Hello,

I am investigating the flow in the cooling system of a racing car. I am modeling the front section of the car and the internal ducting, inside a control volume. What turbulence model is best to use here? What turbulence specification method should i choose?

Do you need more details?

Thanks,

Oliver.

(1). The turbulence model, the geometry model as well as the mesh model, all need to be "modelled". (2). The turbulence model depends on the solution you are trying to find. So, each case is unique. (3). If you don't want to model the turbulence, you can pick some existing ones to see which one is better for you. I am assuming that you will be able to determine which solution is better than others based on the computed results. (4). The turbulence model is calibrated based on some existing flows (not the one you are trying to solve I think), so, using those in your flow calculations would generate unknown results. (5). So, what the expert would do is to use the desirable flow field data as the target and adjust the turbulence model to fit the data. In general, it is called the "turbulence modelling". It is a field similar to the geometry modelling, except that it deals with physics rather than geometry. It is like asking question: " Can I use a flat plate to simulate the flow over airfoil?" In general, the answer is no. But as a first try, you could. (6). The solution is in your hands, not in the code.

Start off with standard k-e and wall functions. Try and keep the y+ values in a reasonable range (< 500).

I am assuming that you have modeled the nose of the vehicle, wheel wells, suspension, engine, etc.

So, chances are you have some ugly geometry with air as a working fluid. What you will predict, will be an approximation to the actual flow characteristics.

Once you have the model running you can change turbulence models and compare (rng, realizable k-e).

Chinor

Thanks for your help John and Chinor.

Chinor,

I am modeling the nose of the car, however the engine is in the rear so the air enters the inlet duct at the front, passes through the rad. and exits over the top of the nose, it is not interupted by the suspension.

I will begin with the standard k-e model, but should I use intensity and length scale (and if so what value should i take for l?) or should i use intensity and hydraulic diameter?

Thanks again for your help.

Regards, Oliver.

Oliver,

You can also specify k-e at the inlet, or intensity and viscosity ratio.

If you really do not have any idea what your conditions are at your inlet, I would use intensity and viscosity ratio.

How far upstream is your inlet?

If it is one or two vehicle lengths upstream, then an intensity of 3-5% should not be too unreasonable.

As far as viscosity ratio goes, for lack of knowing any better, a value of between 10-100 should work.

What you do not want to happen is for the viscosity ratio in the domain to get too high, as a result of poor inlet estimates. Between 10 & 100 times laminar viscosity at the inlet, is a good bet.

These are some very loose generalities and many users will scoff at this. However, you are not splitting atoms and I'm sure your boss would like you to gravitate to an answer.

With that in mind, have fun!

Chinor

I would go for a Realizable k-eps, with a Non-equilibrium wall function.

Concerning the boundary conditions, what was said by other people makes sense.