# Slip boundary condition giving strange results

 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 17, 2007, 11:24 Hi! I am currently modeling #1 Senior Member   Rasmus Hemph Join Date: Mar 2009 Location: Sweden Posts: 108 Rep Power: 9 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 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, 21:13 Hi Rasmus, Wanna post your #2 Senior Member   Ziad Boutanios Join Date: Mar 2009 Location: Montréal, Canada Posts: 114 Rep Power: 9 Hi Rasmus, Wanna post your configuration files and maybe your mesh? cheers, Ziad

 January 18, 2007, 05:22 Hi Rasmus I have been playi #3 New Member   Joakim Möller Join Date: Mar 2009 Posts: 26 Rep Power: 9 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, 06:15 Hi, I did a bit more investig #4 Senior Member   Rasmus Hemph Join Date: Mar 2009 Location: Sweden Posts: 108 Rep Power: 9 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(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 Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post A.T. Main CFD Forum 7 November 28, 2012 04:19 vas FLUENT 11 August 6, 2012 06:36 kumar2 OpenFOAM Running, Solving & CFD 8 March 24, 2008 19:38 Sohag CFX 1 June 21, 2007 06:34 lei wang FLUENT 0 May 16, 2007 22:47

All times are GMT -4. The time now is 12:45.