ill-posed CFD problem ?

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

 March 27, 2007, 06:40 ill-posed CFD problem ? #1 Noel Guest   Posts: n/a Sponsored Links Dear all, I have a basic CFD problem of an incompressible steady state fluid flow. A domain is given where the area of the inflow equals the area of the outflow (Ain = Aout). Then I set these following two boundary conditions : 1. The pressure at the inflow (Pin) and at outflow (Pout) are fixed. 2. The inflow velocity (Vin) and outflow velocity (Vout) are the same (Vin = Vout). I don't fix the value, I just want the convergent velocity will give me the condition Vin = Vout. Is this problem feasible to solve ? Algebraically speaking, we have some available equations : 1. momentum equation 2. continuity equation 3. Pin = fixed 4. Pout = fixed 5. Vin = Vout Is this sufficiently specified or overspecified ?

 March 27, 2007, 11:35 Re: ill-posed CFD problem ? #2 sidd Guest   Posts: n/a If In-Out pressures are same, why would there be any flow?

 March 27, 2007, 14:56 Re: ill-posed CFD problem ? #3 Paolo Lampitella Guest   Posts: n/a The only case i know in which these conditions apply is the Poiseuille flow, a self-similar laminar steady incompressible flow in a rectilinear circular pipe. In this case you have a velocity profile which has the same shape all along the tube (a parabolic profile) and whose maximum depends by only two parameters: Re number and (Pout-Pin)=dP. This is the analytical case. If you are making an incompressible numerical simulation it's all different. At the inlet you have to specify a velocity profile not just a value of velocity. At the outlet you can't specify any kind of value for the velocity and about it's profile but you can specify the pressure (if you want) and an outflow condition (you must). In this case the pressure jump is implicitly defined by the velocity at inlet. Otherwise you can implicitly assume that the assial variation of pressure is linear and assigning the pressure at inlet and outlet it drops out of the x momentum equation as unknown and this simplify the outflow condition on velocity.

 March 28, 2007, 05:57 Re: ill-posed CFD problem ? #4 George Guest   Posts: n/a The inlet and outlet pressure are not the same, but are fixed.

 March 28, 2007, 06:54 Re: ill-posed CFD problem ? #5 TITAN Algorithms Guest   Posts: n/a The image below is from the TFS tutorial as follows: http://www.titanalgorithms.com/tutor..._bc/index.html http://www.titanalgorithms.com/tutor...nsbasicsb1.PNG Your problem has specified pressure Dirichlet BC so the conjugate velocity BC is a Neumann type. That is, you must specify the gradient in velocity at the inflow and outflow faces. Last edited by wyldckat; March 9, 2014 at 17:20. Reason: removed direct images that were showing publicity, as the site is now dead

 March 28, 2007, 09:07 Re: ill-posed CFD problem ? #6 Noel Guest   Posts: n/a Hi Titan, thank's for the example. But I think the second case (fixed velocity at inlets and fixed pressure at outlets) is somewhat different from my problem. You have pressure fixed at outlet only, whilst in my problem the pressure is fixed at both inlet and outlet. Anyway, after seeing your examples, now I have question : Must we provide information of velocity at the inlet and the outlet ? - Your 1st example : Vin = fixed; Vout = fixed - Your 2nd example : Vin = fixed; grad(Vout) = fixed - My problem : Vin = Vout, but not fixed. So I only have one information at the boundary, while at your both problems two information are defined

 March 28, 2007, 10:18 Re: ill-posed CFD problem ? #8 Noel Guest   Posts: n/a Thank's, Paolo. Indeed this is not a typical CFD problem. I am dealing with a micro scale problem that requires me to impose Vin = Vout. It seems, from your explanation (correct me if I'm wrong), that my problem is underspecified as it doesn't specify the inlet velocity profile. I myself suspect that my problem is overspecified. It comes from a very simple problem in the following : I want to solve a fluid flow by using a staggered grid in 1D domain. Suppose I use a single horizontal line as my 1D domain. I divide the line into 2 cells (cell-1 and cell-2), therefore with staggered grid I will have 2 cell centers (X1 and X2) and 3 face points (Xin, Xmid, and Xout). Geometrically : x1 is lying between xin and xmid; x2 is lying between xmid and xout. As before, my boundary conditions are : 1. fixed pressure at the inlet and outlet; 2. inlet velocity equals the outlet velocity (not fixed). Since I only have 2 cells, the first boundary condition will give me : P1 = pressure at X1 = fixed ; P2 = pressure at X2 = fixed. Now it remains to solve the velocity at all faces (Vin, Vmid, Vout). So we have 3 unknowns. On the other hand, I have 4 equations to satisfy : 1. Vin = Vout (2nd boundary condition) 2. Momentum equation at point Xmid 3. Continuty equation at cell-1 4. Continuty equation at cell-2 There are 4 equations for 3 unknowns, so it is overspecified and cannot be solved. But I am afraid I make mistakes in defining the equations. If my problem is underspecified or sufficiently dpecified, which equation should be wiped out ?

 March 28, 2007, 11:10 Re: ill-posed CFD problem ? #9 Ananda Himansu Guest   Posts: n/a Your problem is a well-posed steady-state problem if your governing equations have terms other than the inertial term to balance the pressure gradient. This has been explained in "TITAN Algorithms"' second post, but let me try to put it in different words. Because the flow is steady and because the cross-section area is unchanged between inlet and outlet and the flow is incompressible, the pressure difference cannot cause a fluid acceleration (either temporal or spatial) or fluid dilatation. Therefore, the pressure difference between inlet and outlet must be balanced by some opposing force, viscous or magnetohydrodynamic or such. The opposing force must be an increasing function of velocity, in order to reach a unique stable steady-state inlet/outlet velocity (effectively a unique mass flux). Incidentally, for the little two-cell discretization you examine, you cannot enforce continuity in both cells AND (equal) velocities at both inlet and outlet. Either you must replace one of the continuity equations with one of the inlet/outlet velocity dirichlet conditions (preferably the nearest one, to avoid major banding in the coeff matrix) or, more naturally, replace one of the dirichlet velocity bcs (preferably the one at the outlet, to yield a more natural downstream sweeping relaxation algorithm if need be) with the neighboring continuity equation. You are right that as laid out by you, the discretization is overspecified. If you include streamwise viscous terms or use central spatial differencing, and your solver therefore needs velocity bcs at both inlet and outlet, then as TITAN Algorithms mentions, you must specify a null gradient or null second-derivative (null streamwise diffusion) bc on the velocity at the outlet.

 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 ArslanOZCAN FLUENT 3 January 26, 2011 07:25 Vijay CFX 0 June 20, 2003 08:23 John C. Chien Main CFD Forum 54 April 23, 2001 08:10 John C. Chien Main CFD Forum 36 January 24, 2001 22:10 Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52