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

Car aerodynamics

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 18, 2008, 16:03
Default I finished to run the first si
  #21
New Member
 
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 8
morfeus80 is on a distinguished road
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?
morfeus80 is offline   Reply With Quote

Old   February 19, 2008, 16:11
Default How does the field look like?
  #22
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 470
Rep Power: 11
bastil is on a distinguished road
How does the field look like? What are your solver settings? Residuals?
bastil is offline   Reply With Quote

Old   February 20, 2008, 09:34
Default Hello Here are some work in
  #23
Member
 
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 80
Rep Power: 8
juho is on a distinguished road
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 k-epsilon
3,1 million tetrahedral elements
juho is offline   Reply With Quote

Old   February 20, 2008, 09:51
Default Hi Juho, Would it be possib
  #24
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 275
Rep Power: 9
vinz is on a distinguished road
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
vinz is offline   Reply With Quote

Old   February 20, 2008, 10:15
Default No data, it's an imaginary car
  #25
Member
 
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 80
Rep Power: 8
juho is on a distinguished road
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 -1.10134e-15) (12.4 3.031 2.4)
Boundary openness (-3.90098e-17 3.3708e-16 -1.22955e-16) OK.
Max cell openness = 1.79272e-16 OK.
Max aspect ratio = 8.64372 OK.
Minumum face area = 2.77654e-06. Maximum face area = 0.114004. Face area magnitudes OK.
Min volume = 2.783e-09. Max volume = 0.0111914. Total volume = 127.35. Cell volumes OK.
Mesh non-orthogonality Max: 67.6634 average: 19.6029
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.878654 OK.
Min/max edge length = 0.0016882 0.607378 OK.

================================================
juho is offline   Reply With Quote

Old   February 20, 2008, 10:23
Default Thanks for your reply Juho. I
  #26
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 275
Rep Power: 9
vinz is on a distinguished road
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
vinz is offline   Reply With Quote

Old   February 20, 2008, 10:37
Default The ICEM CFD is good I hear, h
  #27
Member
 
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 80
Rep Power: 8
juho is on a distinguished road
The ICEM CFD is good I hear, haven't used it. It probably isn't cheap though.

Does anyone actually know the price?
juho is offline   Reply With Quote

Old   February 20, 2008, 13:18
Default ICEM/CFD can cost upwards of U
  #28
New Member
 
Mark J.
Join Date: Mar 2009
Posts: 15
Rep Power: 8
vtk_fan is on a distinguished road
ICEM/CFD can cost upwards of US $15,000 for a node-locked license. A floating license would probably cost a lot more.
vtk_fan is offline   Reply With Quote

Old   February 20, 2008, 17:58
Default ICEM has restrictions regardin
  #29
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 470
Rep Power: 11
bastil is on a distinguished road
ICEM has restrictions regarding hexcore meshes. Hexas all have the same size. His is not very well suited for Aerodynamic meshes.
bastil is offline   Reply With Quote

Old   February 20, 2008, 18:40
Default What do you mean by restrictio
  #30
pbo
Member
 
Patrick Bourdin
Join Date: Mar 2009
Posts: 40
Rep Power: 8
pbo is on a distinguished road
What do you mean by restrictions on hexcore meshes?
I generated several multi-block structured meshes around wing and aircraft geometries using ICEM-CFD, 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.
pbo is offline   Reply With Quote

Old   February 21, 2008, 15:28
Default Patrick: You are takling ab
  #31
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 470
Rep Power: 11
bastil is on a distinguished road
Patrick:

You are takling about ICEM Hexa. This is good for block-structured 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 T-Grid or ANSA can do or even more hex-dominant meshes (quality trobles!)

Regards
bastil is offline   Reply With Quote

Old   February 22, 2008, 12:47
Default BastiL, my residuals are very
  #32
New Member
 
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 8
morfeus80 is on a distinguished road
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((1|A(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 1e-08;
relTol 0;
smoother GaussSeidel;
nCellsInCoarsestLevel 40;
mergeLevels 1;
agglomerator faceAreaPair;
cacheAgglomeration off;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;
scaleCorrection true;
directSolveCoarsest false;
};
U BICCG 1e-07 0;
k BICCG 1e-06 0;
epsilon BICCG 1e-06 0;
R BICCG 1e-06 0;
nuTilda BICCG 1e-06 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?
morfeus80 is offline   Reply With Quote

Old   February 22, 2008, 13:45
Default ? Did I really - this looks pr
  #33
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,756
Rep Power: 21
hjasak will become famous soon enough
? 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
hjasak is offline   Reply With Quote

Old   February 22, 2008, 17:02
Default I'm sorry, Vincent RIVOLA used
  #34
New Member
 
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 8
morfeus80 is on a distinguished road
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?
morfeus80 is offline   Reply With Quote

Old   February 23, 2008, 05:08
Default Mattia, how bad is your mes
  #35
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 470
Rep Power: 11
bastil is on a distinguished road
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
bastil is offline   Reply With Quote

Old   February 23, 2008, 09:03
Default BastiL, I use a tetrahedral m
  #36
New Member
 
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 8
morfeus80 is on a distinguished road
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.
morfeus80 is offline   Reply With Quote

Old   February 23, 2008, 10:26
Default Mattia, quality sounds good
  #37
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 470
Rep Power: 11
bastil is on a distinguished road
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 hex-dominant meshes.

Regards
bastil is offline   Reply With Quote

Old   February 23, 2008, 10:48
Default I'm baffled by the pressure re
  #38
Member
 
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 80
Rep Power: 8
juho is on a distinguished road
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 30/2 = 450?

What am I missing?
juho is offline   Reply With Quote

Old   February 25, 2008, 13:43
Default Hallo, this is the output of
  #39
New Member
 
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 8
morfeus80 is on a distinguished road
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 zip-up check OK.
Face vertices OK.
Face-face 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 -9.1e-06 -0.05) (5 1.5 1.5)
Boundary openness (-1.88276e-17 1.94498e-15 2.05761e-15) OK.
Max cell openness = 1.70742e-16 OK.
Max aspect ratio = 7.26466 OK.
Minumum face area = 1.3057e-06. Maximum face area = 0.012724. Face area magnitudes OK.
Min volume = 6.59628e-10. Max volume = 0.000420286. Total volume = 37.1445. Cell volumes OK.
Mesh non-orthogonality Max: 67.8068 average: 19.6179
Non-orthogonality 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.
morfeus80 is offline   Reply With Quote

Old   February 25, 2008, 14:23
Default Looks like a pretty good mesh.
  #40
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 470
Rep Power: 11
bastil is on a distinguished road
Looks like a pretty good mesh. Try zero non-orthogonal correctors. This will speed up your solution. What software did you use for meshing?

Regards
bastil 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
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 Pro-Am in aerodynamics Javidan Ahmad CD-adapco 8 December 3, 2004 00:27
unsteady aerodynamics R.KRISHNAMURTHY Main CFD Forum 1 December 6, 2000 02:17


All times are GMT -4. The time now is 11:58.