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

domain definition of a impeller

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2009, 11:41
Default domain definition of a impeller
  #1
blazer75
Guest
 
Posts: n/a
hello,every one I want to simulate a impeller. I specified three domains. the domain round the impeller as rotating domain,the entrance part and the outlet part as stationary domain. there are two frozen rotor interfaces,which can connect this three domains.

but my teacher told me, that I can specify a complete rotating domain (from inlet to outlet), the stationary wall of the fluid channel as counter rotating wall specified. at this rate cfx can caculate without interface.

I want to ask, whether this two kind of domain setting are same?? can get the same result??

thanks very much for answer!!!
  Reply With Quote

Old   February 24, 2009, 11:56
Default Re: domain definition of a impeller
  #2
wayne
Guest
 
Posts: n/a
i don`t think it is right way,it is not just problem of boundary.it is of basic modeling.shortly saying .there is centrifugal force and coriolis force in so calling "rotating domain"

Regards

wayne
  Reply With Quote

Old   February 27, 2009, 02:54
Default Re: domain definition of a impeller
  #3
radionline
Guest
 
Posts: n/a
Why do you want to use Frozen rotor? Is it an transient problem?
  Reply With Quote

Old   February 27, 2009, 08:53
Default Re: domain definition of a impeller
  #4
CycLone
Guest
 
Posts: n/a
Hi Blazer,

What your professor suggested is correct. If your inlet and outlet parts are annular segments (i.e. no inlet vanes or diffuser vanes), then they can be included as part of the rotating frame and a counter-rotating wall can be applied to the hub and shroud.

If your mesh is coarse you may not get the same solution. When solving flow in a rotating frame of reference, the numerical diffusion will result in "false swirl", which is a tendancy for the flow to be driven in the rotating direction. You can see this effect if you model a straight pipe in a rotating frame with counter rotating walls, which should be equivalent to flow moving through a stationary pipe. In the stationary frame the flow will begin to swirl as it moves through the pipe.

Using the Alternate Rotationg Model will reduce this swirl (it is on by default if you use the turbo set-up mode), but refining mesh will also help.

So what university are you at?

-CycLone
  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
OpenFOAM static build on Cray XT5 asaijo OpenFOAM Installation 9 April 6, 2011 12:21
CFX domain comparison Kiat110616 CFX 4 April 3, 2011 22:43
Domain Imbalance HMR CFX 3 March 6, 2011 20:10
Material definition of a porous domain Hitch8 CFX 0 May 3, 2010 05:00
CFX Solver Memory Error mike CFX 1 March 19, 2008 08:22


All times are GMT -4. The time now is 04:08.