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

Transist calculation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 29, 2002, 04:27
Default Transist calculation
  #1
DANDY
Guest
 
Posts: n/a
Hi everyone:

Can you help me on transisit calcultation using CFX-TASCflow. The problem is about a twin stage low speed axial compressor. I use Rotor/Strator as interactions instead of Stage when transisit clcultation starting. I did it as the help document said. But I couldn't get a convergence result. The monitor show that a wall placed on outlet as 20%.... .Whatever the DTIME be selected as. The wall still on. What can I do??
  Reply With Quote

Old   May 29, 2002, 08:06
Default Re: Transist calculation
  #2
cfd guy
Guest
 
Posts: n/a
Hi DANDY,
I will be no help for your convergence problem but regarding these walls I can tell you that is possible to avoid it. These walls prevents the fluid to enter in the domain through an OUTLET boundary condition. If you set IO_WALLS = f in your PRM file, TASCflow will not create these walls and you'll have some backflow on that BC. Have you tried an OPENING BC instead of an OUTLET one?
Regards, cfd guy
  Reply With Quote

Old   May 29, 2002, 20:16
Default Re: Transist calculation
  #3
DANDY
Guest
 
Posts: n/a
Thanks CFD guy I really appreciate your help. I'll try it as you said. By the way, if I did so, then the result maybe have some backflow on BC? But you know, the problem I was working have no backflow yet. Does it right? And, an Opening BC instead of OUTlet can do what for solving the problem. Hoping you answer again. Thanks
  Reply With Quote

Old   May 30, 2002, 17:01
Default Re: Transist calculation
  #4
Robin
Guest
 
Posts: n/a
Dandy,

When running a transient simulation, you should not expect the solution to converge. A transient rotor/stator analysis will always show residuals because there is no steady state solution.

The problem at your outlet may be the result of many things. Did you start with a converged frozen rotor solution? This will help, since you must initially run the transient solution until the startup transient has passed. Also, if the outlet is placed too close to the trailing edge of your last component, the wake may not have time to mix out before hitting the outlet, thus causing the wall off. If this is the case, move your outlet farther away to place it in a more predictable flow location.

Do not allow the outlet wall off to persist, this will adversely affect your solution. Changing it to an opening will only make the warning go away, you will still not get the right solution if this is the outlet of your stage calculation!

Finally, your timestep for a transient rotor/stator simulation should be at least 1/10 of the time it takes for one pitch change.

Robin
  Reply With Quote

Old   May 30, 2002, 21:43
Default Re: Transist calculation
  #5
DANDY
Guest
 
Posts: n/a
Robin: Thanks for your help. I want to discuss the problem with you for details. 1.The timestep for transist simulation was about 1/30 of the time it takes for one pitch change. And I started the simulation from a converged steady-state solutation. As you said, the converged frozen rotor had been my choosen sometime ago. But I found it didn't help for the simulation. Maybe it not a good initial soluation for transist problem of axial component, because the middle result shown that the over all efficiency was far from the reality. Finally, I choose the steady-steate as the initial soluation. 2.The outlet is placed about a chord to the trailing edge of last component. Does it enough? 3.Discretization is Modified Linear Profile. 4.Some other CFD software can define CFL number for the inner timestep(virtual timestep) when running a transist simulation, but it seems that CFX-TASCflow couldn't control it.The only thing I could do is to define the Dtime, and it determine the outer timestep (physiscal timestep). When the Dtime was reduced enough (such as 1/1000 of the time it takes for one pitch change), the CFL number shown in the beginning of the transist simulation may be less than 1. Sometimes I thought if that the converge problem maybe arose from the CFL number? 5. For two months, I was working on it. 1/30,1/300 the time it takes for one pitch change as the transist simulation timestep had been attempted. And the Grid scale(per component) also be changed from 10,000 to 80,000. Unfortunately, it still cann't get an acceptable result.

  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
MRF and Heat transfer calculation Susan YU FLUENT 0 June 2, 2010 08:46
Defining output as input for second calculation mannobot FLUENT 1 June 2, 2010 04:20
Transfer output data as input for second calculation mannobot Main CFD Forum 1 June 2, 2010 03:55
Warning 097- AB CD-adapco 6 November 15, 2004 05:41
Heat Flux Calculation under REPORTS Alberto Schroth FLUENT 0 May 16, 2000 08:19


All times are GMT -4. The time now is 11:32.