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

Creeping Flow in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 5, 2005, 09:20
Default Creeping Flow in CFX
  #1
Taner Baytekin
Guest
 
Posts: n/a
Hello everybody,

I'm simulating the fluid dynamics of steady lubricant flow, which is basically creeping flow governed by the Stokes equations (Re<<1).

Is it possible to take the advantage of creeping flow in CFX? In other words, can one cancel some terms in Navier-Stokes equations for a specific simulations? e.g. the convective term.

I appreciate any advice/comment on the subject.

Best regards.
  Reply With Quote

Old   September 5, 2005, 19:14
Default Re: Creeping Flow in CFX
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

I don't think it is possible to turn the convective terms off. I also suspect you won't have to. For very low Reynolds number flows the simulation should converge very rapidly as the lack of convection makes convergence very easy and fast. Just run it with the convective terms on as normal and it should converge very quickly.

Glenn Horrocks
  Reply With Quote

Old   September 6, 2005, 02:44
Default Re: Creeping Flow in CFX
  #3
Taner Baytekin
Guest
 
Posts: n/a
Hi Glenn,

Thanks for your comments.

Before I go for the simulations, I also thought as you do: steady creeping flow, no problem, this would converge very rapidly; but it does not. In fact the problem is the ratio of characteristic lengths in respective coordinate directions; e.g. for a journal bearing the ratio of clearance(film thickness) to bearing radius is in the order of 10^-3, i.e. either finite volumes with enormous aspect ratio (poor quality), or models which consists of quite a few million cells (good quality).

The number of outer iterations required for convergence is about 150, which I find ridiculous, if I employ a good quality mesh (4.5*10^6 cells),this amount to a huge computational time. The idea was to simplify the Navier Stokes equations in order to have a converged solution after just a few iterations.

Wish you all a rapid convergence.

Taner Baytekin

  Reply With Quote

Old   September 6, 2005, 19:28
Default Re: Creeping Flow in CFX
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Are you using CFX4 or CFX5/10? 150 iterations per timestep is not unheard of in CFX4, but CFX5 should have only around 5.

The difference in lengths should be OK in either code. A tet/prism mesh in CFX5 will not work well as you say, but a structured (hex) mesh should work well as the flow is aligned with the grid and this greatly mitigates the disadvantages of high aspect ratio elements.

Glenn Horrocks
  Reply With Quote

Old   September 7, 2005, 02:30
Default Re: Creeping Flow in CFX
  #5
Taner Baytekin
Guest
 
Posts: n/a
Hi,

I'm using CFX5, the grid should be OK, it is structured hexas and consists of only one block.

Another observation is the following: if the aspect ratio of an average hexa is extremely high, about 1:80, then the simulation does not converge, the residuals fluctuates around a constant mean value with rather small amplitudes.

Taner Baytekin

  Reply With Quote

Old   September 7, 2005, 18:35
Default Re: Creeping Flow in CFX
  #6
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Have you tried double precision?

Glenn Horrocks
  Reply With Quote

Old   September 8, 2005, 02:24
Default Re: Creeping Flow in CFX
  #7
Taner Baytekin
Guest
 
Posts: n/a
Hi Glenn,

I usually use double precision.

The problem is now better, I tried the following: I interpolated a coarse grid solution for the initialisation, then the convergenge criteria is fulfilled within 25 outer iterations, I can live with it.

Thanks a lot for your comments.

Taner Baytekin

  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
[HELP] Slip flow boundary condtion in CFX jeffwmb CFX 20 March 13, 2013 17:21
Ansys 11.0 CFX - solving electric potentials and multiphase flow cfd_multiphyiscs CFX 2 March 10, 2010 14:43
Different flow pattern between OpenFOAM and CFX AirS OpenFOAM 0 January 12, 2010 08:08
demo free flow blunt body in cfx ansys 11 jan CFX 1 July 31, 2007 19:44
Inviscid Drag at subsonic, subcritical Mach # Axel Rohde Main CFD Forum 1 November 19, 2001 13:19


All times are GMT -4. The time now is 22:08.