Pressure boundary condition
While solving PPE for incompressible flow with neumann BC, the resulting pressure matrix is singular. This is because the incompressible flow is driven by pressure gradient and does not depend on pressure datum. Therefore, to solve PPE in 3D simulation, whether we should arbitrarily fix pressure only at a single node, or along a whole line or plane!

Re: Pressure boundary condition
A single node. You'd be imposing a solution if you assigned the pressure along a line or plane  think about it!
Adrin Gharakhani 
Re: Pressure boundary condition
Adrin is right. For ALL THE DETAILS, you need to see my book. Contact me if you want details. 925 422 1812

Re: Pressure boundary condition
(1). I think, whether you should specify the pressure at one point, one a line or on a surface , depends on the nature of the problem you are trying to solve.( and in turn, how you define your computational domain). (2). If the flow is stationary, that is, u,v,w are everywhere zero, then you should be able to set the pressure on all boundary surfaces equal to a constant value.(a trivial case ?) By the way, you can set the pressure gradient terms in the momentum equations equal to zero, and still can obtain proper velocity field. (3). If you are solving the flow over a flat plate, the old boundary layer flow subject to a uniform pressure, then you can also set the pressure along the outer boundary equal to a constant value. (4). Along this line, you can set pressure along the outer boundary equal to certain distribution, and this is how we solve the boundary layer equation subject to arbitrary prescribed pressure distributions. (5). The same principle also applies to the internal flows as well as the external flows in the inlet boundary condition specification. (6). So, the answer is: it depends on the problem you are trying to solve, or how you try to simulate the problem. And the best way to find out the most suitable condition for your problem is to try out different type of conditions, namely pressure at a point, or along a line, or on a surface. (7). One thing you have to remember is that, the pressure at a single point is very weak to fix the pressure field accurately through the regular secondorder pressure equation. So, if you let the pressure to float or create a computational domain such that the pressure is everywhere different,then, you will have very hard time to get accurate converged solution. So, it is very important to know your problem and know how to properly define the computational problem to your advantage. And, even if you can specify the pressure at a point in the CFD simulation, the question is, in the real testing, how do you keep the pressure in the flow field at that same point the same value so that you can make the direct comparison with the test data? (8). To specify (adjust) the pressure at a point and keep it at a constant value in the testing is nearly impossible. ( a better way to do is to simulate the testing conditions, instead of the mathematical conditions. It will save you a lot of troubles)

Re: Pressure boundary condition
The question was not what type of pressure BC to use (for what type of problem). The question was what to do with the matrix singularity that develops due to the illposedness of the Neumann problem. If you specify a line or surface of pressure, then you have a mixed BC not a Neumann BC.
The Neumann problem does not have a unique solution  or more appropriately, it has a unique solution up to a constant. Since in NS equations we deal with pressure gradients and not pressures then the value of that constant is immaterial. You can set it to anything you want and anywhere you want it. That "anchors" your Neumann problem. In essence, we have changed the purely Neumann problem to a new problem with mixed NeumannDirichlet BC's (where the D. B.C. is available at one point). But the new mixed problem has a unique solution. This has been dealt with analytically, and numerically in the FVM, FEM and BEM contexts. In the numerical implementation, though, one has to be careful with satisfying the compatibility contraint. In the FEM and BEM worlds (pretty sure that's a possible source of problem in FVM too) the matrix has to be modified to account for this effect. Basically, when one sets the pressure at one point to a constant (say zero) and obtains the pressure everywhere else (subsequent to solving the matrix) the surface pressure may not be compatible. And compatibilty will give a new pressure value at the fixed point which is actually different from zero! This is a matter of resolution. For a novel solution of the Neumann problem by BEM check A. Gharakhani & A.F. Ghoniem, "BEM Solution of the 3D Internal Neumann Problem and A Regularized Formulation for the Potential Velocity Gradients," Int'l. J. of Numer. Meth. in Fluids, Vol. 24, No. 1, pp 81100, 1997 Adrin Gharakhani 
Re: Pressure boundary condition
(1). I guess, at the wall, the normal pressure gradient is normally specified as zero. (If that is what you called Neumann condition) (2). So, it is fine to use zero gradient condition at the wall. But, then, it will float in the streamwise direction. And it will take longer for the solution to converge, that is why the boundary layer type was invented. (3). Other than the walls, one can try to model the inlet, exit, farfield in such a way that the pressure itself is modelled or prescribed (that must be the Dirichlet condition, I think, I am not used to this type of terminology anyway. Such terminology is not common in CFD codes) (4). The point I was trying to make is: it is fine to define the problem according to the mathematics, but it is far more important to know your flow problem and be able to modelled it to your advantage. (if that means you have to change the type of the boundary conditions , the domain of the computational problem, or the governing equation itself. ) (5). For a 2D cavity flow with a sliding lid, the problem was solved long time ago without using the pressure equation. It is fine to use the pressure equation, but then, one has to drill a hole on the cavity wall to pressurize the cavity at that precise point, such that the CFD calculation and the testing pressure can match at that point. Everywhere else, the pressure gradient condition is used on the walls. The other way to say is that, the manmade pressure equation do not have unique solution. The nature does not care, and it is purely a mathematical formulation problem. (6). In the cavity flow with a sliding lid, where is the right place to specify the pressure? Anywhere? Will it affect the pressure solution? I think so.

Re: Pressure boundary condition
I find the following point of view helpful. In nature, the absolute value of pressure does make a difference to a flow field: by its affect on density. If you write density=P*R/T, for example, it is clear that the Navier Stokes equation contains an explicit dependance on Pressure, not just the pressure gradients.
If we make the assumption of incompressible behaviour, the absolute value of the pressure does not matter, both in nature and in computation. In such cases, it is pointless to wonder where to "fix" the pressure: anywhere is fine, so long as it is just one computational node. As for comparison with experiment, the computed pressure field can easily be offset by a constant amount to make it match any given point, and the variation at the other points can be compared. By the way, my experience has been that it is almost always more problematic to solve with P specified along an entire face (the "Pressure boundary condition" in commercial codes) than to specify a fixed inlet velocity (if known) and a reference pressure location. Especially if the region in question is large, you end up with recirculating flows across the boundary plane, which can't be suppressed by the constant pressure condition. 
All times are GMT 4. The time now is 16:02. 