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   September 11, 2007, 23:55
Default Vincent, BastiL, I just sen
  #41
New Member
 
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8
vega is on a distinguished road
Vincent, BastiL,

I just sent you the whole model via yousendit.com.
Just go to the link that you will get on email accounts in the profile and download the file.

thanks

--
Rajneesh
vega is offline   Reply With Quote

Old   September 12, 2007, 03:09
Default Thanks a lot Rajneesh, I recei
  #42
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9
vinz is on a distinguished road
Thanks a lot Rajneesh, I received it.

I just had a look at your mesh and it's totaly different from mine, so it will be very interesting.

I'm going to run it to see what I get, and I'll post my results.

Regards,

Vincent
vinz is offline   Reply With Quote

Old   September 12, 2007, 03:35
Default I can not try 1.4 at the momen
  #43
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11
bastil is on a distinguished road
I can not try 1.4 at the moment, I am using simpleFoam 1.4.1 and I get:

Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0254472, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.00714854, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0269422, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00938556, No Iterations 13
time step continuity errors : sum local = 38.8664, global = -1.26956, cumulative = -1.26956
DILUPBiCG: Solving for epsilon, Initial residual = 0.999636, Final residual = 0.0488436, No Iterations 1
bounding epsilon, min: -316.208 max: 3.94271e+06 average: 149.224
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 7.80029e-05, No Iterations 1
ExecutionTime = 215.08 s ClockTime = 215 s

...

Time = 4

DILUPBiCG: Solving for Ux, Initial residual = 0.123077, Final residual = 0.00151918, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.291113, Final residual = 0.00156297, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.539444, Final residual = 0.000117586, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.646448, Final residual = 0.00622016, No Iterations 59
time step continuity errors : sum local = 17.5265, global = 0.715884, cumulative = 0.36078
DILUPBiCG: Solving for epsilon, Initial residual = 0.0334807, Final residual = 4.11484e-05, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.233191, Final residual = 0.000210396, No Iterations 1
ExecutionTime = 870.11 s ClockTime = 870 s

....

Time = 9

DILUPBiCG: Solving for Ux, Initial residual = 0.147892, Final residual = 1.23908e-07, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.414654, Final residual = 1.23514e-06, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.51769, Final residual = 1.05291e-06, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.597334, Final residual = 0.00588535, No Iterations 23
time step continuity errors : sum local = 7.93123e+08, global = 3.50323, cumulative = 12.0621
DILUPBiCG: Solving for epsilon, Initial residual = 0.0486521, Final residual = 0.00112071, No Iterations 1
bounding epsilon, min: -1.14166e+14 max: 1.22753e+25 average: 2.34251e+19
DILUPBiCG: Solving for k, Initial residual = 0.611983, Final residual = 9.01935e-06, No Iterations 1
bounding k, min: -3.57866e+09 max: 3.03393e+19 average: 3.13484e+13
ExecutionTime = 1790.34 s ClockTime = 1791 s

...

Time = 12

DILUPBiCG: Solving for Ux, Initial residual = 0.00277457, Final residual = 3.62285e-05, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.00162991, Final residual = 4.10471e-05, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.00264718, Final residual = 4.61501e-05, No Iterations 1
#0 Foam::error::printStack(Foam:stream&) in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt in "/lib64/tls/libc.so.6"
#3 Foam::DICPreconditioner::calcReciprocalD(Foam::Fie ld<double>&, Foam::lduMatrix const&) in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::DICPreconditioner::DICPreconditioner(Foam::l duMatrix::solver const&, Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#5 Foam::lduMatrix::preconditioner::addsymMatrixConst ructorToTable<foam::dicprecond itioner>::New(Foam::lduMatrix::solver const&, Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::lduMatrix::preconditioner::New(Foam::lduMatr ix::solver const&, Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#8 Foam::fvMatrix<double>::solve(Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libfiniteVolume.so"
#9 main in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoam "
#10 __libc_start_main in "/lib64/tls/libc.so.6"
#11 Foam::regIOobject::readIfModified() in "/home/brblo/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/simpleFoam "
Floating point exception


I tried to play around with relaxation factors and nonorthogonal correcors without success. I would be very happy if a FOAM expert could give me some hints. As mentioned before checkMesh reports some errors but other solvers run on this mesh without problems.

Thanks
bastil is offline   Reply With Quote

Old   September 12, 2007, 03:50
Default Hi Bastil, As I allready sa
  #44
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9
vinz is on a distinguished road
Hi Bastil,

As I allready said , I got the same problems.

What I didn't mentioned earlier is that my mesh was also running fine with other solvers but not with OpenFOAM (1.4.1 at least). So I guess it's really a problem of stability with respect to cell shape.

By the way, is your mesh refined a lot at the wall? Because I also noticed that simpleFoam doesn't really like very refined meshes at walls.

I would also be interested in openfoam expert solution toughts on the subject.

Vincent
vinz is offline   Reply With Quote

Old   September 12, 2007, 04:28
Default At first, you can try to start
  #45
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 217
Rep Power: 9
fra76 is on a distinguished road
At first, you can try to start from the potential solution.
Then, you can try switching off any turbulence model, at the beginning.
After a few iteration, switch it on again, starting from the laminar solution.

Good luck!
Francesco
fra76 is offline   Reply With Quote

Old   September 12, 2007, 05:52
Default Vincent: I have two prims laye
  #46
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11
bastil is on a distinguished road
Vincent: I have two prims layers near the walls. I do not know if this is "very refined". But in every case it is a mesh suitable for turbulence model + wall function.
Francesco: Thanks for these hints. I will try to turn off turbulence first, maybe this will help.

Bastil
bastil is offline   Reply With Quote

Old   September 12, 2007, 19:54
Default BastiL, I had better succes
  #47
New Member
 
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8
vega is on a distinguished road
BastiL,

I had better success with GAMG solver for pressure. See it in the setup files I posted in this thread.
Also, see if your initial k and eps values are reasonable
--
R
vega is offline   Reply With Quote

Old   September 13, 2007, 02:52
Default Rajneesh, I agree. I get be
  #48
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11
bastil is on a distinguished road
Rajneesh,

I agree. I get better results with the settings from Hrv:

http://www.cfd-online.com/OpenFOAM_D...es/1/4245.html

Nevertheles in 1.4.1 use GAMG instead of AMG. I have 68 Timesteps so far and it looks much better. I will keep you up.
bastil is offline   Reply With Quote

Old   September 13, 2007, 05:27
Default Hi everybody, did someone t
  #49
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9
vinz is on a distinguished road
Hi everybody,

did someone tried to change the liftDrag utility to account for turbulence. I mean replacing dragCoefficient(...) by turbDragCoefficient(...).
I face a stupid problem. For the turbDragCoefficient computation, one need to pass the turbulence model since the first function argument is:
const autoPtr<turbulencemodel>& turbulence
my question is what should I add to liftDrag.C to pass this turbulence model?

Thanks in advance.

Vincent
vinz is offline   Reply With Quote

Old   September 13, 2007, 10:42
Default I had written time ago this ap
  #50
Member
 
Rosario Russo
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 56
Rep Power: 8
ariorus is on a distinguished road
I had written time ago this application which computed at runtime the forces on a body. It is not too efficient but it should work.
It runs by this command:

ssimpleFoam <root> <case> "(patch1 patch2 patch3)"

where patch1-3 are the patches of the body you want to calculate the force on.

I run it in version 1.3 but it I verified it works with 1.4 as well (I don't have installed 1.4.1).

Hope this is useful.

ssimpleFoam.tgz

to Rajneesh: I had a quick look at the setting of the Amhmed body you posted. How did you choose turbulent parameters? I mean k and epsilon at inlet.
Why did you start by zero velocity as initial condition?
ariorus is offline   Reply With Quote

Old   September 13, 2007, 23:13
Default Rosario, Initially I had pi
  #51
New Member
 
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8
vega is on a distinguished road
Rosario,

Initially I had picked values corresponding to the turbulence intensity of 0.6 and length scale of 0.02. It gives k and eps of order of 0.1. After that I played with several other values. Simulation does blow up if these values are too much out of reasonable limits.

There is no particular reason for starting from 0. Just thats the way I have been doing at my work for Fluent simulations. This choice seems safest even though it may take little longer to converge for some cases.
vega is offline   Reply With Quote

Old   September 14, 2007, 10:46
Default Thank you Rajneesh for your an
  #52
Member
 
Rosario Russo
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 56
Rep Power: 8
ariorus is on a distinguished road
Thank you Rajneesh for your answer.

Actually I was thinking to use an higher value for turbulence intensity, but I don't know the details of the ahmed body experiment.

Are your result affected much by the turbulence set at inlet? (I'm just curious).
ariorus is offline   Reply With Quote

Old   September 17, 2007, 04:25
Default Hi Rajneesh, I come back t
  #53
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9
vinz is on a distinguished road
Hi Rajneesh,

I come back to you after I run your case.
I didn't change anything and the computation went fine to the end.
Now I would like to compute the lift and drag and I get some strange results.
Here is what I get from my liftDrag utility:

Create mesh for time = 1500

Time = 1500
Reading U

Reading p

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model RNGkEpsilon

Inlet velocity: (60 0 0)
pressure Coefficient: 0.00540718 viscous Coefficient: 0.000145663 turb Coefficient: -0.00139343
Wall patch 3 named a.forebody :
Reference area: 1 Reference length: 0.182 Total Turbulent drag coefficient: 0.00415941 Lift coefficient: (0 -0.0314594 0.00310949)

pressure Coefficient: -1.42641e-12 viscous Coefficient: 0.000213444 turb Coefficient: -0.000637851
Wall patch 4 named a.side :
Reference area: 1 Reference length: 0.862199 Total Turbulent drag coefficient: -0.000424407 Lift coefficient: (0 -0.0411145 8.50987e-07)

pressure Coefficient: -2.85131e-07 viscous Coefficient: 0.000111487 turb Coefficient: -0.000347901
Wall patch 5 named a.top :
Reference area: 1 Reference length: 0.645392 Total Turbulent drag coefficient: -0.000236699 Lift coefficient: (0 3.45158e-06 0.0261528)

pressure Coefficient: 0 viscous Coefficient: 0.000150484 turb Coefficient: -0.00048029
Wall patch 6 named a.bot :
Reference area: 1 Reference length: 0.862 Total Turbulent drag coefficient: -0.000329805 Lift coefficient: (0 -1.36859e-07 -0.0361365)

pressure Coefficient: 0.00288352 viscous Coefficient: 3.65491e-05 turb Coefficient: -4.66086e-05
Wall patch 7 named a.baklite :
Reference area: 1 Reference length: 0.216612 Total Turbulent drag coefficient: 0.00287346 Lift coefficient: (0 1.51287e-06 0.0129836)

pressure Coefficient: 0.0133659 viscous Coefficient: 3.91805e-07 turb Coefficient: 0.000242045
Wall patch 8 named a.rear :
Reference area: 1 Reference length: 0 Total Turbulent drag coefficient: 0.0136083 Lift coefficient: (0 -1.37909e-05 5.13891e-06)


One thing to notice is that I prescribe a reference area of 1m². So the numbers have to be divided by the real frontal area of the ahmed body which in your case is 0.5x0.288x0.389 (because it's a half body,am I right?).
So, to obtain the pressure coefficient for instance, I sum all pressure coefficients of each body part and divide by the number explained above. Then I get a rounded pressure coefficient of 0.387 which is exactly twice as yours. The same can be done with the viscous coefficient and I obtain 0.012 which is also twice as yours.

My questions are then, are your drag coefficients computed using the half body frontal area or the whole frontal area? are my computations wrong? Where is my mistake?

Thans a lot for your help.

Regards,

Vincent
vinz is offline   Reply With Quote

Old   September 17, 2007, 09:33
Default Vincent, Its quite possible
  #54
New Member
 
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8
vega is on a distinguished road
Vincent,

Its quite possible that I am using area for the
full body. We have to use the half model frontal area, exactly as you mentioned. I will check it from home tonight and let you know

I had modifed the computeForces.H program by hardcoding the area
value (full body area = 0.1120). I have been lately using full model as well to see if the symmetry assumption makes any difference. The Fluent setup that predicted Cd exactly for 12.5 deg body is way off for this 30 deg model.

BTW if you are interested here is full mesh model for 30 Deg Ahmad body.It should be available on this link for next two-three days.

http://download.yousendit.com/09F309E86E2932AB

Rosario: I was playing with various turbulence conditions to see if the solution converges or blows up. I never really ran it long enough to get final values.

All: I am still trying to figure out best schemes for the second order accuracy for external aero simulations. Please post your observations.
--
Rajneesh
vega is offline   Reply With Quote

Old   September 17, 2007, 10:59
Default Ok, so I guess the drag coeffi
  #55
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9
vinz is on a distinguished road
Ok, so I guess the drag coefficient you gave before in this thread should be multiplied by 2.

This actually closer to the results I get by using my own mesh.

Unfortunately this is not a good news since it is twice as large as ahmed results. And this factor 2 is very disturbing.

I'm going to download you 30° mesh and run it to see if we obtain the same results (i.e. drag coefficient twice as large as ahmed for a 30° slant angle).

Anyway thanks a lot for sharing your work.

Vincent
vinz is offline   Reply With Quote

Old   September 18, 2007, 00:00
Default Yes, confirmed I was using are
  #56
New Member
 
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8
vega is on a distinguished road
Yes, confirmed I was using area of the full model.
So Sorry for the confusion.

By changing to second order schemes, Pressure Cd does come down to 0.320 (with correct area) but it is still quite far from the experimental values.

--
R
vega is offline   Reply With Quote

Old   September 18, 2007, 04:53
Default Hi all, I started working o
  #57
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11
bastil is on a distinguished road
Hi all,

I started working on the half model from Rajneesh yesterday.First calculations went fine. Concerning the differences we should consider the following (I do not have th evalues of th ehmed experiment...)

1.) Make sure drag/lift is computed correct. Which tools are you using? I can not find any of the draglift tools in OF 1.4.1, are they? Where can I get them?

2.) Get rid of mesh-dependencies concerning near wall resolution and farfield. I guess mesh from Rajneesh is nice but hexcore mesh would be nicer. Also wake and stagnation point refinements are the key to validation.

3.) Turbulence modelling is another key.

BastiL
bastil is offline   Reply With Quote

Old   September 18, 2007, 05:54
Default Hi everybody, So, unfortuna
  #58
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9
vinz is on a distinguished road
Hi everybody,

So, unfortunatly I was right, the drag coefficients were wrong. But as you said, Rajneesh, by changing fvSchemes we get closer to the right values. Actually I changed the schemes to these ones:

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 SFCD;
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;
}


and I'm getting a value of 0.27 (using th right area) for the drag coefficient which is not so bad. I'm still playing with the schemes to find the best ones to use.

Then, we'll have to find the best turbulence model to see if we get better results as Bastil has mentioned.

For the liftDrag utility, I use one I found on this forum. Use the search command to find the thread, there is an explanation on how to install the liftDrag tool on previous version of OpenFOAM (and this also works with 1.4.1).

Vincent
vinz is offline   Reply With Quote

Old   September 18, 2007, 16:18
Default A good news I guess Fluent si
  #59
New Member
 
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8
vega is on a distinguished road
A good news I guess
Fluent simulation for the same mesh (0.63 Mill Cells) as used for OpenFoam predicts Cd of 0.309.
Now OF results do not look that bad. Fluent model
of ~3 Mill cells gives same result as test. I will
try that on my machine sometime soon.

From now on, I will be uploading interesting results, flow vis comparisons to the googlepage site
linked in my profile.
vega is offline   Reply With Quote

Old   September 18, 2007, 16:53
Default Actually, yes, it looks like a
  #60
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9
vinz is on a distinguished road
Actually, yes, it looks like a good news.
I didn't understand how OpenFOAM was so far from Fluent, but the mesh difference is certainly one of the reasons.

I'm waiting forward to see what you get. I'll keep you updated if I find better results with other shemes.
vinz 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 15:29.