Eddy Dissipation Rate for LES
Hi,
I want to extract eddy dissipation rate for LES model. I do not understand how to do it. I have the required formula in front of me which says: total edddy dissipation rate for LES = e = (Mut+Mu)/2*(du'/dy+dv'/dx)^2 I don't understand how to post process that? I am using v12.1 of CFX. Any help will be appreciable. Thanks 
Common guys! noone has any idea? A little hint will be useful!

Do you want to evaluate it over the whole domain (ie create a field variable) or just at certain points or get a global value?

i want to evaluate it both locally and globally.

Evaluating u' will be tricky. If you want fixed points you can get it by taking a moving time average of a monitor point but I can't see an easy way of doing it spatially. You will probably need user fortran to do this, and even then it will be tricky.
You may be able to determine a sort of bulk flow velocity by mapping the velocity field to an additional variable with some dissipation on it. If you adjust the dissipation to give an appropriate level of smoothing this can give you an smoothed velocity field which you can then evaluate u' from. This might work. So it is easy to evaluate it a monitor points as a post processing operation. 
understood the method of obtaining the epsilon for LES
Please refer to the article
http://leskandepsilon.blogspot.com/2...yforles.html This article is based on the understanding of how to obtain epsilon for LES. Cheers 
hello Rsin,
I want to calculate turbulent dissipation rate in LES in fluent 14. I looked at the article you suggested in your post above but couldn't understand. Could you please give me some step by step calculations on how to do it in fluent? Thanks, 
turbulent dissipation rate in LES
Hello,
No one has any idea of how to calculate turbulent dissipation rate in LES in FLUENT 14? 
In the CFX forum, correct, we have no idea how to do this in fluent.
Try the fluent forum. 
yes there is a simple way
Dear maphd,
thes easiest way is to create a plane (otherwise the instanteneous data will be too much for each timestep, offcourse, the mean values can also be extracted at what ever timestep you want, i prefer instantaneous at each time step and mean (after each complete revolution)) in which you want to extract the data, so then select the 9 gradients of the velocity (along with any other aspects you want) to be extracted in that plane and the mean for the whole geometry. Now, use matlab etc to create the EDR equation of the 12 gradients as shown by Adrian and Sharp for their PIV estimations. 9 graidents are available and the 3 gradients are constructed using the available ones because those are crossproduct gradients. Just remember to have sufficient amount of timesteps to achieve statistical convergence of the data. this convergence can be done using the extracted data in matlab etc. is it clear? Most importantly, it can be done in Fluent but not in the CFX. Otherwise, going more theoretically, create gradients by yourself from each of the velocity components based on your grid (still these velocity components need to be extracted as well in a plane (instantenously) or whole geometry). Cheers 
Not that it matters since the work will be done in Fluent anyways. Could you please describe what cannot be done in CFX out of the workflow you described ?
The extraction of variables at a plane during the simulation ? or the extraction of the gradient variables during the simulation ? Otherwise, it seems just a series of formulas to be evaluated. Thank you.. 
Dear Opaque
CFX just doesnt give this option of the 9 gradients of the velocity to be extracted (i dont know if has changed in the lastest version till v 15, there wasnt such an option). These gradients will have to be estimated manually by creating them with the mesh size and the velocity components which will be extracted.
Extraction of variable can be done with ethe CFX as well, just there arent these 9 gradients available to be extracted. Is it clear enough? Fluent provide all these options. Cheers 
Thank you..
Just for clarification, the access to gradient components for variables has been available since CFX5.5 (pre ANSYS CFX) via UserFortran, and since ANSYS CFX 11.0 via CEL using similar syntax as used in ANSYS CFDPost. If the direct access fails, you can always copy the variable into an additional variable and access the gradient of the copy. A gradient component is available by using Code:
[FluidSolid].[Material Component].<VariableAdditional Variable>.<Gradient XYZ> 
Thank you!
I perhaps never paid that much attention at the time i used to be working with CFX. In Fluent its direct. Thanks anyways. Should help newcomers..and in the future!! 
All times are GMT 4. The time now is 12:10. 