[hconel]

Hi,
I'm imposing slip type boundary condition for U at the top of my solution domain. However, I get non-zero normal velocity component at this boundary:



I am really puzzled because as far as I know, slip BC imposes zero vertical component at the boundary. The vertical cylindrical boundary seen here has time-varying inlet-outlet (flow angle rotates with time) velocity of 10 m/s. So the 18 m/s vertical component at the top boundary I'm getting is clearly abnormal and non-neglectable.

Note: the bottom boundary also has slip BC and the same happens there.

How is this possible? Did anyone experience something like this?

solver: pimpleFoam
turbulence: laminar
top BC: U slip, p zero
vertical boundaries: time-varying inlet-outlet (flow angle rotates with time)
ddt scheme: 2nd order
div schemes: 2nd order
momentum predictor: on
nOuterCorrectors 2;
nCorrectors 2;
nNonOrthogonalCorrectors 1;

Regards,
Huseyin

[piu58]

You should set a defined p only at one cell, the p reference. And not at the boundary. p may change here.

[hconel]

Originally Posted by piu58

You should set a defined p only at one cell, the p reference. And not at the boundary. p may change here.

Mr. Uwe,
Thanks for the heads-up, indeed, it is something that can be easily overlooked!
I've set the pRefPoint to the middle of the domain, however, it did not work.
The problem was setting pressure to fixedValue 0 on the same boundary as the velocity slip condition. Changing pressure to slip fixed my problem (although I've always though that slip BC is reasonable only for vector fields). Zero gradient also seems to work.

The weird thing is, OpenFOAM does not complain about not being able to satisfy the given boundary conditions. I guess this is due to the segregated nature of the pimple solver algorithm; pressure and velocity systems are solved separately?

FYI: OpenFOAM version is 2.4.0

Hope this helps others. Regards!