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

How to achieve the forced transition in CFX?

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   July 4, 2012, 08:57
Default How to achieve the forced transition in CFX?
  #1
New Member
 
Fukun Zhang
Join Date: Jul 2012
Posts: 3
Rep Power: 6
seraphzfk is on a distinguished road
How to achieve the forced transition in CFX?
I want to simulate Vortical Flow of wing ,and achieve the forced transition in the wing location where I just set. In the CFX how to achieve the forced transition in CFX?
seraphzfk is offline   Reply With Quote

Old   July 4, 2012, 23:24
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,542
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Do you mean laminar to turbulent flow transition?
ghorrocks is offline   Reply With Quote

Old   July 5, 2012, 01:07
Default
  #3
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,470
Rep Power: 25
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Apart from grid-induced separation in a Detatched Eddy Simulation (which is rather a modeling error) i can't think of of a "pre-built" solution for this purpose in CFX.
flotus1 is offline   Reply With Quote

Old   July 5, 2012, 01:35
Default Transition
  #4
New Member
 
Fukun Zhang
Join Date: Jul 2012
Posts: 3
Rep Power: 6
seraphzfk is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Do you mean laminar to turbulent flow transition?
We all konw that in the laminar flow the separation is earlier than in the turblence flow. Indeed the turblence separation is promoted more area than the laminar.
In my study,my problem is that the separation is promoted earlier, and I think the laminar flow has an efficient effect on my study. Because the experient results show that the separation should occur downstream.
So I would like to set the boundary between laminar and turblence , I called it forced transition. Could I achieve it?
seraphzfk is offline   Reply With Quote

Old   July 5, 2012, 03:09
Default
  #5
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,329
Blog Entries: 6
Rep Power: 45
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
Originally Posted by seraphzfk View Post
We all konw that in the laminar flow the separation is earlier than in the turblence flow. Indeed the turblence separation is promoted more area than the laminar.
In my study,my problem is that the separation is promoted earlier, and I think the laminar flow has an efficient effect on my study. Because the experient results show that the separation should occur downstream.
So I would like to set the boundary between laminar and turblence , I called it forced transition. Could I achieve it?
Your question is not clear.

1. We all know that laminar flow is more prone to separation than turbulent flow.

2. Separation is not a good effect. What type of geometry you are modelling?

3. It is known fact that, all RANS model assume the fully turbulent flow unless the separate equations are solved for the transition mechanism. One such example is gamma theta transition model, which does not model the transition physics, rather it uses the correlation to properly model the different type of transitions such as bypass, natural and separation induce transition. http://www.cfd-online.com/Forums/flu...ent-flows.html

4. LES and DNS are the methods which solve the transition in real sense.

5. There is a trip term in SA model http://turbmodels.larc.nasa.gov/spalart.htmlwhich forces the transition from laminar to turbulent at prescribed location. But this term is abandoned in commercial codes. http://courses.washington.edu/mengr5...our-report.pdf

So if you still do not want to use the transition model and/or LES/DNS then you can make two fluids. For one use the laminar model and for other use the turbulence model. I used this in Fluent http://hpce.iitm.ac.in/website/Manua...ug/node267.htm and I believe there should be no difficulty using this combination in CFX as well. http://www.cfd-online.com/Forums/flu...same-time.html https://www.sharcnet.ca/Software/Flu...e231.htm#36737
This should work for CFX http://www.kxcad.net/ansys/ansys_cfx.../i1324236.html

http://www.dept.aoe.vt.edu/~cjroy/Jo...icles/jsr1.pdf

one of the old post: http://www.cfd-online.com/Forums/cfx...turbulent.html
Far is offline   Reply With Quote

Old   July 5, 2012, 06:03
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,542
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes. The turbulence transition model in CFX has an option where you can specify which regions of the flow are turbulent and which are laminar. You can use this to specify the lam-turb transition point. This has been used to model things like turbulence trip wires and similar things.
Far likes this.
ghorrocks is offline   Reply With Quote

Old   July 5, 2012, 06:11
Default
  #7
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,329
Blog Entries: 6
Rep Power: 45
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
This is the quote from one of the above references: http://www.kxcad.net/ansys/ansys_cfx.../i1324236.html


Quote:
For the zero equation transition model, the best way to specify the intermittency is with a user defined subroutine that is based on the x, y and z coordinates. This way, if else statements can be used to define geometric bounds where the intermittency can be specified as zero (laminar flow) or one (turbulent flow). This method can be used to prescribe laminar zones at the leading edges of the wings, for example. A CCL example for the zero equation model is shown below where the user function TRANSITION TRIP(x,y,z) returns either a 0 or a 1 based on the geometric location:

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
Far is offline   Reply With Quote

Old   July 8, 2012, 21:07
Default
  #8
New Member
 
Fukun Zhang
Join Date: Jul 2012
Posts: 3
Rep Power: 6
seraphzfk is on a distinguished road
Quote:
Originally Posted by Far View Post
Your question is not clear.

1. We all know that laminar flow is more prone to separation than turbulent flow.

2. Separation is not a good effect. What type of geometry you are modelling?

3. It is known fact that, all RANS model assume the fully turbulent flow unless the separate equations are solved for the transition mechanism. One such example is gamma theta transition model, which does not model the transition physics, rather it uses the correlation to properly model the different type of transitions such as bypass, natural and separation induce transition. http://www.cfd-online.com/Forums/flu...ent-flows.html

4. LES and DNS are the methods which solve the transition in real sense.

5. There is a trip term in SA model http://turbmodels.larc.nasa.gov/spalart.htmlwhich forces the transition from laminar to turbulent at prescribed location. But this term is abandoned in commercial codes. http://courses.washington.edu/mengr5...our-report.pdf

So if you still do not want to use the transition model and/or LES/DNS then you can make two fluids. For one use the laminar model and for other use the turbulence model. I used this in Fluent http://hpce.iitm.ac.in/website/Manua...ug/node267.htm and I believe there should be no difficulty using this combination in CFX as well. http://www.cfd-online.com/Forums/flu...same-time.html https://www.sharcnet.ca/Software/Flu...e231.htm#36737
This should work for CFX http://www.kxcad.net/ansys/ansys_cfx.../i1324236.html

http://www.dept.aoe.vt.edu/~cjroy/Jo...icles/jsr1.pdf

one of the old post: http://www.cfd-online.com/Forums/cfx...turbulent.html
Thank you very very much! My English is poor, and I had barely written the question in English.
Your suggestion is a great favor for me. Thank you!
Now I am simulating the delta_wing based on VFE-2 geometry. When I calculate delta_wing in the condition of medium leading_edge (round leading_edge ) and in the Ma=0.4, Re=3 Million , angle of attack 13 degree, my calculation did not fit the experiment data very well. I found that in my study the onset of the main primary separation was in more upstream position compared with the experimental separation point.
Result:
http://www.imageuploading.com/ims/pi...2z5nL&i=137831

Last edited by seraphzfk; July 8, 2012 at 22:00.
seraphzfk is offline   Reply With Quote

Old   July 9, 2012, 05:31
Default
  #9
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,329
Blog Entries: 6
Rep Power: 45
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
I
Quote:
found that in my study the onset of the main primary separation was in more upstream position compared with the experimental separation point.
Why? In plot station 1 corresponds to leading edge?
Far is offline   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
Trans. SST Intermittency Factor and Viscosity Ratio eishinsnsayshin FLUENT 3 May 23, 2012 03:02
need help on defining boundary conditions for forced transition LSC CFX 7 June 15, 2009 07:01
Code release: Flow Transition and Turbulence Chaoqun Liu Main CFD Forum 0 September 26, 2008 17:15
Coupled vs Seg - Natural vs. Forced Convection Alex CD-adapco 5 December 12, 2007 05:58
forced transition dirk steudel CD-adapco 5 July 11, 2000 03:17


All times are GMT -4. The time now is 19:09.