
[Sponsors] 
February 18, 2008, 16:03 
I finished to run the first si

#21 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 10 
I finished to run the first simulation with simpleFoam and the realizableKe model for turbulence. I made 1700 iterations and I hadn't covergence problems, but the flow field I visualized is very far from reality.
I don't know if the problem can be caused by the fvSchemes, I'll try to change them. Do you have any hints? Is there anybody has experience in simulation with this kind of turbulence model? 

February 19, 2008, 16:11 
How does the field look like?

#22 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 488
Rep Power: 13 
How does the field look like? What are your solver settings? Residuals?


February 20, 2008, 09:34 
Hello
Here are some work in

#23 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 87
Rep Power: 10 
Hello
Here are some work in progress pictures of my not quite yet converged practise case: http://www.students.tut.fi/~peltol20/it500.png http://www.students.tut.fi/~peltol20/it500_2.png simpleFoam standard kepsilon 3,1 million tetrahedral elements 

February 20, 2008, 09:51 
Hi Juho,
Would it be possib

#24 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 11 
Hi Juho,
Would it be possible to know the grid generator you used to create this simulation? Do you have experimental or other software numerical results to compare some parameters like drag coefficient on your model? Anyway, interesting start, and I'm waiting forward to see your converged solution. Regards, Vincent 

February 20, 2008, 10:15 
No data, it's an imaginary car

#25 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 87
Rep Power: 10 
No data, it's an imaginary car I drew. Just learning to use OpenFOAM and some qualitative results on how geometry changes affect things. Velocity is 30m/s forgot to say.
Next I should try to figure out how to use liftDrag I guess. The mesh is made in Gambit, my school has a license. Here's what checkMesh says: ================================================= Domain bounding box: (5.6 0.031 1.10134e15) (12.4 3.031 2.4) Boundary openness (3.90098e17 3.3708e16 1.22955e16) OK. Max cell openness = 1.79272e16 OK. Max aspect ratio = 8.64372 OK. Minumum face area = 2.77654e06. Maximum face area = 0.114004. Face area magnitudes OK. Min volume = 2.783e09. Max volume = 0.0111914. Total volume = 127.35. Cell volumes OK. Mesh nonorthogonality Max: 67.6634 average: 19.6029 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.878654 OK. Min/max edge length = 0.0016882 0.607378 OK. ================================================ 

February 20, 2008, 10:23 
Thanks for your reply Juho.
I

#26 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 11 
Thanks for your reply Juho.
I'm actually looking for a good and easy to use free (or not too expensive) mesher for this kind of complex meshes. But I still didn't find the perfect one. I guess I'm putting the bar a little too high!:D Problems come when beginning to use lifdrag, so don't be too hurry! Anyway, nice draw!Good luck. Vincent 

February 20, 2008, 10:37 
The ICEM CFD is good I hear, h

#27 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 87
Rep Power: 10 
The ICEM CFD is good I hear, haven't used it. It probably isn't cheap though.
Does anyone actually know the price? 

February 20, 2008, 13:18 
ICEM/CFD can cost upwards of U

#28 
New Member
Mark J.
Join Date: Mar 2009
Posts: 15
Rep Power: 10 
ICEM/CFD can cost upwards of US $15,000 for a nodelocked license. A floating license would probably cost a lot more.


February 20, 2008, 17:58 
ICEM has restrictions regardin

#29 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 488
Rep Power: 13 
ICEM has restrictions regarding hexcore meshes. Hexas all have the same size. His is not very well suited for Aerodynamic meshes.


February 20, 2008, 18:40 
What do you mean by restrictio

#30 
Member
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
What do you mean by restrictions on hexcore meshes?
I generated several multiblock structured meshes around wing and aircraft geometries using ICEMCFD, all were featuring graded edges to properly resolve the boundary layer. Gridgen from Pointwise is worth looking at (I prefer it to ICEM as far as I am concerned...), the academic licence is about 1500 GBP. On the (almost) free side, there is CUBIT. Another alternative: you can use the preprocessing utilities from EDGE (FOI CFD code with freely available binaries), and convert the generated mesh files to meet FOAM format. 

February 21, 2008, 15:28 
Patrick:
You are takling ab

#31 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 488
Rep Power: 13 
Patrick:
You are takling about ICEM Hexa. This is good for blockstructured meshes like wing flows. However, for real complex car shapes you will need lots of time to generate block structered grids. Therefore it is quite common to use more automatic methods like hexcore meshes. Hexcore meshes in ICEM Tetra can only generate hexas with a uniform edge length. His is a stupid restriction. It is better to uses hexahedrals of different sizes like TGrid or ANSA can do or even more hexdominant meshes (quality trobles!) Regards 

February 22, 2008, 12:47 
BastiL,
my residuals are very

#32 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 10 
BastiL,
my residuals are very low (10^8), but the wake has an absurd shape. The solver settings I used are: ddtSchemes { default steadyState; } gradSchemes { default fourth; grad(p) fourth; grad(U) fourth; } divSchemes { default none; div(phi,U) Gauss SFCD; div(phi,k) Gauss SFCD; div(phi,epsilon) Gauss SFCD; div(phi,R) Gauss SFCD; div(R) Gauss linear; div(phi,nuTilda) Gauss SFCD; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } // ************************************************** *********************** // solvers { p GAMG { tolerance 1e08; relTol 0; smoother GaussSeidel; nCellsInCoarsestLevel 40; mergeLevels 1; agglomerator faceAreaPair; cacheAgglomeration off; nPreSweeps 0; nPostSweeps 2; nFinestSweeps 2; scaleCorrection true; directSolveCoarsest false; }; U BICCG 1e07 0; k BICCG 1e06 0; epsilon BICCG 1e06 0; R BICCG 1e06 0; nuTilda BICCG 1e06 0; } SIMPLE { nNonOrthogonalCorrectors 1; pRefCell 0; pRefValue 0; } relaxationFactors { p 0.3; U 0.4; k 0.5; epsilon 0.5; R 0.7; nuTilda 0.5; }  Hrv suggested these settings in another topic of this forum. What's your opinion? 

February 22, 2008, 13:45 
? Did I really  this looks pr

#33 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,793
Rep Power: 23 
? Did I really  this looks pretty bizarre to me.
gradSchemes { default fourth; grad(p) fourth; grad(U) fourth; } Nope. Use Gauss linear or leastSquares if your mesh is bad. div(phi,k) Gauss SFCD; div(phi,epsilon) Gauss SFCD; div(phi,R) Gauss SFCD; Here, Gauss upwind is probably good enough. For momentum convection, try div(phi,U) Gauss GammaV 0.5; and see if it converges. If not, we can talk more... Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

February 22, 2008, 17:02 
I'm sorry, Vincent RIVOLA used

#34 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 10 
I'm sorry, Vincent RIVOLA used these settings.
On manday I'll test with the schemes you suggest. According your opinion, are the solvers OK? Is it possible make iterations faster? Another thing: in each time step, that should be an iteration counter for steady solvers, there are several iterations inside. Why? 

February 23, 2008, 05:08 
Mattia,
how bad is your mes

#35 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 488
Rep Power: 13 
Mattia,
how bad is your mesh? Btw, how did you create it? Could you post the output from checkMesh, please. It might be worth trying to reduce nNonOrthogonalCorrectors to 0 if your mesh is not too bad. This will give you an aditional speedup. Youre right, a timesteps corresponds to what other solvers call iteration. The output of iterations give you the inner iterations for each variable (called sweeps in STAR). Hrv please correct me if I am wrong. Regards 

February 23, 2008, 09:03 
BastiL,
I use a tetrahedral m

#36 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 10 
BastiL,
I use a tetrahedral mesh of 1.3mil cells and I think it's quite good. Max cell skewness is less than 0.40 . However on monday I'll post the checkMesh result. 

February 23, 2008, 10:26 
Mattia,
quality sounds good

#37 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 488
Rep Power: 13 
Mattia,
quality sounds good. I am looking forward to see the checkMesh results. What tool did you use? Is it komplex geometry? Cell count is low so I guess it is a more simple shape? In general perver hexahedral over tetras so aim for more hexdominant meshes. Regards 

February 23, 2008, 10:48 
I'm baffled by the pressure re

#38 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 87
Rep Power: 10 
I'm baffled by the pressure results in my case.
My free stream velocity is 30m/s After 3000 iterations, and max. pressure hasn't changed much during the last 1500 of them, simpleFoam gives a stagnation pressure of 672 at the front of the car. Shouldn't it be 30²/2 = 450? What am I missing? 

February 25, 2008, 13:43 
Hallo,
this is the output of

#39 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 10 
Hallo,
this is the output of checkMesh: Mesh stats points: 262914 edges: 1633690 faces: 2644429 internal faces: 2450187 cells: 1273654 boundary patches: 7 point zones: 0 face zones: 0 cell zones: 0 Number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 1273654 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Topological cell zipup check OK. Face vertices OK. Faceface connectivity OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface Ahmed_body 55893 28228 ok (not multiply connected) simmetry 59808 30528 ok (not multiply connected) side 5778 3066 ok (not multiply connected) outlet 546 305 ok (not multiply connected) inlet 539 301 ok (not multiply connected) road 66226 33517 ok (not multiply connected) top 5452 2902 ok (not multiply connected) Checking geometry... Domain bounding box: (11 9.1e06 0.05) (5 1.5 1.5) Boundary openness (1.88276e17 1.94498e15 2.05761e15) OK. Max cell openness = 1.70742e16 OK. Max aspect ratio = 7.26466 OK. Minumum face area = 1.3057e06. Maximum face area = 0.012724. Face area magnitudes OK. Min volume = 6.59628e10. Max volume = 0.000420286. Total volume = 37.1445. Cell volumes OK. Mesh nonorthogonality Max: 67.8068 average: 19.6179 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.97498 OK. Min/max edge length = 0.00165297 0.196461 OK. All angles in faces OK. All face flatness OK. Mesh OK. 

February 25, 2008, 14:23 
Looks like a pretty good mesh.

#40 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 488
Rep Power: 13 
Looks like a pretty good mesh. Try zero nonorthogonal correctors. This will speed up your solution. What software did you use for meshing?
Regards 

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 