[LSC]

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?

[ghorrocks]

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

[LSC]

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!

[ghorrocks]

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

[LSC]

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

[ghorrocks]

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

[LSC]

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?

[ghorrocks]

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