Flow through a 90°pipe bend
 

Hi,


I do a simulation of a turbulent flowthrough a 90°pipe bend (Re = 10^6) with Ansys CFX. But, I'm not sure about the turbulence quantities to impose at inlet boundary conditions because on the upstream of my computational domain, there is two other 90°pipe bends (it's a test bench). And, we know that the turbulence intensity at the inlet is totally dependent on the upstream history of the flow. It is difficult for me to know/understand what combination of intensity and turbulent length scale is the better representation of the physical reality? Is it I=5%;Lt=10%Dh or I=5%;Lt=Dh, and so on ?


Thank you very much for your help

There are a few ways to approach this:

* This shows you do not know the flow conditions at the location you selected your boundary condition - so you cannot put a boundary condition there. You should move the boundary condition further upstream to a location where you know how to specify the flow. In this case that might be upstream of the two 90 degree bends.

* It might not matter anyway. If you try several reasonable guesses of what the turbulence condition is you may well find it makes no difference to the flow anyway. Then you can choose anything you like because it does not matter.

Thank you for your response !

The first point which you mentioned is not possible for me but I had already done the second point. And it seems that it changes nothing for the quantity of interest I look. But why ? Is it because turbulence is created primarily in shear layers ?

Despite I can choose anything because it doesn't matter, I would like to know your opinion on what reasonable guess of turbulence conditions (It-Lt) is the most realistic to have at the inlet of my computational domain ?

Turbulence (where ever it comes from) increases effective viscosity and diffusion. But if the viscosity and diffusion are small and not a big contributor to your flow then your turbulence model won't change much.

The choice of turbulence boundary condition needs to match your device you are modelling. I have no idea about the details of what you are modelling so cannot comment. But things which might help are:
* Turbulence intensity, as a % of flow energy. You may have this data.
* Length scale - if you don't know the length scale then you can guess based on the dimensions of the device.

But I would not bother thinking about it too much if it does not matter. Do a reasonable guess, show that it does not matter and that would be good enough for me.

Thank you very much for these useful tips. But, I would like to ask you another question.

I found on Wikipedia and here on CFD-Online wiki too that the turbulence intensity at the core of a fully-developed duct flow can be estimated from the following formula: I = 0.16 Re^(-1/8). Moreover, an approximate relationship between the turbulent length scale and the physical size of the duct is found: Lt = 0.07 L. (Generally, L is based on hydraulic diameter)

Do you know, where are these relations coming from ? I have searched in litterature but I have not found it.

Thanks a lot for your help !

I do not know where those references come from. You would have to chase that up from the page you got it from.

You can get who wrote that stuff from the wiki page (look at the edits made on the page) and you might be able to contact the person directly.

That is what I have been using, except for CFX I believe the turbulence length scale is 0.038 * Dh instead of 0.07, which is for Fluent.
Here is my calc sheet I use for internal pipe flow. Left side (blue) is calculating by Turbulence length scale and Intensity. Right side (pink) is calculated by specifying intensity and Viscosity ratio.