# interFoam-losing fluid in free surface simulating

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

December 18, 2012, 10:30
#21
Member

Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
Hi Santiago, i tried will bigger domain at inlet (30d), but there is losing fluid yet.

Quote:
 Originally Posted by santiagomarquezd HI, two inlets is correct, but two outlets with fixed position for the free surface is not since you don't know the exact free surface position. The outlet can be only one boundary with zeroGradient for alpha1. Regards.
i always have used zeroGradient for alpha1 at outlet, but because of that the wave which forming on free surface, don't reach the outlet, maybe we can use two outlet and then fix the level of fluid! i will try and inform the result.

December 18, 2012, 10:36
#22
Member

Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
Quote:
 Originally Posted by ngj Hi Amin, Something just occurred to me. You are specifying a flow rate over the water column and you are specifying the water level at the inlet. In order to maintain this flow condition, you need some kind of driving force, which in your case can only be a horizontal component of the gravitational vector OR a slope of the free surface. Have you checked whether the slope of the free surface and hence your loss of water is not a physical sane response; especially because with the presence of the cylinder, the flow resistance is much larger than without the cylinder. Kind regards, Niels
Hi Niels
I use gravity in y direction(-9.81), why should i use gravity(g) in two component(x and y)? isn't that against of the reality?
However i'm trying the two component for g. and inform the result.

 December 18, 2012, 11:21 #23 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,609 Rep Power: 25 Hi Anim, A gravity vector pointing in the non-vertical direction is merely the same system represented in a different coordinate system, so it should work. Kind regards, Niels

 December 22, 2012, 08:45 #24 Member   Amin Join Date: Mar 2012 Posts: 60 Rep Power: 5 Hi Friends, sorry for my late reply Dear Santiago, you are right, i used two outlet for liquid and gas, but that couldn't solve. Dear Niels, i applied gravity in X direction(horizontal), for positive values the liquid loses rapidly, and for negative values liquid increases rapidly. do you think the very small negative values could help?!

 December 22, 2012, 10:27 #25 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 418 Rep Power: 14 Well, I think you should retain the enlargement of the domain and the zero gradient BC at the outlet, now, with this base try to refine the mesh towards the original interface position, both over and down the interface and try again. interFoam is a robust solver, it's only a matter of setting the proper BC's, initial conditions and mesh. Regards. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Post-doctoral Fellow Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL T.E.: 54-342-4511594 Ext. 1005 Güemes 3450 - (3000) Santa Fe Santa Fe - Argentina http://www.cimec.org.ar

 December 22, 2012, 13:22 #26 Member   Amin Join Date: Mar 2012 Posts: 60 Rep Power: 5 thanks, santiago i used the fine mesh both sides of interface and also near the cylinder before, but the problem existed. what's your idea about BC in page 1? actually i just used there and i don't know what are they exactly or how exactly work! "buoyant pressure, pressureinletoutletvelocity, calculated, ..." i read the user guide and this site posts but couldn't get something, how can i obtain good help about this BCs? because i can't understand source codes.

 December 22, 2012, 16:52 #27 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,609 Rep Power: 25 Hi Amin, Let us try something different. Close all of the boundaries but keep the present boundary condition for the cylinder. What I mean is that you apply wall boundary conditions on all the outer boundaries (equivalent to a box). Whether you use slip or noslip boundary condition should not matter. Now answer this: 1. Is the amount of water in the domain constant? a. If yes: The model is mass conserving with the present boundary conditions on the cylinder. b. If no: The boundary condition on the cylinder is wrong. If you go to "a", then the model is not loosing water per say, but what you are experiencing is rather an adjustment of the model toward a physical equilibrium. So you "loosing" water is only the model, which tries to adjust to the boundary conditions you enforce. As you do not have any driving force in the system to balance the flow resistance in the horizontal direction, the model tries to create the necessary pressure gradient; in this case a slope of the water surface. This is then what you subsequently interpret as a loss of water. By the way, what are the physical dimensions of the model? Diameter, water depth, etc. Important relative to the 1 m/s velocity at the inlet. Kind regards, Niels

 December 22, 2012, 16:54 #28 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,609 Rep Power: 25 Sorry, studied your drawing again, so you already gave the dimensions. Merry Christmas, Niels

 December 29, 2012, 07:39 #29 Member   Amin Join Date: Mar 2012 Posts: 60 Rep Power: 5 Hi Niels I put gravity in horizontal(gx=.0001) and result became better, just a few losing fluid. then i put gx=.0005 and now a little increasing in fluid. you can see the pictures. so i think we have to use Trial and Error method to obtain correct "gx" for each case. it need much time. is there any better way to solve losing problem? like write own BC for each boundary? Regards

December 29, 2012, 07:46
#30
Member

Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
Quote:
 Originally Posted by ngj Let us try something different. Close all of the boundaries but keep the present boundary condition for the cylinder. ......
i did that and put all boundaries wall except up boundary.
no-slip for velocity, buoyant pressure for "P" , and zero gradient for alpha1. and for up boundary, i put previous conditions. you can see the result that shown we don't have horizontal free surface.
Attached Images
 all-wall.jpg (13.5 KB, 14 views)

December 29, 2012, 07:56
#31
Member

Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
sorry, i uploaded pictures for post #29
Attached Images
 111.jpg (14.3 KB, 21 views) 005-0.jpg (12.3 KB, 23 views) 005.jpg (13.1 KB, 22 views)

 January 2, 2013, 12:52 #32 Member   Amin Join Date: Mar 2012 Posts: 60 Rep Power: 5 happy new year! dears, no answer for this problem yet? specially about BCs?

 January 2, 2013, 12:59 #33 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,609 Rep Power: 25 With respect to post #30 would you have forgotten to put the initial velocities to (0 0 0) in the simulation? With respect to the figures concerning the tilting of the gravity vector it looks good. The tilting of the gravity vector depends on the flow speed you want and the force on the cylinder. Kind regards, Niels

 January 2, 2013, 13:11 #34 Senior Member   Kent Wardle Join Date: Mar 2009 Location: Illinois, USA Posts: 195 Rep Power: 10 I don't think you should try to make the bottom boundary open, just make it a wall with zeroGradient and freeSlip for velocity. It seems like it is far enough from the cylinder to have any effect on the liquid rise in that region anyway--am I missing something? I don't think tweaking gravity to give the correct behavior is the right approach. I have been following along since this seems interesting--I wish I had time to try out the case on my own so I could better appreciate the issues you are having and better offer suggestions--on the surface (pardon the pun :-) ) it does seem like a pretty straightforward problem and I am confused by the issues.

 January 2, 2013, 13:34 #35 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,609 Rep Power: 25 Hi Kent, I agree that tweaking the gravity vector is not feasible in production runs if a particular mean velocity is needed, however, it is a very good way to understand what is happening in the system. I am convinced that the "loosing" of the fluid is founded in the physical adjustment of the system toward an equilibrium, though it does not seem that Amin has responded to that. This basically explains the results with the different magnitudes of the gravity tweak. One can understand the gravity tweak as a rotation of the coordinate system from a sloping channel with vertical gravity vector to a horizontal channel with a sloping gravity vector. In this way the water surface in the pure channel flow (without the cylinder) will remain horizontal, which interFoam would like very much. Kind regards Niels

 January 3, 2013, 10:58 #36 Member   Amin Join Date: Mar 2012 Posts: 60 Rep Power: 5 Hi Niels Niels, u were right, i had forgotten to set velocity to zero, so i solved again with zero velocity and there was no increasing or decreasing in liquid. u mentioned that direction in gravity depends on the inlet velocity and i think maybe height of liquid phase too. so is there any relation between them? i think the problem is because of pressure condition, specially at outlet:there is no coordination between pressure at inlet and outlet, so, outlet loses liquid to equilibrium. i read the source code of interFoam (OF 1.6): there is no modified pressure, means that the pressure used in source code is (p) not (pd=p-rho*g*h). however i read before in interFoam the pressure is (pd=p-rho*g*h). by the way so thanks to ur replies and attentions. if there is any help to solve this issue, i will be glad to hear. Regards Amin

 January 3, 2013, 11:02 #37 Member   Amin Join Date: Mar 2012 Posts: 60 Rep Power: 5 Hi Kent thanks for ur comment. now, i use slip condition at down. maybe using angled gravity not bee a good approach but as Niels mentioned, it works. however if there is the exact solution or better approach, can share with us. Regards Amin

 January 3, 2013, 11:40 #38 Senior Member   Kent Wardle Join Date: Mar 2009 Location: Illinois, USA Posts: 195 Rep Power: 10 Amin, I also wanted to comment on your use of 1.6--for this very reason--the treatment of pressure was changed between 1.6, 1.7, and 2.x in interFoam. Probably you are referring to an earlier version (1.5?) where it was pd. In 1.6 it is p, 1.7 it is p_rgh, and 2.x it is back to p. A little schizo, yes. Should not make a difference--except for maybe in your selection of BCs. Note that 2.1.x has a BC type called phaseHydrostaticPressure which might be useful to you on your outlet. This is because the actual pressure on a vertically oriented surface is not a constant--it varies with height (depth)--this BC accounts for that. Good luck.

 January 3, 2013, 14:28 #39 Member   Amin Join Date: Mar 2012 Posts: 60 Rep Power: 5 I don't access to OF 1.5 an 1.7, Kent. (p_rgh) used in 1.7 is (p - rho*g*h)?? I use buoyantPressure Bc at inlet and walls. i think it's same as phaseHydrostaticPressure that mentioned, i think. Regards

 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 sjtusyc CFX 3 September 5, 2012 18:33 sci Main CFD Forum 10 August 29, 2012 07:43 Andreas.Herwig OpenFOAM 0 March 1, 2011 13:07 lostin4ever Main CFD Forum 4 October 12, 2010 08:29 therockyy FLOW-3D 1 June 20, 2010 19:36

All times are GMT -4. The time now is 08:21.