[Skaiwalker]

Hello all,

I learned a lot from the members of this awesome forum but by now I can't get my head around the hydrodynamic pressure and its point of reference:

I made a simple cuboid case, with z=0m at the bottom and z=0.1m at the top, the case is attached. I set the top plane as "fixedValue uniform 1e5" in "0/p" and "0/p_rgh" and "U=noSlip" at the entire boundary. But, as can be seen in the attached picture (top plane: boundary "air", sides show the internal mesh), the pressure distribution is wrong: It decreases from 1e5 at the bottom to ~.98e5 at the top. It should be 1e5 at the top (as stated in the boundary file) and ~1.2e5 at the bottom.

So the question is: Why is my boundary condition not accepted or what am I missing?


Background info on provided case: I want to simulate ingot melting in a crucible. The top plane represents the melt-air interface (pressure = 1e5Pa). The solver is buoyantPimpleFoam using an fvOpttion of type solidificationMeltingSource for ingot modeling. pRef cell is a cell at the top of the domain set to pRefValue 1e5.

PS: When I adjust the mesh to be z=0 at the top and z=-0.1m at the bottom the pressure distribution is right, represented by blockMeshDict_adjusted in the uploaded case.

Thank you very much in advance! Greetings
Kai

[Carlo_P]

In he first case, there is a conflict between p and p_rgh.
It is not possible that both have the same value at 0.1m.
Only in the second case they have the same value, because rgh=0, so p and p-rgh are the same.


In the first case, if p_rgh is 1e5, the pressure is something less.


Is 1e5-1.2*9.81*0.1=1e-5-1.1772=99998 as shown.


So, the p file is ignored and only the p_rgh is taken in account.

[Skaiwalker]

Thank you for your fast and precise answer! Sometimes one misses the wood for the trees

After tinkering around with the boundarys a bit, I found the "prghPressure" boundary condition, which sets the pressure to my pleasure!