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/)
-   -   Slip boundary condition giving strange results (http://www.cfd-online.com/Forums/openfoam-solving/59858-slip-boundary-condition-giving-strange-results.html)

hemph January 17, 2007 11:24

Hi! I am currently modeling
 
Hi!
I am currently modeling two-phase flow using the twoPhaseEulerFoam-application. As a boundary condition for the velocity of the dispersed phase at the outlet, I set the slip-condition. From the user manual, this boundary condition should limit the velocity normal to the face to 0, and the tangential velocity to zero gradient.

However, I get an outflow of particles/dispersed phase through this boundary!

(snip from the output log at successive time steps)
Dispersed phase volume fraction = 0.0327019 Min(alpha) = -2.2858e-31 Max(alpha) = 0.237186
Dispersed phase volume fraction = 0.0327019 Min(alpha) = -6.25311e-33 Max(alpha) = 0.237186
Dispersed phase volume fraction = 0.0326999 Min(alpha) = -2.19122e-31 Max(alpha) = 0.237179
Dispersed phase volume fraction = 0.0326999 Min(alpha) = -5.10842e-33 Max(alpha) = 0.237179
Dispersed phase volume fraction = 0.032698 Min(alpha) = -2.10048e-31 Max(alpha) = 0.237171
(/snip)

The flux of phia is of non-zero.

(example from phia-output file)
outlet
{
type calculated;
value nonuniform List<scalar>
12
(
2.93748e-10
3.68239e-10
4.54842e-10
5.29354e-10
5.82653e-10
6.10416e-10
6.10416e-10
5.82653e-10
5.29354e-10
4.54842e-10
3.68239e-10
2.93748e-10
)


It is important to the simulation that the particles stay within the domain! Am I misunderstanding something about the slip boundary condition?

Best Regards
Rasmus H

ziad January 17, 2007 21:13

Hi Rasmus, Wanna post your
 
Hi Rasmus,

Wanna post your configuration files and maybe your mesh?

cheers,
Ziad

joakim January 18, 2007 05:22

Hi Rasmus I have been playi
 
Hi Rasmus

I have been playing along with interFoam using both the slip and the symmetry condition (in 2D). In both cases I get convergence problems, with pressure oscillations along the surface, whereas when I change he b.c. to a wall condition, everything works fine.

Has anybody else had any equal experiences?

Regards

/Joakim

hemph January 18, 2007 06:15

Hi, I did a bit more investig
 
Hi,
I did a bit more investigation. The slip condition does actually set the outward velocity Ua to zero for the dispersed phase. The problem is that the corresponding flux field phia does not know about this.. For the case where the boundary condition is derived from fixedValue, phia is updated correspondingly in phaseModel/phaseModel.C.

In the present case of a slip boundary condition, this update is not performed, and phia and Ua are not strictly coupled. I added a test for slip b.c. to phaseModel.C as:

if
(
isType<fixedvaluefvpatchvectorfield>(U_.boundaryFi eld()[i]) ||
(U_.boundaryField()[i].type() == "slip") )
{
phiTypes[i] = fixedValueFvPatchScalarField::typeName;
}

which seems to do the trick. This might have other implications which I am not aware of. Generally, care needs to be taken to boundary conditions which are not fixed value, but should stop one of the phases.


All times are GMT -4. The time now is 09:23.