[terrybarnaby]

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]

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]

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).
Cd.png

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

Takuya

[terrybarnaby]

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.