# Incorrect velocity behaviour near outflow boundary

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

 January 14, 2005, 08:16 Incorrect velocity behaviour near outflow boundary #1 Knut Erik Guest   Posts: n/a Hello. I have a problem with my 2D incompressible Navier-Stokes solver. I am using a vertex-centered Finite Volume method with triangular primary cells (Control Volume Finite Element) together with a pressure-correction algorithm and colocated variable arrangement. The Rhie & Chow method is implemented to avoid oscillations in pressure and velocity. The problem is this: When simulating flow in a rectangular channel with Poiseuille-profile (u = parabola, v = 0) at the inlet, the converged steady state solution is correct everywhere except near the outlet. Here, there is a disturbance in the velocity component normal to the flow direction (v in this case), and it is not zero as it should be. The Rhie & Chow interpolation is not used for boundary faces, because then another error appears. It seems to me that the problem is caused by the velocity corrections near the outflow boundary. Is there anyone who has experienced this and know the solution to the problem? Thanks, Knut Erik

 January 18, 2005, 11:56 Re: Incorrect velocity behaviour near outflow boun #2 Oscar Link Guest   Posts: n/a HI, What about the BC at the outlet, usually you implement a spounge layer. Oscar.

 January 19, 2005, 06:45 Re: Incorrect velocity behaviour near outflow boun #3 Knut Erik Guest   Posts: n/a The BC at the outlet is du/dn = dv/dn = 0, implemented by neglecting diffusive fluxes across boundary edges. The BC for pressure correction is dp'/dn = 0 everywhere, but the pressure is fixed in one node (p' = 0). It doesn't seem to matter where on the boundary this node is located. In each outer iteration, before the pressure correction equation is solved, the outlet normal velocities are corrected so that global mass conservation is satisfied for the solution domain. The Rhie & Chow interpolation is then used for velocities on the RHS of the pressure correction equation. The diagonal element of the momentum matrix needed in this interpolation is the same for u and v, except for boundary nodes. However, when interpolating velocities on boundary edges, the Rhie & Chow method is not used. In stead the velocities are interpolated linearly. If this is not done, an error appears for both u, v and p near the node where the pressure is fixed. I would like to know if Rhie & Chow near (outlet) boundaries requires special treatment with this algorithm. It seems to me that the pressure correction (and then velocity corrections) is over-estimated just inside the outlet.

 January 19, 2005, 07:52 Re: Incorrect velocity behaviour near outflow boun #4 andy Guest   Posts: n/a Pressure smoothing is a kludge which adds unphysical mass fluxes to prevent decoupling. If the unphysical mass flux is significant in size and you add it to only one of the pair of faces in the downstream direction for the cells next to the boundary you will distort the flow. A dramatic example is provided by swirling flow because of the strong (and non-linear) radial pressure gradient. For a swirling pipe flow it is not unusual to see the velocity change direction by more than 45 degrees for the cell next to the wall because of pressure smoothing. In the real world kludges are necessary and used in variety of places for real world CFD codes. If pressure smoothing is a problem for your flow (for many it is not) there are alternatives. It is not usual to have strong normal second derivatives in pressure where a zero gradient exit boundary condition is appropriate. Zero gradient for the pressure is not wise. Extrapolating the pressure or implementing the implicit equivalent is what is usually done. In order to see the physical correctness of this, consider how velocity and pressure vary in fully developed pipe flow.

 January 19, 2005, 07:57 Re: Incorrect velocity behaviour near outflow boun #5 Oscar Link Guest   Posts: n/a the Rhie & Chow interpolation does not require a special treatment at the outlet boundary. If your solution looks wrong at the outlet even for the stationary case, I think there must be a mistake in the code. Otherwise, implementing a numerical sponge layer you can transport waves through the domain without reflections at the outlet.

 January 19, 2005, 14:31 Re: Incorrect velocity behaviour near outflow boun #6 Tony Guest   Posts: n/a Andy is right about the pressure outlet BC. The zero gradient of pressure is not physical. Instead, you can simply set the pressure itself to be constant (say zero) along the outlet.

 January 21, 2005, 07:48 Re: Incorrect velocity behaviour near outflow boun #7 Knut Erik Guest   Posts: n/a Thank you for your explanation. Do you know of any litterature concerning the effects of pressure smoothing?

 January 24, 2005, 06:21 Re: Incorrect velocity behaviour near outflow boun #8 andy Guest   Posts: n/a I am not aware of a good one but it was a widely studied topic in the early/mid 80s as the incompressible flow community adopted curvilinear meshes and could no longer use staggered Cartesian velocity components. The most common problem is that many presentations dress it up as being in some way correct. The Rhie and Chow papers are not particularly clear and the presented pressure smoothing is a function of relaxation factor which is a poor feature and avoidable. The compressible flow community moved to curvilinear/unstructured grid earlier and developed pressure smoothing earlier in the 70s. They tended to be upfront about it being undesirable and developed various schemes to minimise the size of the terms. One or two of these papers might be useful to read. The earliest approach to tackling pressure/velocity decoupling was probably by the Los Alamos group in the late 60s but they smoothed on the velocity field rather than pressure.

 November 18, 2015, 03:17 #9 New Member   Matthew de Haast Join Date: Aug 2014 Location: Cape Town Posts: 7 Rep Power: 3 I am having the exact same issue with my code. Does anyone have an idea on what could be causing the issue?

 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 rsmartins CFX 9 September 12, 2015 06:32 murali CFX 5 August 3, 2012 08:56 Morten Andersen CFX 1 January 8, 2007 12:37 michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15 chong chee nan FLUENT 0 December 29, 2001 06:13

All times are GMT -4. The time now is 14:17.