CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Stokes Flow Simulation (http://www.cfd-online.com/Forums/openfoam-solving/125136-stokes-flow-simulation.html)

angushendrick October 19, 2013 17:11

Stokes Flow Simulation
 
I am trying to find the steady-state velocity field for laminar flow transverse to a random array of parallel cylinders using simpleFoam in OpenFOAM 2.2.1. I am using empty boundary conditions on faces normal to the cylinder axes and cyclic boundary conditions for the other faces. The flow is supposed to be driven by gravity acting in one of the two cyclic directions.

The simulation does not work. It converges to a velocity that approaches 0, if seeded with non-zero velocities (as the attached case does). It appears that the gravitational term is ignored, though I have included "g" in the constants directory.

The case is zipped here. I'm sure I'm doing something stupid. Any help, especially if it wittily points out just how stupid I am, is much appreciated.

m5m5kh October 20, 2013 23:58

Quote:

Originally Posted by angushendrick (Post 457848)
I am trying to find the steady-state velocity field for laminar flow transverse to a random array of parallel cylinders using simpleFoam in OpenFOAM 2.2.1. I am using empty boundary conditions on faces normal to the cylinder axes and cyclic boundary conditions for the other faces. The flow is supposed to be driven by gravity acting in one of the two cyclic directions.

The simulation does not work. It converges to a velocity that approaches 0, if seeded with non-zero velocities (as the attached case does). It appears that the gravitational term is ignored, though I have included "g" in the constants directory.

The case is zipped here. I'm sure I'm doing something stupid. Any help, especially if it wittily points out just how stupid I am, is much appreciated.

Hi Angus and welcome to this forum
take a look to this project specially page 23 ;) I think it would be helpful for your case

http://www.diva-portal.org/smash/get...T01.pdf‎

best regards
Mohsen

angushendrick October 21, 2013 21:00

Thanks for the response to my question. I read the paper you linked, and while it is broadly related (i.e., flow around cylinders), I don't find a discussion of the problem I am having. That is, in my case I need to generate body-force (i.e., gravity) driven flow.

Bernhard October 22, 2013 01:56

There is something physically wrong with what you expect. You have a fluid with constant density. How would gravity act on it? E.g.: in a bottle of water there is no movement.

angushendrick October 22, 2013 20:21

The simulation is set up so that it has cyclic boundary conditions top and bottom. With gravity acting downward, I expect that all the fluid will fall, exiting the bottom and re-entering at the top. Because of the no-slip boundary conditions on the cylinders within the domain, I expect that it will eventually reach a steady state where the momentum added by gravity is equal to the momentum lost at the solid surfaces.

I recognize that if gravity is added as a modified pressure, then there will be no flow, and so an explicit body force term may be necessary. I don't know how to add this if it is.

angushendrick November 3, 2013 16:33

Solution using a vectorSemiImplicitSource
 
Putting the following in system/fvOptions is my current approach. It seems to work.

momentumSource1
{
type vectorSemiImplicitSource;
active true;
selectionMode all;

vectorSemiImplicitSourceCoeffs
{
volumeMode absolute;
injectionRateSuSp
{
U ((1e-6 0 0) 0);
}
}
}


All times are GMT -4. The time now is 00:39.