# Which turbulence models are suitable for CFD analysis on a streamlined vehicle body?

Many commercial and open-source CFD codes implement several closure methods for the non-linear convective acceleration term of the Reynolds-averaged Navier-Stokes (RANS) equations. Common methods (also known as turbulence models) include

Which of these are suitable for CFD simulation of a streamlined vehicle body? The purpose of the simulations is to guide the refinement of the body shape to minimize aerodynamic drag forces. An exemplary answer would briefly outline the advantages and disadvantages of each method for this simulation application.

Potentially useful details:

The vehicle is a small one-person vehicle with approximate dimensions

• L = 2.5 m,
• W = 0.7 m, and
• H = 0.5 m.

It will be travelling at speeds ranging from 0 m/s to approximately 12 m/s. All three wheels are enclosed by the body envelope, and the vehicle has an approximate ground clearance of 15 cm except near the wheels, where the body shell extends down to within 1 cm of the road surface.

Normally aerodynamic forces at these speeds are very nearly negligible, but assume that this vehicle is being designed to compete in a "Super Mileage" competition on a smooth track, is very light-weight, and uses low friction drivetrain components throughout, so the aerodynamic forces have a significant effect on the achievable fuel consumption.

The turbulence model can make a big difference in your simulation. There are many turbulence models around. It becomes a tough job to select one out of them.

There is no perfect turbulence model. It all depends on several parameters like Reynold's number, whether the flow is separated, pressure gradients, boundary layer thikness and so on. In this answer, brief information about a few popular models is given along with pros and cons and potential applications. However, interested users can see this excellent NASA website and references therein to know more about turbulence modeling.

A) ONE EQUATION MODEL:

1. Spalart-Allmaras

This model solves for one additional variable for Spalart-Allmaras viscosity. According to a NASA document, there are many modifications in this model targeted for specific purposes.

Pros: Less memory intensive, Very robust, fast convergence

Cons: Not suitable for separated flow, free shear layers, decaying turbulence, complex internal flows

Uses: Computations in boundary layers, entire flowfield if mild or no separation, aerospace and automobile applications, for initial computations before going to higher model, compressible flow computations

Applicability to your case: a good candidate for reducing simulation time. You can predict the drag fairly well with this model. However, if you are interested in knowing the flow separation region, this model will not give highly accurate results.

________________________________________________________________________________

B) TWO-EQUATIONS MODELS:

1. $k$-$\epsilon$ turbulence model:

A general purpose model. This model solves for kinetic energy ($k$) and turbulent dissipation ($\epsilon$). The equations for this models can be found at this cfd-online page. This model requires wall functions to be computed for the implementation. Suitable only for fully turbulent flows.

Pros: simple to implement, fast convergence, predicts the flows in many practical cases, good for external aerodynamics

Cons: Not suitable for axi-symmetric jets, vortex flows and strong separation. Very low sensitivity for the adverse pressure gradients, difficult to start (need initialization with Spalart-Allmaras), not suitable for near wall applications

Uses: Suitable for initial iterations, good for external flows around complex geometries, good for shear layers and free non wall bounded flows

Applicability in your case: Although this model is good for external bluff body computation, it is suitable only for turbulent flows. Since the velocities are low, flow is going to experience transition from laminar to turbulent (max $Re = 1.98*10^6$ using this calculator). You might benefit better with a variant like realizable $k$-$\epsilon$ model.

2. $k$-$\omega$ turbulence model:

Solves for $k$ and turbulence frequency $\omega$. Gives better results for near wall flows. Predicts transition (although early sometimes). Quite sensitive to the initial guess and hence initial few iterations are performed with $k$-$\epsilon$ model. This article gives near wall treatment for this model.

Pros: Excellent for boundary layers, works in adverse pressure gradient, works for strong separated flows, jets and free shear layers

Cons: Time required for convergence is more, memory intensive, Requires mesh resolution near the wall, predicts early and excessive separation

Uses: Internal flows, Pipe flows, Jet flows, vortices

Applicability in your case: Not completely suitable for your case since the boundary layer values depend strongly on free stream $\omega$. This requires a very fine grid to resolve and hence long computation time. Also it does not account for the transport of turbulent shear stress.

3. $k$-$\omega$ SST

Best of both worlds! This model has a blending function which uses $k$-$\omega$ near the wall and $k$-$\epsilon$ in the free stream. It does not use wall functions.
All the variants of this model can be found at this NASA page.

Pros: Accounts for turbulent shear stress while giving all the benefits of $k$-$\omega$ model, Highly accurate prediction of separation and transition, Very good free stream as well as boundary layer results

Cons: Not suitable for free shear and vortex flows as much as standard $k$-$\omega$, Not suitable for jet flows, Requires fine mesh resolution near walls

Applicability in your case: Highly applicable. If you want better results, use a variant of sst model which uses $k$-$\epsilon$ RNG or realizable model away from the walls

So which model is most appropriate?

My guess would be $k$-$\omega$ SST model. Since it will give better transition, separation and works even under adverse pressure gradients, you will get better skin friction drag. At the same time, it works well away from the walls, which will give you good pressure drag and hence parasitic drag. You will get better flow visualization. You can very well use the Spalart-Allmaras model, but if you see this study, you will notice how much difference the SST model makes.

And don't take my word for it. A report on 'Aerodynamic Analysis and Drag Coefficient Evaluation of Time-Trial Bicycle Riders ' uses the SST model. This paper compares all the turbulence models results for cyclist aerodynamics and arrives at a conclusion that the SST model gives the best overall results. I am citing these results because Reynold's number wise and dimensions wise, a bicycle goes most closer to your case, for which tons of studies are available.

However, if time is limited in your case, go for Spalart-Allmaras model. You can also go for RNG $k$-$\epsilon$ or realizable $k$-$\epsilon$ in that case. However, this study of a bicycle wheel shows, S-A model gives better results than $k$-$\epsilon$ (this is very much geometry specific, different model might work for your geometry). If you have all the time in the world, conduct studies using SST and epsilon model and publish your comparison so others might also benefit from it.

If you have better computational resources, go for LES. But I feel it is not called for in this case and it might not be appropriate. I do not have experience with LES, so can't comment.

Some interesting resources:

1. The FOAM house: If you want to learn OpenFOAM step by step

2. Recent advances on the numerical modeling of turbulent flows

3. Lectures in Turbulence for the $21^{st}$ century - highly recommended reading if you wish to understand turbulence

All the best!

Cheers!

I can't say that this will be the ideal answer, but it should get you started. As will be apparent, I not a true expert.

The quality of these models will generally increase with their sophistication, which in this case basically tracks with the number of equations use. So (S-A) would be least effective while k-$\epsilon$, k-$\omega$ and SST would be better. RSM would be the best.

Within the middle three, SST is (so I'm told) better at correctly predicting flow separation. The other two have a habit of not predicting separation when they should. Given that separation generally causes drag, these could result in a flawed design seeming good.

While RSM would definitely be preferred if possible, it will be the most time consuming because it adds 7 equations on top of N-S. 10 years ago, you might have had to make a tough choice here. Theses days you should be able to turn around RSM models of this kind of vehicle in reasonable amounts of time.

I've been been working on an FSAE (open wheeled single seat race car) aero design for the past couple of months and have found the use of RSM to be reasonable to run on a fairly high end laptop or any respectable gaming rig desktop. You can also find places where you can rent run time if you need to evaluate a large number of design iterations. I can add the name of a company that we used that was set up to run the software that we needed and helped us out with student prices (somebody please comment if that's appropriate for SE).

A slight tangent: I'd strongly recommend that you look for papers (ideally experimental) that you can use to validate your methods. We made very sure that we could recreate (within reason) results from wind tunnel experiments before we proceeded to running our own designs. It's also important to run mesh sensitivity analysis to make sure that your resolving the structure of the flow.

Also, prism layers coming off of your surfaces (to better resolve boundary layers) are important.

Last: this document from the folks at Fluent is a bit old, but was still very helpful in getting us started. (sorry for the scribd link.

In case you only have the resources to perform one simulation only I would agree with @Subodh and use $k-\omega\:SST$.

In case you can afford multiple simulations I would use different models and compare. This way you can identify the influence of the turbulence model in your particular application.

Could you clarify if you are looking for an optimal velocity distribution or if you are more interested in separations?