CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   CFX 11 Scheme for LES in Multiphase (http://www.cfd-online.com/Forums/cfx/27065-cfx-11-scheme-les-multiphase.html)

Man February 25, 2009 03:07

CFX 11 Scheme for LES in Multiphase
 
Hi

I am working on an academic problem involving use of LES for multiphase systems. For LES Single Phase, the Central Difference Advection scheme is available, but this is not the case for Multiphase. Can anyone from CFX support, let me know as to how i can turn on the Central Difference Advection scheme for LES Multiphase system. This was i tink possible with CFX 4 and 5. Also, what scheme would be a better alternative to CDS (higher order scheme that won't lead to diffussion), is it High Resolution or Blend Factor around 0.75 or 1. Can anyone please clarify. Thank you for your help. Regards, Mandar

Man February 25, 2009 19:53

Re:
 
Hi Glen , do you have any knowledge of this. I have gained lots of info through your various posts. Thanks.

lkf February 25, 2009 23:10

Re: CFX 11 Scheme for LES in Multiphase
 
My understanding of HRS is that the blend factor is adjusted locally to be as close to 1 as possible, whereas a specified blend factor of 'x' will be enforced throughout the entire domain.

So, from an acedemic perspective, specified blend factor = 1 would be preferable to HRS. However, the difficulties associated with getting a tightly converged solution using specified blend = 1 may be very difficult.

Perhaps there is a way to create an isovolume in POST that shows beta values above a certain value? Then you could visualise how much of your domain is/isn't near a fully CDS solution while still taking advantage of the stability of HRS.

Glenn Horrocks February 26, 2009 17:44

Re: CFX 11 Scheme for LES in Multiphase
 
Hi,

(It is nice to be loved :) )

High res differencing uses second order differencing where-ever it reckons it will not generate too unphysical an overshoot and for those locations blends in first order upwinding. This is discussed in the documentation. You can also see the areas where it is blending the first order differencing with the ".beta" variables.

But if you are doing LES then forget high-res differencing scheme, it is too diffusive in most cases.

The hybrid differencing scheme, even set to pure second order is still too diffusive for most LES work as it is still an upwinding scheme (although a lot less diffusion than a first order upwinding scheme).

CFX has the central differencing scheme, it is just not available in CFX-Pre. You have to put it in the CCL. If you look in the file (CFX ROOT)/etc/RULES you will find an entry "SINGLETON: ADVECTION SCHEME". This will list all the available differencing schemes and central differencing is one of them.

For most LES work you will need CDS to eliminate numerical diffusion.

You may also be interested in my PhD thesis where I did soem preliminary LES work on CFX4 where I used a second order upwinding scheme to provide my sub-grid dissipation rather than a sub-grid model. I think the study was in chapter 5 or 6. http://hdl.handle.net/2100/248

Glenn Horrocks

Man February 26, 2009 20:36

Re: CFX 11 Scheme for LES in Multiphase
 
Hello lkf and Glenn,

Thank you for sharing the information. It was very useful. I will have a look at the .beta profile for my present runs. Thanks. For my future simulations, I manually changed the advection option to 'Central Difference' in ccl and imported it to CFX-Pre 11. I get an error in Pre "This does not match any of the allowed values, and while saving the def file, it says that the definition file may not run in the solver. But, it is running and I can see the advection scheme coming printed as 'Central difference'. So, any idea, is it indeed running the Central Difference? Thanks for the help.

Reg, Mandar

Glenn Horrocks March 1, 2009 18:18

Re: CFX 11 Scheme for LES in Multiphase
 
Hi,

CFX-Pre does not support CDS so it will give an error. The solver does and should work fine. Just check the CDS scheme is actually being used and Pre has not overwritten it - check the CCL statements at the start of the output file.

Glenn Horrocks

mixer March 30, 2009 23:32

Hi

Can someone plese let me know on this. Is there a bug in CFX 11 LES runs, even though i select the turbulent kinetic energy and dissipation variables in tranres and tranStat files, it doesn't get written in ouput result files. Thanks.

Reg,
Mandar

LSC May 19, 2009 00:31

Hi, I faced the same problem as I wanted to select the Central Differencing but from the manual this scheme is only available for LES..Is there any guide to work around with it as I want to study the effect of different discretization schemes for my airfoil simulations..

mixer May 21, 2009 00:58

Hi LSC

There sure is. You just have to write in ccl file 'Central difference' and import it back. While saving the solver definition, you may see an error and an warning, but you just ignore it and save it. It works.

ghorrocks May 21, 2009 01:31

Quote:

Originally Posted by mixer (Post 211341)
Hi

Can someone plese let me know on this. Is there a bug in CFX 11 LES runs, even though i select the turbulent kinetic energy and dissipation variables in tranres and tranStat files, it doesn't get written in ouput result files. Thanks.

Reg,
Mandar

Hi,

In an LES simulation the turbulence kinetic energy is calculated directly from the velocity field, it does not have a separate variable. Unless you are using a sub-grid model which includes a k component, then it should be available. I think the default SGS model is Smagorinsky (not sure) and that does not have a k component.

Glenn Horrocks

LSC May 21, 2009 06:06

Hi Mixer, thanks a lot for the reply! Anyway is there any way I can activate incompressible flow in CFX? Also, I was rather confused about the reference pressure in CFX. From the manual it says that the reference pressure is the absolute pressure reference datum. So since I am taking perfect vacuum pressure as reference, Shall I set the reference pressure under the domain fluid model to 0[Pa] and proceed on to get my outlet BC's relative static pressure to 101325[Pa] since I am running simulations for airfoil. Is this the correct way of setting? Is there any difference between this "Reference Pressure" and the "Operating Pressure" found in Fluent? Please advice.:confused:

mixer May 25, 2009 02:45

thanks glen. I checked with 12 version also, as u said even this does not give kinetic energy as a separate variable. If i wish to obtain an averaged turbulent kinetic energy in post, then is their any user function/user routine which will help me get mean of a field. i may need to get fluctuatiing velocities at each time step to calculate kinetic energy, and to get its mean. Similarly, for energy dissipation rate, where i will have to use stress.
thank you,
regards
Mandar

Quote:

Originally Posted by ghorrocks (Post 216808)
Hi,

In an LES simulation the turbulence kinetic energy is calculated directly from the velocity field, it does not have a separate variable. Unless you are using a sub-grid model which includes a k component, then it should be available. I think the default SGS model is Smagorinsky (not sure) and that does not have a k component.

Glenn Horrocks


ghorrocks May 25, 2009 20:26

Hi,

Yes, the transient statistics output will be useful for you. Have a look in the output tab on CFX-Pre and select the transient statistics. You can then calculate time averaged flows, time averaged variances (which can be used the calculate k) etc.

Glenn Horrocks


All times are GMT -4. The time now is 07:41.