CFD Online URL
[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 11, 2010, 10:28
Default
  #61
mdz
New Member
 
Margarita DUFRESNE
Join Date: Jan 2010
Posts: 13
Rep Power: 6
mdz is on a distinguished road
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
mdz is offline   Reply With Quote

Old   May 12, 2010, 10:45
Default
  #62
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 178
Rep Power: 7
louisgag is on a distinguished road
Send a message via ICQ to 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
louisgag is offline   Reply With Quote

Old   June 18, 2010, 10:11
Default
  #63
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 299
Rep Power: 8
openfoam_user is on a distinguished road
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.
openfoam_user is offline   Reply With Quote

Old   June 18, 2010, 16:35
Default
  #64
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 178
Rep Power: 7
louisgag is on a distinguished road
Send a message via ICQ to louisgag
I will provide you a STL surface for snappyHexMesh if you agree to share your results on the forum after.

Cheers!

-Louis
louisgag is offline   Reply With Quote

Old   June 18, 2010, 17:03
Default
  #65
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 299
Rep Power: 8
openfoam_user is on a distinguished road
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.
openfoam_user is offline   Reply With Quote

Old   June 24, 2010, 05:09
Default
  #66
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 178
Rep Power: 7
louisgag is on a distinguished road
Send a message via ICQ to 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
louisgag is offline   Reply With Quote

Old   July 1, 2010, 06:09
Default
  #67
Member
 
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 6
Mo-ITB is on a distinguished road
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

Last edited by Mo-ITB; July 1, 2010 at 19:09.
Mo-ITB is offline   Reply With Quote

Old   July 1, 2010, 11:31
Default
  #68
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 178
Rep Power: 7
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Moritz,

Quote:
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
louisgag is offline   Reply With Quote

Old   July 1, 2010, 14:30
Default
  #69
Member
 
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 6
Mo-ITB is on a distinguished road
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
Mo-ITB is offline   Reply With Quote

Old   July 1, 2010, 15:02
Default
  #70
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 299
Rep Power: 8
openfoam_user is on a distinguished road
hereafter the link for the slides:

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

Stéphane.
openfoam_user is offline   Reply With Quote

Old   July 1, 2010, 15:47
Default
  #71
Member
 
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 6
Mo-ITB is on a distinguished road
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
Mo-ITB is offline   Reply With Quote

Old   July 1, 2010, 23:49
Default
  #72
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 178
Rep Power: 7
louisgag is on a distinguished road
Send a message via ICQ to 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?)
louisgag is offline   Reply With Quote

Old   July 2, 2010, 02:50
Default
  #73
Member
 
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 6
Mo-ITB is on a distinguished road
Hi Louis,

are the new wallfunctions part of OF 1.7?

best,
Moritz
Mo-ITB is offline   Reply With Quote

Old   July 2, 2010, 03:41
Default
  #74
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Yes (at least the low-Re ones): http://www.openfoam.com/docs/release-notes.php
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   July 2, 2010, 05:05
Default
  #75
Member
 
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 6
Mo-ITB is on a distinguished road
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?
Mo-ITB is offline   Reply With Quote

Old   July 2, 2010, 09:19
Default
  #76
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 178
Rep Power: 7
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Should be.

I use 1.6.x and they are available. Look for source files in
Code:
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?
louisgag is offline   Reply With Quote

Old   July 2, 2010, 12:57
Default
  #77
Member
 
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 6
Mo-ITB is on a distinguished road
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
Mo-ITB is offline   Reply With Quote

Old   July 8, 2010, 06:37
Default
  #78
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 299
Rep Power: 8
openfoam_user is on a distinguished road
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.
openfoam_user is offline   Reply With Quote

Old   July 8, 2010, 14:04
Default
  #79
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 178
Rep Power: 7
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Mortiz,

Quote:
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
Quote:
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
louisgag is offline   Reply With Quote

Old   July 26, 2010, 04:52
Default
  #80
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 299
Rep Power: 8
openfoam_user is on a distinguished road
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.
openfoam_user 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 11:43
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 22:45.