# Creeping Flow in CFX

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 September 5, 2005, 09:20 Creeping Flow in CFX #1 Taner Baytekin Guest   Posts: n/a Sponsored Links 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.
 Sponsored Links

 September 5, 2005, 19:14 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

 September 6, 2005, 02:44 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

 September 6, 2005, 19:28 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

 September 7, 2005, 02:30 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

 September 7, 2005, 18:35 Re: Creeping Flow in CFX #6 Glenn Horrocks Guest   Posts: n/a Hi, Have you tried double precision? Glenn Horrocks

 September 8, 2005, 02:24 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post jeffwmb CFX 20 March 13, 2013 17:21 cfd_multiphyiscs CFX 2 March 10, 2010 14:43 AirS OpenFOAM 0 January 12, 2010 08:08 jan CFX 1 July 31, 2007 19:44 Axel Rohde Main CFD Forum 1 November 19, 2001 13:19

 Sponsored Links

All times are GMT -4. The time now is 10:26.

 Contact Us - CFD Online - Top