pressure wall boundary condition in CFX
I have a question concerning the pressure at wall boundaries in CFX. I am studying the flow around an obstacle (e.g. a sphere). When I plot the pressure along the streamline ending in the stagnation point, I observe the following behaviour: The pressure and it's gradient increase constantly while moving closer to the wall, but if you look closely you can see that the pressure gradient decreases again in the last cells before the wall boundary. See the red curve in the attached picture. The black curve is what I would expect from my physical understanding.
My questions are:
1) Is this behaviour caused by a dp/dn = 0 pressure boundary condition at solid walls in cfx?
2) As far as I know, segregated solvers that solve a Poisson equation for pressure-velovity coupling definately need a boundary condition for the pressure. I am not sure how this is in a coupled solver like CFX. Can anybody shed some light on this for me?
3) If dp/dn= 0 is applied: How can expect my simulation results to reflect reality when I use a physically wrong boundary condition? I made a test case to study the drag on a sphere. The drag coefficient pretty accurately agrees with the literatury values. I would like to know why.
Any help is appreciated!
Nice question, well spotted.
1) I am not sure exactly where this comes from but it probably comes from the zero normal gradient condition. Also I am not sure your black curve is correct - I would check what the correct curve is and not just assume.
2) I do not think it is in the documentation but I am pretty sure CFX also uses the zero normal pressure condition at wall boundaries. It is not unique to segregated solvers, it is a pretty common assumption in most CFD codes.
3) The error gets smaller as mesh resolution is increased. So if your mesh is fine enough to be accurate then you know you have reduced the error from this effect to a manageable amount.
Also: Note the zero normal gradient is an assumoption which only applies at moderate to high Re numbers. At low Re this assumption is not correct and can lead to errors in low Re flow. I do some work in MEMS structures with very low Re and have found some problems with the zero normal gradient assumption leading to systematic error.
But fo the vast majority of flows with moderate to high Re the zero normal gradient assumption is quite accurate.
So far, I got down to Reynolds numbers of approx. Re = 1e-3. And I remember a bouncy behaviour of my monitor points (which are the forces and torques on a solid body) in the low Re cases. I may have to go even lower in future.
Any suggestions for a solver to use, that allows a different condition at walls?
At Re=1e-3 I would expect to see that you might also see convergence difficulties. As inertia plays such a small role it can be neglected, so a Stokes solver is more appropriate.
Unfortunately I do not know of any CFD codes which allow a proper low Re treatment of pressure, and I do not know of any Stokes solvers either. I know OpenFoam, FreeFEM, matlab and similar packages can be configured to Stokes flow but you will have to set it up.
In my test case, the drag coefficient on a sphere at Re=1e-3 differed only about 2.5% from the literature value. The difference between different literature sources is in the same order of magnitude. So I am pretty ok with that. The convergence was also no problem for the test case. I will try lower Re cases and see how that works out.
I am interested in the inertial lift force on a sphere in poiseuille flow. Solving the Stokes equation yields zero lift, so I am restricted to real CFD solvers I guess. So maybe the way to go is to simply increase the wall-normal mesh resolution so much that even for very low Re, the wrong pressure BC does not affect my results.
|All times are GMT -4. The time now is 01:48.|