces are not yet converged, as can be seen from the image attached. For clarification, the first 500 iterations are truncated, so it runs to 5500. In the first 500 iterations, there are some oscillations and high values, which dissapear rather quickly, but from then convergence is very slow. My fvSchemes for the latter part of the iterations looks like: ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) cellLimited Gauss linear 1.0; } divSchemes { default none; div(phi,U) Gauss GammaV 0.2; div(phi,k) Gauss linearUpwind cellLimited Gauss linear 1; div(phi,omega) Gauss linearUpwind cellLimited Gauss linear 1; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear limited 0.7; laplacian((1A(U)),p) Gauss linear limited 0.7; laplacian(DkEff,k) Gauss linear limited 0.7; laplacian(DomegaEff,omega) Gauss linear limited 0.7; laplacian(1,p) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default limited 0.7; } fluxRequired { default no; p; } While my fvSolution is as: solvers { p GAMG { tolerance 1e06; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; }; U smoothSolver { smoother GaussSeidel; nSweeps 1; tolerance 1e8; relTol 0.1; }; k smoothSolver { smoother GaussSeidel; nSweeps 1; tolerance 1e8; relTol 0.1; }; omega smoothSolver { smoother GaussSeidel; nSweeps 1; tolerance 1e8; relTol 0.1; }; } SIMPLE { nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; } relaxationFactors { p 0.3; U 0.7; k 0.7; omega 0.7; } PISO { nCorrectors 2; nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; } To be complete, checkMesh gives as output: Mesh stats points: 1726824 faces: 15463989 internal faces: 15147131 cells: 7343044 boundary patches: 12 point zones: 0 face zones: 0 cell zones: 0 Number of cells of each type: hexahedra: 0 prisms: 1237404 wedges: 0 pyramids: 1540 tet wedges: 0 tetrahedra: 6104100 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology body_top 14666 7543 ok (nonclosed singly connected) body_front 9357 4807 ok (nonclosed singly connected) body_bottom 18400 9499 ok (nonclosed singly connected) body_slant 4413 2310 ok (nonclosed singly connected) body_base 5116 2685 ok (nonclosed singly connected) body_struts 1500 799 ok (nonclosed singly connected) body_side 26563 13581 ok (nonclosed singly connected) tunnel_road 101873 51568 ok (nonclosed singly connected) tunnel_inlet 1713 1042 ok (nonclosed singly connected) tunnel_infinity 10052 5508 ok (nonclosed singly connected) tunnel_outlet 3088 1730 ok (nonclosed singly connected) tunnel_symmetryplane120117 66275 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (4.176 5.46623e12 0) (7.308 3.3265 3.3265) Mesh (nonempty) directions (1 1 1) Mesh (nonempty, nonwedge) dimensions 3 Boundary openness (1.43894e17 5.86639e15 1.04078e15) OK. Max cell openness = 5.96728e16 OK. Max aspect ratio = 12.1381 OK. Minumum face area = 7.52672e08. Maximum face area = 0.0367279. Face area magnitudes OK. Min volume = 1.12097e11. Max volume = 0.00212606. Total volume = 99.7353. Cell volumes OK. Mesh nonorthogonality Max: 67.1824 average: 16.1836 Nonorthogonality check OK. Face pyramids OK. Max skewness = 2.47713 OK. Mesh OK. I was wondering if anyone has a suggestion to speed up convergence, or do others have similar amounts of iterations until convergence? Obviously there are also some oscillations in the forces, could this indicate too severe unsteady behavior for the steady state solver, or should these damp out as well? Any experience and comments would be welcome and appreciated. Kind regards, Tom Fahner 

February 18, 2009, 11:50 
Dear Tom,
in my experience

#49 
Member
Luca Gasparini
Join Date: Mar 2009
Location: Italy
Posts: 37
Rep Power: 9 
Dear Tom,
in my experience Gamma with a value much less than 1 is not very stable. The "Gauss linearUpwind..." scheme is quite more expensive than Gamma X, so unless you really noticed an improvement I would use Gamma on the turbulence fields as well. Although at convergence it should make no difference, you may try using 1 or 2 nNonOrthogonalCorrectors to add robustness and maybe speedup convergence (in terms of iteratin count), since although your grid quality is high you still have quite some non orthogonality. Finally, given the large separation area do not necessarily expect a convergence to a steady state; a kind of oscillating wake is likely to occur. Regards, Luca 

February 19, 2009, 06:08 
Dear Luca,
Thank you for yo

#50 
Senior Member

Dear Luca,
Thank you for your reply. I have been experimenting in 2D at first and found that Gamma did not behave stable for the turbulence, while with linearUpwind I had a bit more succes. So therefore I adapted to that scheme. I will try out Gamma there. I will also try adding some nonorthogonal correctors. Thanks again. Regards, Tom 

April 3, 2009, 16:26 

#51 
Senior Member

Tom,
I think you could relax the tolerance on P and you would observe a quicker convergence. Regards, Louis 

June 9, 2009, 00:15 
CFD for car

#52 
New Member

Hi, I am newbie in CFD,. wanna ask about the best domain to simulate flows around the car. (length behind, above, beside).ALso, how small the grid close to the surfaces if i want to obtain the drag coefficient for low velocity car (is that related?).
very well, thank you. 

June 14, 2009, 11:18 

#53 
Senior Member

Hi Elingselasri,
I suggest you use the same lengths as done in the windtunnel case you are trying to replicate. As for the grid size, that depends on the precision of the results you're looking for and the computer power available to you. In 3D a y+ of 60 and more is generally ok for a car travelling at highway speed... Also, if you are new to CFD you should start with RANS models and avoid LES for now. Good luck, Louis 

June 15, 2009, 01:36 

#54 
New Member

Thank LOuis.. but i want to simulate with farfield condition.


June 15, 2009, 10:33 

#55 
Senior Member

still.. find a wind tunnel test to replicate


June 20, 2009, 14:00 

#56 
Member
Join Date: Jun 2009
Posts: 36
Rep Power: 9 
What kind of hardware is needed to do these computation? 4gb of ram are enough? Is it possible to use a cartesian grid? Xwang


June 20, 2009, 20:44 

#57 
Senior Member

It's better than nothing.. I run 2D simulations with 2Gb ram on two processors. However for my 3D simulations I'm switching to 23 computers with each 2gb ram and I still expect my CFD runs to be long..... Serious vehicle CFD people use at least 20+ computers, but if you just want to learn you should be fine...


June 21, 2009, 02:49 

#58  
Member
Join Date: Jun 2009
Posts: 36
Rep Power: 9 
Quote:


November 3, 2009, 02:31 

#59 
New Member
Jarno
Join Date: Nov 2009
Posts: 1
Rep Power: 0 
Greetings!
First of all, sorry my bad english language but hope you get idea what i am trying! I am looking for right kind of software for linux. I have a complete 3dmodel from my racing car and i need to put it on somekind virtual wind tunnel that i can test different wings and under body air flows. What is best program for this idea? I hawe made 3dmodel of my racing car with Blender, and it can also opened with Paraview program. Should i install OpenFOAM and run some test with that? Does Paraview program has any plugs in that can help me? By the way, progam should be free... Jarno. 

November 8, 2009, 13:25 

#60 
Senior Member

Hi Jarno,
you should be able to convert your model into a mesh that will work with OpenFOAM. Do a search on the forum for "blender" and you'll likely find the information you're looking for. I have not tried it personally so I can't really help you there. good luck, Louis 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Aerodynamics  vengi  FLUENT  5  October 25, 2011 10:43 
Aerodynamics  Bonny Jacob Zachariah  Phoenics  3  February 10, 2009 05:43 
CFD in aerodynamics  Ujjwal Bhaskar  FLUENT  1  December 26, 2007 11:29 
Use of ProAm in aerodynamics  Javidan Ahmad  CDadapco  8  December 3, 2004 00:27 
unsteady aerodynamics  R.KRISHNAMURTHY  Main CFD Forum  1  December 6, 2000 02:17 