Turbulent kinetic Intensity greater than 100%
 

Hello,

I am modelizing a gas flow through a Laval nozzle. (the flow become supersonic) with a 2D axisymmetric model. I started the simulation with a laminar flow to ease convergence. Then I want include Turbulence in my model.

I read enough the FLUENT documentation and my former turbulence courses to understand the main ideas of the different models available. The RMS model being quite unstable, I decide, in order to complete my converged-laminar-solution, to set up a k-e model with enhanced wall function ( my mesh is not wall-resolved). My max Reynolds number being ~50 000 and considering the hydraulic diameter, I set a Intensity of 5% at inlet and outlet.

The solution converged quite well, with physically coherent results, and the flow pattern is not deeply changed from the laminar solution. But by plotting the Turbulent intensity, it appears that my TI is ~1e6 on almost all the nozzle domain ! The TI should be between 0% to 100% or maybe I misunderstood something very important, how is it possible ? I wonder wether the supersonic flow can make the turbulence model incorrect ?

Thank you

Florian

This indicates that your solution is not fully converged if every thing else is OK.

Thanks, but the residuals of the Turbulence parameters (k and epsilon) converge as well, reached 10-5, just as the other residuals. And my intuition is that a 10000% of turbulent intensity should totally deteriorate the flow pattern and the flow should appear as a big mess, am I wrong ?

Florian

With a Re number that you mentioned, the whole inside of domain is naturally a mess and turbulent intensity gets very high. I do not suppose that it's wrong since your parameters converged.

Best regards.

can a turbulent intensity goes beyond 100%? What does this physically mean?

The turbulent intensity is defined by Uturb/Uavg : ratio of the turbulent velocity with the mean flow velocity. I read everywhere than TI = 10% is already a quite turbulent flow, but of course, nothing mathematically prevent Uturb (named u' in ANSYS help if I remember well) to be bigger than Uavg, except maybe if some high order term in (Uturb/Uavg)^(n) are neglicted to derive the averaged Navier Stokes equation and the other turbulent-relevant equations, but I don't think so. Imagine a fast flow going rigth into a wall perpendicular to the flow direction. At the stagnation point, the turbulent flow is way higher than the mean flow, isn't it ?

I would like plot actually separatly Uavg and Uturb, is it possible ?

[QUOTE=FlorianM;390764]The turbulent intensity is defined by Uturb/Uavg : ratio of the turbulent velocity with the mean flow velocity. I read everywhere than TI = 10% is already a quite turbulent flow, but of course, nothing mathematically prevent Uturb (named u' in ANSYS help if I remember well) to be bigger than Uavg, except maybe if some high order term in (Uturb/Uavg)^(n) are neglicted to derive the averaged Navier Stokes equation and the other turbulent-relevant equations, but I don't think so. Imagine a fast flow going rigth into a wall perpendicular to the flow direction. At the stagnation point, the turbulent flow is way higher than the mean flow, isn't it ?


It is. Extreme fluctuations could result in high jump of u'.

It is logical and I agree.

Hi all,

I had some problems with the turbulence intensity myself. One suggestion that could resolve the affair is that FLUENT is apparently not normalizing the u' on the local mean velocity but on a velocity selected in the "Reference Value" tab.
So, if your inlet velocity is relatively small compared to the maximum velocity found in the domain and you chose inlet section as your reference value, unreasonably huge intensities will appear due to the high fluctuation velocities are not normalized on the high local mean velocity, but on the rather small inlet velocity.
If the flow is looking as expected and the other values are realistic, I would not worry too much.

It is just a postprocessing problem after all...

Yes, correct. How to overcome this issue in Fluent?

Turbulence Intensity
 

You can go under Report tab in Fluent 14.5 and select "from inlet" in Compute form. Also, depending on the length scale of the your problem change the value of Length. Run the solution of a few iterations. It will give you reasonable values of Turbulence Intensity.

I just thought i'd throw some of my thoughts into the mix here. Theoretically, the turbulence intensity is a function of k and U. And if you're getting values over 100%, the results are pretty much rubbish ( as with most CFD results lol). You've mentioned that you have used the k-epsilon turbulence model. This eddy-viscosity turbulence model calculates your dissipation rate thru the eddy viscosity ratio. If you've received some warning during your calculations saying turbulent viscosity ratio limited to 1e-6 or something like that, chances are your k values are wrongly calculated. Not sure if it might help you but just something i would just like to share.

Defining custom field function:
will give you turbulent intensity (fractions).
You may multiply it by 100 to get TI as percentage.

Hello,

If the model analyzed has re-circulation i.e. very low velocities then there might be large turbulence intensity at the points of re-circulation.