|
[Sponsors] |
Slip boundary condition giving strange results |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 17, 2007, 10:24 |
Hi!
I am currently modeling
|
#1 |
Senior Member
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 17 |
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 |
|
January 17, 2007, 20:13 |
Hi Rasmus,
Wanna post your
|
#2 |
Senior Member
Join Date: Mar 2009
Location: My oyster
Posts: 124
Rep Power: 17 |
Hi Rasmus,
Wanna post your configuration files and maybe your mesh? cheers, Ziad |
|
January 18, 2007, 04:22 |
Hi Rasmus
I have been playi
|
#3 |
New Member
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 17 |
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 |
|
January 18, 2007, 05:15 |
Hi,
I did a bit more investig
|
#4 |
Senior Member
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 17 |
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. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
SLIP BOUNDARY CONDITION | vas | FLUENT | 12 | June 27, 2019 05:48 |
Non-slip Boundary condition | A.T. | Main CFD Forum | 7 | November 28, 2012 03:19 |
RasInterFoam STRANGE RESULTS AT BOUNDARY | kumar2 | OpenFOAM Running, Solving & CFD | 8 | March 24, 2008 18:38 |
"Slip Boundary Condition,Help me Please" | Sohag | CFX | 1 | June 21, 2007 06:34 |
strange things happen with slip boundary | lei wang | FLUENT | 0 | May 16, 2007 22:47 |