Boundary conditions for a free surface flow using interfoam
2 Attachment(s)
HI all! I simulate flow in a channel with a free surface using interfoam solver. For this purpose I built a channel with length of 10 meters, width of 2 meters. For the velocity, pressure and alpha asked the following boundary conditions:
Code:
FoamFile Code:
FoamFile Code:
FoamFile Code:
FoamFile Attachment 16632 Attachment 16633 Нow can I fix it? What I asked wrong in the boundary conditions? Thanks! Regards, FrolovOY |
Hi FrolovOY,
could you tell what cell size you apply, and maybe post your transportProperty file? The surface between air and liquid depends on the grid and on the transportProperties... |
1 Attachment(s)
Quote:
Code:
FoamFile Code:
FoamFile I would be grateful for your help. Attachment 18086 Thanks! Regards, FrolovOY |
Hi Frolov,
why you have such a high kinematic viscosity for alpha1 ? Quote:
|
Quote:
- have you tried using -1 to 3 instead of 0 to 2 in the setFieldsDict? Maybe the fact that you put it exactly on the boundary is the issue - the other thing is indeed the extremely high viscosity (10000 Pas so 1E8 bigger than that of water) which might cause excessive wall drag therefore causing a sort of vena contracta type of behaviour Edit: given the other properties you use I guess you meant to use the (kinematic) viscosity of whether. Which is 1e-6 |
Quote:
|
2 Attachment(s)
Quote:
Following your advice, I expanded setFields borders on Y ((-1 -1 0) (3 4 1) ;), but it did not help. Liquid with small kinematic viscosity (eg water) behaves well. See Figure 1. (Nu = 1.3 * 10e-6; deltaX = 0.05 m) Attachment 18332 Figure 2 shows the flow of fluid with a high kinematic viscosity without gravity. Attachment 18333 It is seen that during the motion between the fluid and the wall is formed air. But it is given no-slip condition? Code:
upperWall Maybe to simulate motion of polymers or similar to them, there is another solver rather than interfoam? How can I set the phase1 parameters (in my case, HDPE) for the non-Newtonian fluid in a file transportProperties? May be it is necessary to ask the contact angle in alpha1 file? |
No slip means that at your boundary nothing moves, so it might be the air cant be pushed away here, although I didn't face that problem in my simulations. With low viscosity your cell center at the boundary probably gets an alpha1 value of liquid due to the high possible gradient in the phase interface, so you won't see the air in your longitudinal sections, but maybe you could check this if you look at the boundary itself in paraview, colored by cell values of alpha1, not by interpolated values.
The other more reasonable explanation would be that because you have no gravity there is no buoyancy to move the air upwards from the lower boundary, which could be the reason for the difference between your two simulations. |
Quote:
That said, for a sharp interface the viscous stress diverges at the contact line because of the no-slip condition and the rate of divergence is obviously worse when the viscosity of the fluid is higher. Therefore it might be (I am guessing a bit here), that the very high viscosity of your fluid causes the contact line to remain immobile, despite the diffuse interface. What you could try to get rid of the stress singularity is to use a navier slip BC to see if that indeed makes the contact line mobile. [EDIT] for a first try you can use the partialSlip BC, if it indeed works you can always implement the navier slip BC for more `logical' behaviour |
All times are GMT -4. The time now is 15:36. |