It's a grid I made some time a
 

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.

Would any of you have access t
 

Would any of you have access to 3d-models of real cars you could spare? Something I could find Cd and Cl figures on?

I'd like to compare results to experimental data.

Hallo, I made 2000 iteration
 

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?

Hi, In my not quite converg
 

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 1-20mm 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%.

Added turbulent drag to the so
 

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

Dear users, we are going to
 

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, 10-11 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 e-mail to me or to the other session organizers of the Automotive session. The deadline is on the 31st March.

Best Regards,

Tommaso

Hi everybody, Still working
 

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

Dear all, Like many on the
 

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 k-Omega-SST 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.

http://www.cfd-online.com/OpenFOAM_D...es/1/11271.png

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((1|A(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 1e-06;
relTol 0.1;

smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;

cacheAgglomeration true;

nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};
U smoothSolver
{
smoother GaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0.1;
};
k smoothSolver
{
smoother GaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0.1;
};
omega smoothSolver
{
smoother GaussSeidel;
nSweeps 1;
tolerance 1e-8;
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 (non-closed singly connected)
body_front 9357 4807 ok (non-closed singly connected)
body_bottom 18400 9499 ok (non-closed singly connected)
body_slant 4413 2310 ok (non-closed singly connected)
body_base 5116 2685 ok (non-closed singly connected)
body_struts 1500 799 ok (non-closed singly connected)
body_side 26563 13581 ok (non-closed singly connected)
tunnel_road 101873 51568 ok (non-closed singly connected)
tunnel_inlet 1713 1042 ok (non-closed singly connected)
tunnel_infinity 10052 5508 ok (non-closed singly connected)
tunnel_outlet 3088 1730 ok (non-closed singly connected)
tunnel_symmetryplane120117 66275 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-4.176 -5.46623e-12 0) (7.308 3.3265 3.3265)
Mesh (non-empty) directions (1 1 1)
Mesh (non-empty, non-wedge) dimensions 3
Boundary openness (-1.43894e-17 5.86639e-15 1.04078e-15) OK.
Max cell openness = 5.96728e-16 OK.
Max aspect ratio = 12.1381 OK.
Minumum face area = 7.52672e-08. Maximum face area = 0.0367279. Face area magnitudes OK.
Min volume = 1.12097e-11. Max volume = 0.00212606. Total volume = 99.7353. Cell volumes OK.
Mesh non-orthogonality Max: 67.1824 average: 16.1836
Non-orthogonality 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

Dear Tom, in my experience
 

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

Dear Luca, Thank you for yo
 

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 non-orthogonal correctors. Thanks again.

Regards,
Tom

Tom,

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

Regards,

-Louis

CFD for car
 

Hi, I am newbie in CFD,:D. 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.

Hi Elingselasri,
I suggest you use the same lengths as done in the wind-tunnel 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

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

still.. find a wind tunnel test to replicate

What kind of hardware is needed to do these computation? 4gb of ram are enough? Is it possible to use a cartesian grid? Xwang

It's better than nothing.. I run 2D simulations with 2Gb ram on two processors. However for my 3D simulations I'm switching to 2-3 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...

I want to learn the program. Then I will buy a more powerful pc. Xwang

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 3d-model 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 3d-model 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.

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

Hi Morfeus80,

I have 7 years experience in R&D in automotive industry.

The turbulence wake modeling is bit difficult,

you can use k-eps model with mesh iterative improving (less complicated), or RSM model (very high grid squeness needing).

KR,

MDZ

Hi Margarita,

would you recommend using a low Reynolds model with y+ values around 1 on the wall of the vehicle and a coarser mesh on the floor but with a slip condition on pressure and velocity?

I'm questioning whether to use a high or low Re model and so far the high Reynolds with wall functions has done well but maybe LowRe would do even better (especially in detached zones)?

Thanks for your insight!


-Louis

Hi,

can someone provide me the geometry file (iges format preferably) of the Ahmed body with 12.5 degree slant angle ?

My email address is :
stephane.sanchi@cfse.ch

Best regards,

Stephane.

I will provide you a STL surface for snappyHexMesh if you agree to share your results on the forum after.

Cheers!

-Louis

Hi Louis,

Yes, I just want to reproduce the results you have obtained and will present during the 5th OpenFOAM workshop in Chalmers !

I will use both snappyHexMesh and ICEMCFD Hexa for mesh generation for comparison.

Regards,

Stephane.

Very nice. I am sending you the mesh shortly. Also, you might find better graphics in my presentation, which should be available on the OFW5 website.

Regards,

-Louis

hi Louis,

have you made any progress with low-re modelling of the ahmed body? i'm on it for quite a while now with lam-bremhorst, but still have not reached convergence.

i tried to make a laminar start and then switch on turbulence, but still epsilon diverges after a while in the subsurface layer.
for the bc i use zeroGradient at the inlet for k and epsilon and slip on top, bottom, left and right for everything.

i also used a lot of combinations of k and epsilon as initial conditions.

so there is only a sublayer at the body, i tried different amounts of layers, up to 40. the cell closest to the wall is 0.05 mm diameter, the mesh is a polymesh made by ccm+ and the fvSchemes for convection are all set to upwind.

as you seem to work on low-reynolds as well, it would be great to exchange our experiences.

my plan now is to make just a cylinder flow and get this to converge with low-re to get the most stable schemes and relaxation factors.

all the best,
moritz

Moritz,

I think this can sometimes be a cause of non-convergence. What version of OF are you using? I use 1.6(.x) with "automatically" implemented wall functions. I can get convergence with all the wall models but have not yet generated a real LowRe mesh. ! My y+ ranges from about 10 to 100. I am not using layers neither. My mesh is fairly basic. I use inlet k and omega (from k-omega-SST model) as defined by regular equations based on turbulent intensity and inlet boundary layer approximation. I do not use a slip upwind condition on the floor but it can be useful to control the boundary layer thickness. You can see the graphical results of my validation on the Ahmed body at 12.5 deg on the OFW5 website, on my slides, and apart from the weakness of vortex "c" the flow is quite well reproduced!


Stephane,

can you post your questions here, it will be easier for me to reply and allow others such as Moritz to follow our discussion!


Best regards,

-Louis

Hi Louis,

i use OF 1.6. At the beginning i had bc for k and eps at the inlet, but this always led to divergence in the boundary layer i used for the bottom.

with zeroGradient and the initial conditions calculated by the equations given on cfd-online, i only have problems of divergence on the body itself.

what characteristic length and turbulent intensity do you use?
i tried different values for both and the best till now were:

- 1mm for characteristic length, 0.5 mm turbulent lenght
- turb. intensity 5 %

that gives the initial conditions:

- k=6
- epsilon= 26454
- nut= 0.0012

this was running quite well for 140 iterations, i also got the cd of 0.38 perfectly ( i have 30 deg ahmed body), but then epsilon rises till divergence, mostly on sharp edges or arround the feet.

i used the slip condition on the floor to prevent epsilon from diverging here, which is working ;).

when i used bc for k and epsilon, i saw in plots that nothing of that reached the body itself, it was only important for the boundary layer at the inlet. as i use slip, i have no boundary layer at the inlet, so i guess no need for a bc.

could you post the url where to find your slides? i just found this one:

http://www.openfoamworkshop.org/2010...itle=Main_Page

but didnt find your slides.

all the best,
moritz

hereafter the link for the slides:

http://web.student.chalmers.se/group...SlidesOFW5.pdf

Stéphane.

hi stephane and louis,

thanks for the link, but for me its not working :(.

Attached are some pics of my case where you can see the problem zones of epsilon behind a foot of the ahmed body. it seems its the stall zone...
any ideas what to do to prevent this? i thought about thinner layers, but i already got 0.05 mm...

having a look at the nut plot makes me wonder if the values are reasonable. may it be they are much too low and so the turb. layer at the surface cannot be build up properly?

Attachment 3965

Attachment 3967

Attachment 3968

Attachment 3970

Attachment 3971

Moritz,

I used 0.5% turb int. and 3cm boundary layer to calculate char length. 5% turb int seems pretty high.

Maybe you should try the new wall functions. There is nutSpalartAllmarasWallFunction, LowReWallFunction, etc.. that way you know what is being done at the wall instead of using zeroGradient..

Best,

-Louis

PS: maybe it's just a matter of make your boundary cells shorter (like cutting them in two on the long axis?)

Hi Louis,

are the new wallfunctions part of OF 1.7?

best,
Moritz

Yes (at least the low-Re ones): http://www.openfoam.com/docs/release-notes.php

how is the low-re-wallfunction working? is it like in lam-bremhorst a function which is added to the eps, k and nut equations or like standard-k-e a function which replaces the eps, k and nut equations?

Should be.

I use 1.6.x and they are available. Look for source files in
or something like that, can't remember right now. The header file of each function contains a small explanation.

Also, be aware that the spalding function (nutSpalartAllmarasWallFunction) will not work if you have a zero velocity on the wall, the trick is to set the velocity to something like (0 0 1e-10). To use these new functions, set them in the nut file of the 0 directory and use kRqWallFunction on corresponding k and omegaWallFunction on omega. Values = 0 might be required but not used and values of constants (C_mu, etc) are not necessary in these files....

Sorry I don't have the files in front of me so I'm telling you this by memory.

Best,

-Louis

PS: what meshing software are you using on the Ahmed body?

here is what i did till now:

when chosing lam-bremhorst i use no wall functions, because in low-reynolds-models there are correction-functions (f1 and f2) implemented in the equations for k, epsilon and turb.visc. for cells close to patches (they depend on the distance from the patch) which simulate the increased turbulent viscosity there and this should build up the laminar layer.

so i have no wall boundary conditions, only patches where the low-reynolds model should apply.

on the patches eps is zero-grad. and k should be 0, where you have to use the trick you mentioned like k=1e-10 because somewhere its divided by k.

what is a low-reynolds-wall-bc changing here?

at the moment im trying to play arround with C_mu which helps to get a thicker boundary-layer at the patches and prevents k and eps to explode there caused by the very high velocity-gradients.

this should be only to get close to a solution and then to be turned back to the standard value..

louis, you mention the nutSpalartAllmarasWallFunction, i think this is for the one-equation-model SpalartAllmaras only or not?
as i understood low-re-models are extended k-eps-two-equation models...

im very interested in the progress in this discussion :).

all the best,
moritz

Louis,

What are the dimensions of the external domain that you have used for comparison with wind tunnel data ?

Graz University has used the following dimensions 15 x 1.87 x 1.4 m3.

https://online.tu-graz.ac.at/tug_onl...cumentNr=81599

And where is located the ahmed body in the X-direction ?

Regards,

Stephane.

Mortiz,

the nutSpalartAllmarasWallFunction works with all RAS models. Just like the most (or all) of the other ones listed in
I use walls (not patch) and the k-Omega-SST model does have f1 and f2 functions but they apply outside of the lowRe region...


Stéphane,

Overall domain bounding box (-6.364 -0.338 -0.8405) (10.636 1.062 1.0295)
and I am pretty sure I have the vehicle frontmost part at x=-0.1 (the start of the cubic box is at x=0 and y=-0.288 .
1.87 width x 1.4 height are pretty much ERCOFTAC recommended dimensions and that is also whats I used for a basis.

http://www.ercoftac.org/fileadmin/us...9.4/index.html

Have you started getting interesting results for the 12.5 degree body?



Best,

-Louis

Hi,

Could someone provide me experimental data (drag, lift, drag coefficient and lift coefficient) for the ahmed body with 12.5 deg slant angle ?

Inlet velocity is 40 m/s.

Regards,

Stephane.