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

Rotating boundary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 14, 2007, 10:50
Default Rotating boundary
  #1
eros
Guest
 
Posts: n/a
Hello! I've to carry out a calculation in which a rotating boundary is present.The boundary moves into the fluid domain at a constant angular velocity.I set up an unsteady calculation in which boundary rotation around x axis is defined with a CEL like this:

omega = 890 [rad s^-1] alfa=omega * t sy = ((y*cos(alfa))-(z*sin(alfa)))-y sz = ((y*sin(alfa))-(z*cos(alfa)))-z

CFX solver gives me always the same error, that is: "A negative element volume has been detected..." Time step is very small (about 10^-5). I tried different meshes and different definitions for mesh stiffness but I obtained always the same result. Thank you for collaboration, bye!

  Reply With Quote

Old   May 14, 2007, 18:26
Default Re: Rotating boundary
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

1) If you are doing rotation then use the rotating frame of reference model rather than a general moving mesh.

2) If you use moving mesh through CEL to define your motions you might be limited in how far you can rotate. If you use specified displacement on the boundaries the default mesh smoothing algorithm for the interior nodes will definitely fail and cause negative volume elements. The way to fix this is to define a subdomain in the rotating region and specify the mesh motion in the entire subdomain. This means you have to describe the motion at all points by a CEL function which is not always possible.

3) To debug mesh motion simulations, use the expert parameters to turn the fluid, turbulence, heat and any other equations off and output a transient result file each iteration. This should run quickly as it has no flow variables to solve for. You can then view the progress of the mesh motion in CFX-Post and see exactly where the mesh is going wrong.

Glenn Horrocks
  Reply With Quote

Old   May 15, 2007, 03:21
Default Re: Rotating boundary
  #3
eros
Guest
 
Posts: n/a
Hi Glenn, thanks a lot for your response! You mean that I've to define a rotating subdomain?Actually rotating boundaries are closing an empty space, have I define a solid subdomain!? I'm not sure to have understood your hint. Thanks again, bye!
  Reply With Quote

Old   May 15, 2007, 18:33
Default Re: Rotating boundary
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Can you describe what you are modelling? Then I might be able to be more specific.

Glenn Horrocks
  Reply With Quote

Old   May 16, 2007, 04:02
Default Re: Rotating boundary
  #5
eros
Guest
 
Posts: n/a
I have to simulate the effect of the air on a crankweb profile. The crankweb rotates in a mixtur of air and oil. In practice it is a solid body on shaft which rotates into a fluid domain. How can I sent you some images to explain the problem in a better way?
  Reply With Quote

Old   May 16, 2007, 18:09
Default Re: Rotating boundary
  #6
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

I would have thought this was easily modelled using a rotating frame of reference. Put the crank in a RFR, the crank case in a stationary frame of reference and join the two with a GGI. Forget about the mesh motion, it will not work here.

Glenn Horrocks
  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
how to set rotating boundary? conan FLUENT 2 April 6, 2012 00:22
rotating wall boundary condition in multiphase sdp FLUENT 0 February 16, 2009 21:12
Boundary conditions for rotating fan rohit FLUENT 5 July 24, 2008 00:26
how to move a rotating boundary zyf FLUENT 1 December 3, 2007 02:49
Solver error message!!! IoSa CFX 1 September 14, 2006 04:48


All times are GMT -4. The time now is 00:13.