need help on defining boundary conditions for forced transition
 

Hi,

I am doing simulations on aerofoil and would like to study forced transition. On hand I have predicted transition locations and would like to separate out the laminar and turbulent at the specific transition location. I have define two zone namely Laminar and Turbulent in gambit. In Fluent, there is an option to select "Laminar Zone" for a particular fluid zone where it switches off the turbulent viscosity and production terms.

I am wondering how would I go about doing this in CFX. I have tried to create two domains (laminar and turbulent) but it does not allow me to specify turbulence models "None" for the laminar domain and "SST" for the turbulent domain. I have also tried creating a subdomain for the laminar zone but no luck so far. Could anyone shed some light?

Hi,

I have already answered this question on a previous post - you use the SST transitional turbulence model and set the transition model to specified intermittency. Then you can specify the transition point and get laminar to turbulent transition.

Glenn Horrocks

Hi Glenn,

in CFX-Pre using the specific intermittency, the value 0 corresponds to Laminar flow which I would define for the Laminar Zone and value 1 for the Turbulent Zone am I right? I have also read up on the help file which I could actually do away with splitting up my mesh into two zone by defining the transition location explicitly through the use of CCL using cartesian coordinates. I am wondering can I specify two locations as the transition for upper and lower surface of the aerofoil occurs at different locations. Please advice. Many thanks!

Hi,

You will have to read the documentation about the use of it, it has been years since I worked with it.

You are correct, no need to split the mesh.

If you are defining a complicated transition function then you are probably going to need a 3D interpolation function. Then you can specify the intermittency field as a function of X,Y and Z.

Glenn Horrocks

Hi Glenn,

many thanks for your advice. My intention is to specify a point so that the region upstream is Laminar and fully turbulent downstream beyond this point. From the help file, there is an example on the CCL code below. If I want to specify say x/c = 0.36, how to I go about implement this? Also does the y variable corresponds to the y coordinate at the specific x/c location?

Extract of the CCL code:

FLUIDS MODELS:
TURBULENCE MODEL:
Option = SST
TRANSITIONAL TURBULENCE:
Option = Specified Intermittency
Intermittency = TRANSITION TRIP(x,y,z)
END
END
END
CEL:
FUNCTION: TRANSITION TRIP
Option = User Function
Argument List = [m],[m],[m]
Result Units = []
END # FUNCTION
END
USER ROUTINE DEFINITIONS:
USER ROUTINE: TRANSITION TRIP
Option = User CEL Function
Calling Name = transition_trip
Library Name = transitiontrip
Library Path = ...
END

END

Hi,

This example calls the function "TRANSITION TRIP" which is a user fortran routine. I would not go this way unless you really need to. I would make the "TRANSITION TRIP" a CEL function, where it is defined by a 3D interpolation function. You give the interpolation function a dataset of XYZ points and the value at that point. You then dream up a dataset which is 0 in the laminar regions and 1 in the turbulent regions.

Glenn Horrocks

Hi Glenn,

which means I can directly input the function in the GUI by selecting the CEL icon? How do I generate the 3D interpolation function with the transition locations data I have?

Hi,

You generate the 3D interpolation function in your favourite number crunching software. You can do it in MS Excel if you must. Just dream up a 3D field of XYZ points and give it the laminar value in the laminar regions and the turbulent value in the turbulent regions.

Glenn Horrocks