[DaveR]

Hi all,

I've been trying to verify a 2D simulation against literature by considering drag coefficients. I have a rectangle in an air flow field of velocity 27 m/s. As such I calculate a very high Re number, therefore I'm using a k-e turbulence model with initial conditions estimated using these guidelines (k= 5.35, e=0.679). To setup my case I have modified the motorbike tutorial.

The data i'm trying to validate against is the table shown on page 20 of BS5400-2.

To compare to my scenario, if length = 18m and width = 2.55m then t/b=18/2.55= 7. For 2D the height is taken to be very large, so assume h/b=40. Therefore CD=1.1. However in my simulation I consistently get CD's within the range of 0.05-0.008, depending on what minor changes I make. Residuals look good (e-6 - e-7), however are obviously converging around the wrong value!

It seems like this should be a simple exercise however it has me stumped. Can anyone suggest what I might be missing?

I've attached my case here if it is of interest.


Thanks and best regards

[piu58]

Do you simulate compressible or incompressible?

If incompressible please keep in mind that the pressure and all values derived form it are scaled by the volumetric mass density.

[DaveR]

Hi,

Thanks for your reply! Could you explain a little further?

I've modelled the flow as incompressible due to the 27m/s flow speed. Should I be doing something with the drag coefficient due to this? I followed this tutorial a few months ago and achieved a similar drag coefficient without dividing/multiplying anything through by rho?

Thanks for your help!

Best regards

[piu58]

If you use the density of air, you have to take that into account.

Or you use a mass density of 1 and calibrate the flow situation with the viscosity: It is only the Reynolds number what counts in incompressible flow.

[DaveR]

I have used rho = 1.225kg/m^3 and nu = 15.11x10-6 m^2/s (approximate values for air at 20 deg C). For a flow velocity of 27 m/s, this gives me a Re to the order of 10^8.

How would you suggest I take this into account?

The Cd values in BS5400-2 do not appear to state an associated Reynolds number, which I found a little confusing. Does this suggest the the variation of Cd is limited for such a shape, and independent of flow conditions?

Regards

[Bazinga]

For sharp edged bluff bodies the flow is usually assumed to be independent of the Reynolds number after a certain minimum Re. I can not access the files from my phone so how did you calculate the drag?

edit:

In your forceCoeff files how did you calculate these values?

lRef 16.55; // Wheelbase length
Aref 37.2375; // Estimated (Frontal Area)

What is the reference length in the literature for a rectangular bluff blody for the cd value? Are you sure these two values are correct?

I also think that you should not worry about the pressure calculation beeing dependent on the density as you defined it in the forceCoeff file, so it should be taken into account automatically.

Sent from my SM-G950F using CFD Online Forum mobile app

[DaveR]

Thanks for clearing that up about the Reynolds number!

Also thanks for pointing out the forceCoeffs, I had got my reference area wrong. Changing this and a few other settings I get a much more amicable Cd ~ 1.05.

My next stages have been to split the rectangle up into a small square and then a rectangle (see attached images).

However, for this simulation I get a Cd ~ 0.952. How much would you suggest I can trust my results? - To me it seems the Cd for the whole body should increase, rather than decrease? I have tried adjusting the level of surface refinement but the change in Cd is trivial.

Any thoughts?

Thanks again for your help and best regards

mesh-rectangle.png
mesh-shapes.png

[Bazinga]

Are we now talking about the drag of the second body?

The second body is now in the wake flow of the first body so I would assume that the drag decreases because of this.

[DaveR]

Thanks for the speedy reply!

I'm not sure how OpenFOAM interprets the shapes, but essentially both the square & rectangle are loaded into snappyHexMesh as a single .stl file named "body". My forceCoeffs file references "body" for taking measurements - so I guess it's working out the average across both shapes?

If I were to separate them, I guess I would see the initial square with a similar Cd as the first simulation (long rectangle), and the rectangle in the wake as quite low. Ideally I'd want to analyse them as one entity however, if that makes sense?

The model is similar to a birds eye view of a articulated lorry. It's known that the gap between the cab and trailer increases turbulence & drag - So would this not be reflected in my results in comparison to the first simulation of the long rectangle?

[Bazinga]

I am not sure if the average of both cd is calculated. I would assume the sum, though. I would just test it with two bodies if I were you.

Sent from my SM-G950F using CFD Online Forum mobile app