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

Automotive test case

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 29, 2007, 11:37
Default Hello everybody, I am runni
  #81
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Hello everybody,

I am running some validation cases for a naca0012 at low angle of attack using simpleFoam and k-epsilon turbulence model. Airfoil chord 1 m, inlet velocity 50 m/s, free-stream viscosity 1.7894e-5.

I noticed that if I compile the liftDrag.C version from Vincent RIVOLA on Wednesday, September 19, 2007 - 09:36 am the results are quite good (if I multiply by density).

However, I tried using liftDrag.C posted by Vincent RIVOLA on Thursday, September 20, 2007 - 03:47 am and I get a drag coefficient which is 4 orders of magnitude lower.

I am checking these two files. I will keep you updated.

Thank you,

Alessandro
gtg627e is offline   Reply With Quote

Old   October 29, 2007, 11:43
Default Sorry, I see you have to pass
  #82
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Sorry, I see you have to pass in Aref.

Howver comparing "Vincent RIVOLA on Wednesday, September 19, 2007 - 09:36 am" with "Vincent RIVOLA on Thursday, September 20, 2007 - 03:47 am " it seems like the values of turbulent and laminar drag coefficients get swapped.

Alessandro
gtg627e is offline   Reply With Quote

Old   October 29, 2007, 13:25
Default Hello everybody, using li
  #83
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Hello everybody,


using liftDrag.C from "Vincent RIVOLA on Wednesday, September 19, 2007 - 09:36 am" and my airfoil at 0-deg angle of attack I get:

total Turbulent drag coefficient: 0.00034
total laminar drag coefficient: 0.00116

which I cannot explain. Even if I multiply my density, say 1.225, the total drag is way too low, as it should be ~~ 0.0058 from "theory of wing sections".

I changed liftDrac.C as suggsted by " Rosario Russo on Monday, September 24, 2007 - 09:32 am" and now I get:

total Turbulent drag coefficient: 0.00198
total laminar drag coefficient: 0.001161


Still way off.
I will re-run my case with better schemes.

Any comments?

Thank you,

Alessandro
gtg627e is offline   Reply With Quote

Old   October 29, 2007, 14:43
Default Ok, I give up. Using the sa
  #84
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Ok, I give up.

Using the same mesh in fluent I get a drag coefficient of 0.0052 which is 10% away from the experimental value in "theory of wing sections."

OpenFoam gives me 0.00314.

Please help

Alessandro
gtg627e is offline   Reply With Quote

Old   October 29, 2007, 16:19
Default Hi Alessandro, I'm also int
  #85
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 277
Rep Power: 9
vinz is on a distinguished road
Hi Alessandro,

I'm also interested in your computations since, I am still not sure that the liftDrag utility is computing the drag correctly.
To really compare the values from OpenFOAM and Fluent, I think it would be interesting to compare the Cp values found in fluent to the ones found in OpenFOAM. If these values are the same, the problem is coming from the liftdrag utility.
Otherwise, the problem is coming from the computation. The same can be done by comparing velocity fields.

Hope that helps.
Regards,

Vincent
vinz is offline   Reply With Quote

Old   October 30, 2007, 23:45
Default liftDrag area calculation for
  #86
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
liftDrag area calculation for force computation is non-trivial. Please make sure that if you are working on a 2D case, the domain length in the third direction is reasonable. See Hrv's comment here to follow what I'm referring to --> http://www.cfd-online.com/OpenFOAM_D...es/1/2726.html
msrinath80 is offline   Reply With Quote

Old   April 24, 2008, 09:23
Default Hi everybody, I now manage
  #87
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 277
Rep Power: 9
vinz is on a distinguished road
Hi everybody,

I now manage to get some interesting results on Ahmed test case and on a real race car.
Pressure and velocity fields look not so bad and some vortices can be observed in some particular regions.
However I still have some doubts on my way to compute lift and drag coeffcients. Drag coefficient looks ok actually, for the ahmed body and for the race car as well.
But the lift coefficient is far from the results I should have.
By reading again this topic I see that some questions stayed without answer. Especially the doubts about the way to compute turbulent part.

Could someone point out what is actually the best liftDrag tool which could be used with simpleFoam?

Regards,

Vincent
vinz is offline   Reply With Quote

Old   April 24, 2008, 10:11
Default Hi Vincent, I ran a Ahmed bod
  #88
New Member
 
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 8
morfeus80 is on a distinguished road
Hi Vincent,
I ran a Ahmed body case with 4M cells for half car in SimpleFoam, but the results I managed weren't so good: the pressure and velocity fields were quite different from experimental data.
Can you describe what models and solvers you used, please?
morfeus80 is offline   Reply With Quote

Old   June 2, 2008, 17:18
Default Hey Mattia, which slant ang
  #89
New Member
 
Thomas Ceyrowsky
Join Date: Mar 2009
Location: Germany
Posts: 9
Rep Power: 8
ceyrows is on a distinguished road
Hey Mattia,

which slant angle did you run? Turbulence modelling is not capable for getting the correct results with 25°. Additionally the flow around the 25°-case is very instationary so simpleFoam has got some converging problems (at least in my calculations).
Apart from that the 35°-results with simpleFoam were pretty good, because the flow has got a stable character. I had positive experiences with the Realizable-k-epsilon model and the limitedLinear TVD-Interpolation.

Best regards,

Thomas
ceyrows is offline   Reply With Quote

Old   October 7, 2008, 15:16
Default Hi all, I have been doing s
  #90
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 208
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Hi all,

I have been doing some Ahmed body drag and lift calculations and although I often get ok results for the drag coefficients, the lift coefficients I get are always in the range of 3-4.. Which is about 10 times too large.

I am working in 2D with simpleFoam and RealizableKE, komegaSST, and SA models.

Has anyone experienced difficulties with computing the lift? I would appreciate some pointers!

Thank you,

-Louis
louisgag is offline   Reply With Quote

Old   October 8, 2008, 05:17
Default From reading some articles, it
  #91
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
From reading some articles, it seems a few people have. How are you calculating the lift coefficient?
madad2005 is offline   Reply With Quote

Old   October 8, 2008, 11:56
Default Hi Adriano, I use the force
  #92
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 208
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Hi Adriano,

I use the forceCoefficients function included in OF 1.5. Also, I verify the results obtained from that with the patchIntegrate on pressure and I get values that correspond (viscous lift excluded) to what forceCoefficients gives.

Aref= frontal projected area

I assume there is something wrong in my pressure field but I find strange that drag forces are still reasonable.

Have a good day,

-Louis
louisgag is offline   Reply With Quote

Old   October 8, 2008, 12:43
Default What is your frontal area valu
  #93
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
What is your frontal area value? What are your minimum values of surface pressure on the upper surface? Have you tried looking at the velocity fields and comparing it to the experimental data?
madad2005 is offline   Reply With Quote

Old   October 8, 2008, 13:49
Default Aref=0.00288 (my mesh is 0.01
  #94
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 208
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Aref=0.00288 (my mesh is 0.01 m thick); min pressure on upper surface is [-1.5,-2.08] (the lowest pressure is proportional to the drag coefficient I get); and my velocity fields look somewhat like the experimental data: two recirculation zones at the vertical back plane (and on the slant plane when slant angle is large enough), very thin B.L. on top surface, acceleration zone on the top leading edge.
The acceleration zone on the leading edge goes all the way to the wall of the vehicle and the velocity is >1 until it reaches the wall where it suddenly becomes 0.

(Longitudinal vortices are excluded since Im in 2D).

Also, another strange trend I noticed is that when drag is overestimated, the value of lift reduces (usually not enough to get appropriate results and the trend is not always respected).

thanks for your help! (I am doing this project for my Master's thesis)

-Louis
louisgag is offline   Reply With Quote

Old   October 9, 2008, 03:29
Default Is that your minimum pressre c
  #95
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
Is that your minimum pressre coefficient? The velocity at the wall should be zero due to the no-slip condition.

Do all your results converge ok? If so, how long do you run them for? Finally, what is the first wall spacing you are using (or y+ would be better)?

-Adriano
madad2005 is offline   Reply With Quote

Old   October 9, 2008, 09:48
Default the is actually the pressure
  #96
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 208
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
the [-1.5,-2.08] is actually the pressure "p" value (using a 0 reference pressure), so I assume it is in (Pa *m^3/kg). ( I wrote lowest upper surface pressure proportional to drag coefficient but I meant lowest upper surface pressure proportional to lift coefficient...)

I use the no-slip condition (fixedValue velocity, value = uniform 0 on the vehicle wall) and still get velocity >1 on the cell/point next to the wall; also, pressure is zeroGradient on the vehicle wall.

My results converge very well, except in a few rare cases.

As for my y+ value, it is not consistent through the whole wall and I have a hard time getting it outsite of the "intertide" zone of 1<yplus<30. (Allthough Im not sure this is an issue with models other than SA)

Here are a few Yplus values I get:

min: 6.9669 max: 90.5637 average: 59.6992 (SA)
min: 0.418455 max: 18.4831 average: 8.81904 (SA)
min: 12.8556 max: 334.043 average: 155.761 (RKE)
min: 12.0163 max: 301.83 average: 144.64 (RKE)

Also, convergence is not a good (or maybe just very slow) when I try to lower my value of Yplus by refinement at the wall.

min: 0.128637 max: 18.1411 average: 6.55086 (komegaSST, with pretty fine mesh)


Have a good day!

-Louis
louisgag is offline   Reply With Quote

Old   October 9, 2008, 10:00
Default Forgot to add... It is my m
  #97
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 208
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Forgot to add...

It is my minimum pressure, yes.

And i run the calculation until drag is constant (at least to the 10^-4), when possible; at that point there are no more iterations per "timestep" on velocities and sometimes 1 on pressure. (Thats usually 20000-30000 iterations.

But again, with the smaller y+ it is not as obvious to run the simulations until convergence!

Also, concerning the velocity field, the velocity near the bottom leading edge of the vehicle lower than on the upper leading edge.

-Louis
louisgag is offline   Reply With Quote

Old   October 24, 2008, 19:58
Default Hi Adriano, Do you have any
  #98
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 208
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Hi Adriano,

Do you have any hints to help me get better lift coefficients?

I am currently trying to see if changing the bottom surface to a fixed one, as in the experiments, will help. So far my results still have a very high lift coefficient.

regards,

-Louis
louisgag is offline   Reply With Quote

Old   October 27, 2008, 09:43
Default Hi Louis, What boundary con
  #99
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
Hi Louis,

What boundary condition did you apply to the lower surface wall previously?

If possible, would you be able to e-mail me your mesh and I can run it myself and take a look at it?

In the meantime, I'd try, if possible, to get a mesh with a y+ of between 30 (abs. min) and 300 and re-run with the k-e model, and have a look at the results. It will give you a better idea before you attempt a more challenging y+=1 mesh.
madad2005 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
3d test case Hassan Raiesi Main CFD Forum 1 August 19, 2006 12:33
Test Case ganesh Main CFD Forum 0 March 16, 2006 13:34
Looking for test case William M. Main CFD Forum 2 May 26, 2005 03:45
test case? lsm Main CFD Forum 0 June 14, 2004 11:39
test case Follet Main CFD Forum 0 July 8, 2002 04:07


All times are GMT -4. The time now is 09:26.