# Initial Values for Turbulence Coefficients

#21

The kinematic molecular viscosity of air can be taken as 1.5e-5 m^2/s for a wide range of applications. You can refer to this table https://www.engineeringtoolbox.com/dry-air-properties-d_973.html.

Turbulent viscosity ratio = turbulent viscosity / molecular viscosity. For incompressible flow, OpenFOAM uses the kinematic version of viscosity. In this case you have kinematic viscosity ratio (nut/nu) = kinematic turbulent viscosity / kinematic molecular viscosity = kinematic turbulent viscosity / 1.5e-5.

The kinematic turbulent viscosity (nut) is calculated by the turbulence model. With each pair of k and omege values, you will get a unique nut.

#22

I should have explained this better. The table on https://www.engineeringtoolbox.com/dry-air-properties-d_973.html contains molecular/laminar viscosity only. The molecular viscosity is a fluid property independent of the turbulence models. The turbulent viscosity is the result of turbulence modelling.

#23

No problem!

So how can I calculate or find the value of this so that I know I am within the 0.1-2 range?

#24

Hi @dylan and good to see you back!

The SA 1 equation turbulence model is adapted for flows around an airfoil and as you know boussinesq approximations to not behave super accurate (whatever you define as accurate in this case), but a contracting section is a good example as the eddies loose their identity along the way. And standard k-epsilon is by definition not realizable (need a separate post to explain what that means) so one usually uses realizable k-epsilon but fully developed pipe flow for instance work pretty well with standard k-epsilon. k-omega SST does a pretty good job and there is no need for SA model, what do you think?

Best,

Jousef

#25

Wow, Sydney, Florida and Germany all at the same time

#26

From Spalart and Rumsey, you have

Calculate k and omega using a length scale of your choice.

From this link https://www.cfd-online.com/Wiki/Turbulence_free-stream_boundary_conditions, you have

where,
is the turbulent viscosity ratio;
is air density;
is dynamic molecular viscosity of air (not kinematic).

#27

@jousefm

I exclusively use SpalartAllmaras, RealizableKE, and SST as RANS. In fact, I find SpalartAllmaras very useful for external aerodynamics with mild separation, such as a plane or a wing. I think @DaleKramer’s problem can be very well solved by SA, because I have done similar projects.

#28

Aha, I finally see it, I can just back it out from known values.

And this means I really need to go to bed now … Thanks.

Dale

#29

Hi @dylan,

I totally agree here but as SA is not implemented on our platform we have to work with another turbulence model.

Best,

Jousef

#30

@dylan

Just curious as to why you suggest calculating ut/u from the cfd_online.com formula rather than from the Spalart and Rumsey recommendation of 2e-7 * Re ?

There is a 20% difference in my case.

And by the way, I did have to change my reference length from a fuselage length of 5m to a value of 2m to stay in your suggested ut/u range of 0.1~2. My ut/u value is now 1.89 (EDIT actual value is now 1.6182, see edit 2 posts down).

Dale

#31

Did you use the same length scale in Reynolds number?

#32

Yes

EDIT: corrected the value for u (dynamic viscosity) which is equal to SimScale Kinematic Viscosity * Density

This makes ut/u = 1.6182 instead of 1.888,

Calculation of Turbulent kinetic energy and dissipation rate
#33

The 2e-7*Re is just an estimation. The actual nut calculated at inlet should return a nut/nu = 1.888 or much closer to 1.888. I don’t think a length scale of 2 or 3 will lead to much difference in Cd or Cl. It is safe to use what you have here.

#34

Turbulent viscosity and eddy viscosity are the same thing. However, nut = mut/rho, where nut is commonly used in incompressible flow, and mut in compressible flow.

#35

Hey guys.

Could you help with this? I think it might be related.

https://www.cfd-online.com/Forums/openfoam-post-processing/217884-flow-rate-phi-not-matching.html#post735070

#36

Hey @bdewar!

Is this related to a problem you have with a project on our platform?

Best,

Jousef