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?

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).

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?

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)

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?

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

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.

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?

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

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

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

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