Hello,

I already found a lot of hints in this forum, but for my problem i don't know exactly what my problem can be.

For my studies I have to do a research on the ahmed body with 20 degrees on the back end. This Body should have a drag coefficient from about 0.25 but my calculations have 0.45 â€" 0.5 as result. The position and the magnitude from the eddies in my solution seems to be right. The max Kinetic Turbulence Energy is in the lower eddy on the back, like in the paper i found. I am confused that my solution is twice as big as it should be.

Maybe someone sees a big mistake in my settings or can give me a hint how I can find the problem.

I already tried different mesh sizes and refinements, but it hasn't changed something. I am using Tetra Meshing with Prism layers on the body. The Element size on the Body is 10 mm, with 5 prism layers with ratio 1.2 and first height of 2 mm. My last mesh had approx. 800000 Elements. But with other meshes i already had 2*10^6 Elements, the change was verry small.

My Boundaries are:

- Velocity Inlet with 40 m/s, the rest is standard settings

- Pressure outlet with gauge pressure 0 pa

- Symmetry

- Ground is wall with defined shear stress 0

- Walls are symmetry

Models are:

- Solver: pressure based and green gauss node based, rest is standard settings - Viscous: ke; realizable; non equilibrium wall function,

Solution controls are:

150 iterations standard settings (first order) then second order and coupled for pressure velocity coupling with standard parameters.

I checked my reference settings and scaled the mesh and for the drag coefficient I used the force in x direction.

With best regards,

Michael

Did you use the correct reference area?

I used the Projected Areas function in x direction. I get 0.056 m² which is the half of the entire area (0.112m²).

If i calculate with symmetrie, the Forces are only for the half body, aren't they? The velocity is also right. Density is 1.225 kg/m³ and viscosity 1.78e-5.

As result i get 27 N pressure force and 2 N viscous Force on the half body at 40 m/s air speed.

How are you specifying turbulence at the inlet? How big is your 'tunnel', i.e. what is your blockage factor? What is predicted average pressure at the inlet? What is predicted max Cp at stagnation?

Inlet turbulence:

- turbulent intensity 2% - turbulent lenght scale 0.1 m

tunnel: 3m in front an 5m behind the body = 10 m. 2.5m high and 2.5m large, that gige a blockage factor of 0.9%

an absolute pressure plot at the inlet shows 1.013e^10 pa on the entire inlet (small place has an higher pressure, approx 0.5 pa).

i am not sure if i understood the thing with the cp right. a force report give a cp of 0.47.

best regards

i plotet a cp contour on the body. the cp at the nose was 1, the cp at the fillet on the upper and down side of the nose was -2.5. i also found a paper with some pictures of results. Pressure plot on the symmetry, pathlines at the back are pretty close. the turbulent kinetic energy plots at 4 cuts behind the body are a bit different, but the guy used a different viscos modell. the biggest difference was 1.5 m behind the body

i found a big problem in the modell of the body. the two vertical fillets on the front where missing.

Now i have a cd of 0.32 and i am searching the next 20%.

sorry for this needles posts.

best regards

In the CD-adapco products, both STAR-CD and STAR-CCM+, I set the ratio of turbulent viscosity to laminar viscosity at the inlet to be something on the order of 1 to 10. Too much more and your fluid starts acting like molasses. See if you can come up with a scalar plot of the ratio at the centerplane. It should be your inlet value till somewhere close to the vehicle. External aerodynamic analyses can be pretty sensitive to initial and inlet turbulence values.

Micheal Ditto what Paul said.

You want a viscosity ratio less than on. Lockheeds low speed tunnel (which is pretty typical) has a viscosity ratio of 0.3 (in fact that might be 0.03) Ie the turbulent viscosity is less (perhaps much less ) than the molecular viscosity.

I learned this one the hard way. Go back to the source paper and see if there is any estimate of tunnel conditions. The turbulent intensity should be very low 1% or less and the length scale in a tunnel is the lenght scale of what ever the smallest feature of the flow straighteners (screens)

Good Luck

Andy R