Just wondering if anyone out there has successfully used 2 different turbulent models on 2 domains? Does CFX even allow this? I have already tried editing the CCL file in Pre but the .def file is always changed to use the turbulent model of the first domain.

thanks

steve

Hi,

Yes this is a hidden functionality in CFX. You can do the following: (note description is for Windows you can do the needful on other operating systems)

CFX-pre only allows constant physics in different fluid domains. To over-ride this behavior of Pre, you need to set an Environmental variable before you open Pre. This variable ones set will allow you to use different physics in different domains. Attached are a few slides which discuss this feature in brief.

To create the Environmental variable on Windows-2000 machine, (Note: You should log in as administrator for the following)

1. Right click on the My Computer icon on the desktop. Click on Properties -->Advanced --> Environmental variables.

2. Click on new in the System variables.

3. In the name toggle which pops up, type CFX5_NO_CONSTANT_PHYSICS for the name of the variable and in the values toggle type T.

4. Click Ok and Apply. Log off the computer and log in again. This procedure is demonstrated in the word file attached.

· Once the environmental variable is defined and you are logged off and logged in again into the computer, you can open pre and set up two domains with different materials and even different physics. (Like one flow being laminar and the other being turbulent). You can get a warning message in Pre, but you can neglect the same. However you need to also swith on the expert parameter: check isolated volume =f

Hope this helps

Hi,

I'm just curious of why you need to apply two different turbulence model in your case? I've doubt if this will cause some numerical instability for the solution. Please let us know if you get any reliable result using this approach. I haven't got any publication that use the turbulence model this way.

Hi,

I think that it may make sense if, for example, there are 2 fluid domains separated by a solid domain.

However, if the 2 fluid domains are connected and you use 2 turbulent models, how (and where) do you set the boundary conditions for the turbulent equations?

Rui

This is interesting and all but what boundary conditions do you then use for the turbulence equations on the domain interface????

I'm not sure why you would want to do this anyways because from a modelling standpoint, connecting two fluid domains with different turbulence models does not make a lot of sense.

Hi,

k-e model & RSM may use the same method for boundary condition (eg. specify k & e). However, I haven't had anything in my mind of how e-based model can be used together with w-based model. Their near wall treatment is not the same on the way.