CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Forces in 1.5 with an Ahmed VWT case (http://www.cfd-online.com/Forums/openfoam-solving/65210-forces-1-5-ahmed-vwt-case.html)

terrybarnaby June 8, 2009 16:09

Forces in 1.5 with an Ahmed VWT case
 
1 Attachment(s)
I have attempted to produce a wind tunnel test case matching the Ahmed test case using OpenFoam 1.5 (SVN from 2009.06.05).

Title: Ahmed case with 25 degree sloping rear
Tunnel: 8x4x3 meters (A bit different from the standard cases)
Speed: 40m/s

The simulation appears to be generally working, but the force and forceCoefficient values calculated appear to be far too high.

From reading around I was expecting values around:
ExpectedDragForce: 30N
ExpectedCd: 0.3

However, I am getting much higher than this:
DragForce: 53N
Cd: 0.53

I have tried many things but still come to these same values.
I wonder if anyone can see what I am doing wrong.
I have attached my current settings which uses the simpleFoam solver. My test mesh is at: http://www.greenpower.beamweb.co.uk/...ed-mesh.tar.gz

This is a low cell count mesh (about 100,000) but I have tried up to a million cells with no effect. It appears to be close to convergence after about 50 iterations of simpleFoam using the 100,000 cell mesh. Any ideas would be appreciated.

tomf June 9, 2009 05:11

Dear Terry,

I am also investigating flow around the Ahmed body, however I am looking at the 35 degree slant angle. I have found reasonable results with the k-omega-SST model, instead of the k-epsilon model. Furthermore, I have read some papers of others, who have demonstrated that the 25 degree slant angle case is a difficult case for 2-equation turbulence models. I have done two runs with a 25 degree slant angle and I could not match the experimental values, but I had a smaller error. Looking at your settings, I noticed that you used

div(phi,U) Gauss upwind;

I think you should change this to a higher order scheme. I have been using

div(phi,U) Gauss GammaV 0.4;

which gives better accuracy and remains stable (in my cases). My grids have been larger (more cells and slightly larger domain, but only half a model with symmetryplane) and I do not use a moving ground plane/tunnel walls. I would suggest to use your mesh of 1 million cells or even finer. I also noticed you have some bumps on the model and rounded edges. These may influence the results as well.

Good luck,

Tom

7islands June 9, 2009 05:51

1 Attachment(s)
Hi Terry,

I have the same impression as Tom. I tried your case with switching from simply
div(phi,U) Gauss upwind;
to
div(phi,U) Gauss linear;
I get the convergence of Cd around 0.3 as shown below (I see GammaV is recommended in another thread though).
Attachment 423

Also what I noticed was perhaps nu should be around 1.5e-05 (if I am not mistaken).

Takuya

terrybarnaby June 9, 2009 08:21

Thanks to you both :)
Using div(phi,U) Gauss GammaV 0.4; or div(phi,U) Gauss linear; worked a treat. They both appear similar with just a few iterations (200). I will have a play with them with a more detailed mesh and a greater number of iterations.

Yes, my presented test mesh is small on cell count. I have been using this for basic testing to speed up the tests. I am using a million cell mesh normally. The bumps in the 100,000 cell mesh are due, for some reason, to snappyHexMesh's algorithm's. A million cell mesh does not have the bumps.

Yes, I think that nu should be 1.511e-5 for 20 degrees C. I think the 1.8e-5 got in there when I was trying other peoples configurations to see if it made a difference.

Thanks again for the input.


All times are GMT -4. The time now is 12:31.