prevent secondary flow

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

 June 2, 2004, 03:40 prevent secondary flow #1 Machteld Guest   Posts: n/a I am trying to simulate a laminar flow in a pipe with a no slip condition. Somehow CFX develops secondary flow in its results. Does anyone know how to prevent this?

 June 2, 2004, 08:17 Re: prevent secondary flow #2 Bart Prast Guest   Posts: n/a Could be caused by your outlet boundary condition: opening or outlet. If it's a straight pipe extending your domain will not do a lot for you. By the way: is it a straight pipe? Other wise your secondary flow could be physical (in real).

 June 2, 2004, 08:30 Re: prevent secondary flow #3 Machteld Guest   Posts: n/a Thanks for helping me. It is indeed a straight pipe, so I do not expect secondary flow (low Reynolds number, so it should be laminar). My outlet boundary condition is an outlet with a relative pressure (static pressure) of 0. Could it help to use an opening? What would be the essential difference?

 June 2, 2004, 08:38 Re: prevent secondary flow #4 Bart Prast Guest   Posts: n/a Outlet boundary prevents inflow from the back (on those cell interfaces the geometry is effectively closed). An opening does allow for back flow (do not use this for compressible flows). Other issues might be: 1. poor grid (not likely in a straight pipe but do try a finer mesh to check influence 2. no convergence yet (do not look at intermediate solutions). What is your convergence now? 3. any difference between upwind results and 2nd order? 4. Whats your inlet condition (imposed velocity profile; do check the interpolation on your mesh)

 June 2, 2004, 09:16 Re: prevent secondary flow #5 Machteld Guest   Posts: n/a 1) I already tried mesh refinement. It does influence it a little but not significantly. 2) It is fully converged. The residual target is 1e-5 (RMS). (Unfortunately I cannot check if changing this to 1e-6 improves my solution due to licence problems this week) 3) Upwind, the secondary flow is much less than at the outlet. What do you mean by second order? 4) my imposed velocity profile is a Poiseuille flow: 2*Vx*(1-r^2/R^2) If the average velocity in the pipe is about 1 m/s, what order of error can I expect? dV=1e-3 or should it be better?

 June 2, 2004, 09:59 Re: prevent secondary flow #6 pi Guest   Posts: n/a Hi there, if relative pressure in the outlet is zero, I assume that there is no pressure drop along the pipe. am I right? -If yes I can't see any force to drive the motion and there is no other stationary (because I guess you are searching stationary and the pipe is horizontal) solution but u=0 everywhere -If no, for incompresible flow it is impossible the flow develops secondary flow for low Re. In this case why you don't solve directly the resulting ODE? for sure it is faster and cheaper than simulate it and try to find where the bug is. hope don't make more confussion pi

 June 2, 2004, 10:20 Re: prevent secondary flow #7 Gloria Gaynor Guest   Posts: n/a Hi pi, if the relative pressure in the outlet (P_outlet) is zero, then the pressure drop along the pipe is: dP = P_inlet - P_outlet = P_inlet Cheers, G. G.

 June 2, 2004, 11:16 Re: prevent secondary flow #8 Bart Prast Guest   Posts: n/a Machteld My guess is that the convergence criteria is not enough. I suppose you're solving with the high resolution schema. You can do it fully second order (blend factor =1). But it shouldn't really matter in your case. Do check whether the velocity profile you impose at the inlet is properly interpolated by CFX. How does the velocity profile look like after a few (1-2) iterations? Is it still symmetrical?

 June 2, 2004, 14:08 Re: prevent secondary flow #9 Juan Carlos Guest   Posts: n/a Dear Matchteld, Secondary flows could be generated by a mesh that is not a good representation of the geometry. For example, for a straight pipe your wall surface mesh must have all faces parallel to the main axis; otherwise, the flow is diverted creating a secondary flow downstream. Imagine flow on a badly beaten up pipe. Also, the parabolic velocity profile you are imposing is an analytical solution that can only be obtained for an infinitely refined mesh. For a more human mesh, the discretization error will affect the parabolic profile a bit; however, this bit will be seeing as secondary flow until the flow is numerically fully developed at the outlet for a given mesh. This is similar to Bart's point of view. Good luck, Juan Carlos

 June 2, 2004, 18:15 Re: prevent secondary flow #10 Glenn Horrocks Guest   Posts: n/a Hi Machteld, In regard to your comment about accuracy: In laminar flow you should be able to get essentially the exact answer. As long as the simulation has been set up correctly and accurately you should be able to get errors as small as your patience is long. Very accurate simulations take a long time! Glenn

 June 3, 2004, 06:40 Re: prevent secondary flow #11 Rui Guest   Posts: n/a Hi, For a straight pipe, try to use a structured hex mesh, with thinner elements close to the wall. You may build it with the Patran tool. I'm quite sure this will help, as an unstructured tet mesh is probably the cause of the secondary flow . And if there is angular symmetry, you may also simulate just a "slice" of the pipe. I also think that a tighter convergence shouldn't be difficult to obtain for this kind of flow conditions. Rui

 June 9, 2004, 15:43 Re: prevent secondary flow #12 Bob Guest   Posts: n/a Try simplifying the problem. Remove the imposed profile from the setup, do you still get secondary flow ? It may help you narrow down the cause of the problem. If its not the inlet profile then it may well be boundary conditon setup at the outlet. What is your fluid setup ? Isothermal ? Bob

 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 kevin FLUENT 8 August 11, 2015 13:00 seaharrier CFX 1 May 18, 2010 07:45 Tajnesaie CFX 2 January 21, 2010 03:00 Miri FLUENT 0 June 7, 2006 05:56 diaw Main CFD Forum 104 February 16, 2006 06:44

All times are GMT -4. The time now is 00:08.