illposed CFD problem ?
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 ? 
Re: illposed CFD problem ?
If InOut pressures are same, why would there be any flow?

Re: illposed CFD problem ?
The only case i know in which these conditions apply is the Poiseuille flow, a selfsimilar 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 (PoutPin)=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. 
Re: illposed CFD problem ?
The inlet and outlet pressure are not the same, but are fixed.

Re: illposed CFD problem ?
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. 
Re: illposed CFD problem ?
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 
Re: illposed CFD problem ?
Noel
Yes you are correct. This example is different. I didn't have an exact simulation to compare to, hence this example was shown. However, in your simulation, the Neumman gradients are zero on both faces. Generally the approach which can be committed to code reads: GRAD(V*en) = [0,0,0] where en = ex for your x directed face. This is simplified as u,x = 0 on inlet, but this assumes the v, and w components are zero. However, for fully developed flow, these will be zero at the inlet and outlet. You say Vin = Vout. Yes this is true, but you cannot specify what this V is. This is only achieved by the Neumann BC and the satisfaction of the continuity equation. You are fixing a gradient on the problem. So as you start your simulation, the flow will locomote across the faces. The middle of the duct will be stagnant until it adjusts from the pressure source. In the end, the pressure gradient will balance viscous diffusion, the advection terms go to 0 and you are left with a fully developed flow. Point to mention: The pressure gradient that you impose by the selection of Pin and Pout must be realistic with respect to the final velocity profile. That is, if you select a GRAD(P) = (P.OT  P.IN)/L.duct which does not satsify the diffusion term mu u,yy then the flow will not converge and will continue to ratchet up until GPF. The missing terms are turbulent contributions. This can be demonstrated in most codes. Solution, activate turbulence in this case. regards 
Re: illposed CFD problem ?
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 (cell1 and cell2), 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 cell1 4. Continuty equation at cell2 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 ? 
Re: illposed CFD problem ?
Your problem is a wellposed steadystate 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 crosssection 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 steadystate inlet/outlet velocity (effectively a unique mass flux). Incidentally, for the little twocell 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 secondderivative (null streamwise diffusion) bc on the velocity at the outlet. 
Re: illposed CFD problem ?
No, what i'm saying is the opposite.
The problem, as defined by you, has a solution in the laminar case and maybe (but i'm not sure because it's not my field) this can be extended to the microscale; that is, the scales involved are so small (but not as much as the molecular ones) that the viscosity is the predominant effect so the flow is laminar. In this case the solution for the steady incompressible flow in a straight pipe with costant circular cross section exists and is that of Poiseuille (other costant cross sections also admits analytical solutions). In this case, after you have defined the radius of the pipe (R) and the viscosity of the fluid (v), just one parameter defines the solution, that is the jump of pressure between the inlet and outlet. The final solution is: U (r) = [ (Pin  Pout) / (4 L v) ] ( R^2  r^2 ) in which r is the radial coordinate, L is the pipe lenght and U(r) is the velocity in the axial direction, the only one different from 0. As you can see the solution is indipendent of x (and t of course) and the parabolic velocity profile is in a manner a consequence of this condition prelimarly imposed. In this sense your problem is similar (if not the same): in a steady incompressible viscous flow the pressure gradient acts like a source term and the costant velocity comes out from taking it as indipendent of x and the parabolic profile emerges from the solution as the only one possible so you don't have to assign it. What i said is that, when these conditions apply, the solution is one and is that of Poiseuille. This kind of solutions imply that the flow in the pipe is unaffected by the inlet and outlet conditions (except for the pressure which instantaneously propagates) and that the Re number is low so the flow is also stable and so the velocity profile remains costant all along the pipe (except near the entrance and the exit). As you can see the problem is well defined and the indipendence of the solution of the x coordinate is necessary to let the non linear terms to drop out in the incompressible steady formulation. Finally, if you want to simulate this flow with CFD (it can be a test case), you DON'T have to set the condition of Vin = Vout nor the velocity profile has to be assigned. If the Re number is low, even if you assign a costant velocity at the inlet (a flat profile), the numerical solution must reach a steady state in which, after some entrance lenght, the flow exhibits it's costancy with x and is parabolic along the radius in the only one velocity component, that along the axis. At the outlet you will specify the pressure (from which a mass conservation correction to the velocity ay the exit is build) or the outflow condition on the velocity (d/dx = 0; this is different from Vin = Vout). I hope this was helpful. 
All times are GMT 4. The time now is 08:06. 