[mdz]

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

[louisgag]

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

[openfoam_user]

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.

[louisgag]

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

Cheers!

-Louis

[openfoam_user]

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.

[louisgag]

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

[Mo-ITB]

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

[louisgag]

Moritz,

bc i use zeroGradient at the inlet for k and epsilon and slip on top

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

[Mo-ITB]

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

[openfoam_user]

hereafter the link for the slides:

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

Stéphane.

[Mo-ITB]

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?

U.jpg

k.jpg

epsilon.jpg

symmetry_k.jpg

symmetry_U.jpg

[louisgag]

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?)

[Mo-ITB]

Hi Louis,

are the new wallfunctions part of OF 1.7?

best,
Moritz

[alberto]

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

[Mo-ITB]

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?

[louisgag]

Should be.

I use 1.6.x and they are available. Look for source files in

src/turbulence/incomp/derivedFvPa/RAS/wallFunctions

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?

[Mo-ITB]

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

[openfoam_user]

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.

[louisgag]

Mortiz,

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...

the nutSpalartAllmarasWallFunction works with all RAS models. Just like the most (or all) of the other ones listed in

src/turbulenceModels/incompressible/RAS/derivedFvPatchFields/wallFunctions/

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

[openfoam_user]

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.