CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

How to set and control the turbulence in CFX?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   November 14, 2006, 03:15
Default How to set and control the turbulence in CFX?
  #1
Wei
Guest
 
Posts: n/a
I'm making a one stage simulation of steam turbine in CFX. I tried to set different Inlet boundary turbulence condition such as intensity, viscosity, etc. But the results seem no difference in inlet and outlet parameters like pressure, temperature, enthalpy, entropy, etc. Thus leading to the same efficiency.

Does anybody know how to control the turbulence? Thanks above!
  Reply With Quote

Old   November 14, 2006, 11:22
Default Re: How to set and control the turbulence in CFX?
  #2
Bian
Guest
 
Posts: n/a
Interesting thing. By changing the parameters you mentioned, the efficiency should be different.

It seems your problem is not how to control turbulence, but what is the effect of turbulence.
  Reply With Quote

Old   November 14, 2006, 18:11
Default Re: How to set and control the turbulence in CFX?
  #3
Wei
Guest
 
Posts: n/a
Yes, the efficiency should be different. But the results remain same.

Once I set a big turbulence for intial guess, and I stoped some times to see the intermediate results. It seems that the effeciency is increasing. After many iterations, the results converge to same one.

As I check, the turbulence parameters are different in the domain, but the inlet and outlet P, T, H, S remain same. This cause the same efficiency.
  Reply With Quote

Old   November 15, 2006, 14:12
Default Re: How to set and control the turbulence in CFX?
  #4
Bian
Guest
 
Posts: n/a
If the flow quickly went to fully turbulent after inlet boudary, setting different turbulence level at inlet might have very less effect.

  Reply With Quote

Old   November 15, 2006, 23:24
Default Re: How to set and control the turbulence in CFX?
  #5
Wei
Guest
 
Posts: n/a
But I always get a efficiency above 95%. It seems a little bit high. When I put the same condition in TASCflow, the entropy producing is higher, and the efficiency is around 90%. I think the difference of efficiency is too large. Do you know the difference between these two solvers?
  Reply With Quote

Old   November 16, 2006, 12:02
Default Re: How to set and control the turbulence in CFX?
  #6
Bian
Guest
 
Posts: n/a
Check out if the post-processing calculation is correct?
  Reply With Quote

Old   November 24, 2006, 03:09
Default Re: How to set and control the turbulence in CFX?
  #7
Wei
Guest
 
Posts: n/a
I checked that the post-processing is correct. After that I tested many times for changing the control parameters in Tascflow. And I found that the "Physical Advection Correction" item influence the efficiency for 5%. But I cannot find this parameter in CFX. Do you have any idea about this parameter in CFX?

Here is the discription of the parameter in TASCflow.

Name LPAC Default false Description Logical, selects PAC (Physical Advection Correction) terms in all transport equations except those for k and ". Also when the multi-component fluid (MCF) model is in use, an independent parameter LPAC_MCF controls PAC terms for mass fraction scalars and energy. When included, the PAC terms can provide a dramatic improvement in accuracy if there are strong streamwise gradients in the solution. For instance, total pressure conservation is poor without PAC terms in variable area ducts. PAC terms can slow down convergence but the increased accuracy usually makes the extra effort worthwhile. A value of true is recommended. For problems where conservation of total pressure is important, PAC discretization is essential.
  Reply With Quote

Old   November 24, 2006, 10:28
Default Re: How to set and control the turbulence in CFX?
  #8
Robin
Guest
 
Posts: n/a
The Physical Advection Correction term is roughly equivalent to the Numerical Advection Correction (NAC) term in CFX. These are the second order corrections to the advection term. While there is no exact equivalent to the PAC terms in TASCflow, the UDS + NAC scheme is regarded as more accurate.

This is on by default in every CFX run. The High Resolution scheme automatically limits the second order NAC term to keep the solution bounded. TASCflow has no equivalent to the High Res scheme, but using the Specified Blend Factor in CFX can yield similar results. Just be careful when specifying the blend factor as it can result in too much numerical diffusion, if too low (blend factor = 0 is first order) or numerical dispersion if too high (blend factor of 1 is second order, unbounded).

Are you using the same mesh, boundary conditions and material properties in both CFX and TASCflow? If you are and you compare the results of running upwind in both codes, the solution should be identical.

Looking back at your original post, I suggest looking at the eddy viscosity in a plane normal to your inlet (or the circumferential average on the meridional plane). If the solution is not responding to your inlet turbulence level, it could be because your inlet velocity profile cannot support the necessary production and your turbulence is dying off rapidly away from the inlet. Adding an appropriate boundary profile (velocity or total pressure) and/or adjusting the eddy length scale can often help.

Regards, Robin
  Reply With Quote

Old   November 28, 2006, 05:41
Default Re: How to set and control the turbulence in CFX?
  #9
Wei
Guest
 
Posts: n/a
Thanks very much for your patient explanation. I got a brief idea from your illustration.

As I said, I have already used same model and condition in CFX and Tascflow. When using UDS+PAC in Tascflow, the result is almost same with CFX. Otherwise, the efficiency is 5% lower without PAC term.

But my senior prefer to believe that the efficiency is 90% instead of 95%. He think 95% is too high for one stage of steam turbine. It seems that he do not believe CFX because CFX10.0 occured error when dealing with steam condition. This bug has already been confirmed by CFX support.

Do you have any idea about steam turbine? If you have time, please mail me so that we can talk about this further. My e-mail: shiweiwinson@gmail.com Thank you very much!
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
CFX convergence problem simulating ogive-cylinders at varied angle of attack jdacosta CFX 6 February 25, 2015 22:42
[ICEM] How to set bocos on 2D model for ANSYS CFX (tuts no help) RossFS ANSYS Meshing & Geometry 4 May 22, 2012 08:56
How to show the transient case? H.P.LIU Phoenics 7 July 13, 2010 04:31
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
How to set the transitional turbulence for blades Hermann CFX 3 January 5, 2006 15:06


All times are GMT -4. The time now is 02:46.