Default inlet boundary conditions for turbulence

Hi everyone,

I've got a question turning in my head for which I can't seem to find an answer in all the documentation and forum about code saturne.

When I set the boundary conditions for the inlet in the GUI, for a calculation using turbulence (not for laminar flows), I can specify the hydraulic diameter of my problem, and the turbulence intensity at the inlet.

For some cases, I've have access to the value of the turbulence intensity at the inlet, so I can give it to Saturne.
I assumed when I specify this value, Saturne use it to find the distribution of k and epsilon (or Rij or another variable of the model considered) based on the laws given in the litterature (k=2/3(Uref Ti)² for example).

My question is : when I choose to give only the hydraulic diameter, what laws (or what default value) does Saturne use to get the distribution of the turbulence variables at the inlet ?


I had a look at the routine usclim.F, and there is an example in which the calculation of these variables at the inlet whitout the turbulence intensity is based on the laws for turbulence in pipes. But what happens when the calculation is not for a flow in a pipe ?

I use Code Saturne to run calculation of flows around different shapes of buildings, so it is always external flows and not internal flows. So another question raises here : what about the hydraulic diameter of the problem in the case of external flow ? (I assumed it's based on the inlet face 4*surface of the inlet/perimeter of the inlet)

Anyway these questions don't prevent me from running any calculation, they are just details which are not very clear for me.

Thanks in advance for your always helpful and informative answers !!

Alicia

Hello,

As you have seen in usclim.F, the code calls a routine keendb, defined in src/base/turent.F.

Using a hydraulic diameter and this function, the formula used is always that for a circular pipe, so it might not always be the best choice.

Similarly, for an external flow, the choice of the hydraulic diameter is up to you. You may use a formula based on the inlet perimeter, or set it to the largest possible vortex size, but either way, its definition/interpetation in external flows is not trivial.

Ideally, your inlet could be far enough from the area in which you are interested in, so that turbulence may "establish itself" naturally (which may take some time if your geometry is very smooth, less if it has many obstacles, so in a case with buildings, the results may be sensitive to your inlet turbulence for the buildings or obstacles most upstream, but not so sensitive for those downstream from those).

Best regards,

Yvan

Hi Yvan,

Thanks a lot for your answer. Things are much clearer now !

I had a look at the turent subroutine in which the function keendb is defined (as well as the function keenin), and I can adapt them to my cases whenever I need to

Best regards,

Alicia