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

time averaged results as initial conditions in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 2, 2007, 16:37
Default time averaged results as initial conditions in CFX
  #1
mike
Guest
 
Posts: n/a
Hi Everybody, I am using CFX 11 package. I have time averaged results of a case and I want to use this "time averaged results" as initial condition for my other run (same mesh). I tried couple of things but could not succeed. Any advice would be greatly appreciated. Thanks, Mike
  Reply With Quote

Old   May 2, 2007, 16:59
Default Re: time averaged results as initial conditions in
  #2
Robin
Guest
 
Posts: n/a
Hi Mike,

Open your results file in Post and replace the Velocity, Temperature and Pressure variables with expressions equating them to the time averaged equivalents (you can do this by selecting the appropriate variable under the Variables tab in Post and checking the box next to "Replace with expression").

Note that the original results are never lost, to recover them just go back to the variable and uncheck the "Replace with expression" box.

Interpolate the results of this modified results file onto new analysis.

Regards, Robin
  Reply With Quote

Old   May 3, 2007, 01:31
Default Re: time averaged results as initial conditions in
  #3
Dr. FLow Squad
Guest
 
Posts: n/a
I've always just use the interpolation function in the solver to have the steady state results as a start value. Is that wrong then?

Just ignore the Pre warning when saving a def file.
  Reply With Quote

Old   May 3, 2007, 08:15
Default Re: time averaged results as initial conditions in
  #4
mike
Guest
 
Posts: n/a
Hi Robin, Thank you very much. I did as you said, and it worked out great. Thanks again for you help. Mike
  Reply With Quote

Old   May 3, 2007, 08:19
Default Re: time averaged results as initial conditions in
  #5
mike
Guest
 
Posts: n/a
Dr Flow, To have steady state results as a start condition, you can do as you said. However in my case, I have time averaged results of transient run. and I want to use time averaged results as initial condition (not steady state solution). Mike
  Reply With Quote

Old   May 4, 2007, 17:14
Default Re: time averaged results as initial conditions in
  #6
Gert-Jan
Guest
 
Posts: n/a
Hi Mike,

I wonder what your application is. Why do you need time averaged results as an initial guess? Is it for a structural calculation?

Just trying to understand for what kind of application I could use this.......

Gert-Jan
  Reply With Quote

Old   May 5, 2007, 20:33
Default Re: time averaged results as initial conditions in
  #7
mike
Guest
 
Posts: n/a
Hi Gert-Jan, I have convergence problems mostly due to the transient effects. Thus, in order to get the best prediction, I run transient and take the time averaged of the field. That is good enough for our application. In addition, I wanted to get the temperature distribution (uncoupled with flow). So I shut the fluid and turbulence solvers off from expert parameters and just wanted to solve heat transfer equation.However I had to define velocity distribution for the domain. For the best prediction, I wanted to use the time averaged velocity field. Thats why I needed time averaged velocity field for initials conditions. Mike
  Reply With Quote

Old   May 7, 2007, 09:46
Default Re: time averaged results as initial conditions in
  #8
Robin
Guest
 
Posts: n/a
Hi Mike,

If that is the case, you should probably adjust the Eddy Viscosity to reflect the diffusion effect of turbulence. Otherwise you will combine the instantaneous turbulence field with the time averaged velocity field.

Interesting idea though.

Regards, Robin
  Reply With Quote

Old   May 7, 2007, 14:54
Default Re: time averaged results as initial conditions in
  #9
mike
Guest
 
Posts: n/a
Thanks Robin, I had never thought about it. I need to figure out something for this. Regards, Mike
  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
Floating point exception error Alan OpenFOAM Running, Solving & CFD 10 April 6, 2012 14:02
icoLagrangianFoam OF1.6 myNewParticleSolver heavy_user OpenFOAM 16 February 11, 2012 06:15
Forces in OF15 richard OpenFOAM Running, Solving & CFD 166 September 17, 2011 03:24
Velocity blows up suddenly after 30,000+ iterations lordvon OpenFOAM 14 October 27, 2010 11:13
Error while running rhoPisoFoam.. nileshjrane OpenFOAM Running, Solving & CFD 8 August 26, 2010 12:50


All times are GMT -4. The time now is 04:31.