# VOF Model/Pipe Flow/Capillary Flow

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

 April 9, 2014, 21:00 VOF Model/Pipe Flow/Capillary Flow #1 New Member   Join Date: Apr 2014 Posts: 1 Rep Power: 0 Hey guys, Currently, I've been working extremely hard at getting a simple semi-working model of water flow in a horizontal capillary tube. (I have also attempted just using the VOF for water flowing in a pipe, just to get familiar with the program, as I am completely new to FLUENT, and CFD in general). Basically, regardless of the scale (pipe vs capillary tube), I am unable to obtain a working simulation which I can observe, in a video, the water forming a meniscus and flowing through the pipe. This seems like such a simple problem, and benchmark; however, I am unable to find any tutorials on something like this. I first attempted a 3D model, then turned to 2D for simplicity, and to attempt to better learn the program. The current setup I am trying to debug is as follows: -The channel is 2D rectangle in the mesh, with dimensions 2.5um tall and 100 um long. (the height is actually 5um tall, but I'm splitting it in half and calling the bottom an "axis" for the BC in order to use axisymmetric). -VOF is turned on. The scheme is Explicit with a volume fraction cutoff of 1e-06 and a courant number of 0.25. -The primary phase is air, the secondary phase is water. The surface tension coefficients are 73.5 n/m. Wall adhesion is turned on. -Operating Conditions: Operating pressure is atmospheric pressure with a reference location of 100micrometers in the x and 1.25 micrometers in the y. [I am unsure of what this condition does, so it is the first point there could be a problem]. -As mentioned before, the bottom boundary of the rectangle is an "axis," the inlet is "velocity inlet," with a small velocity of 0.001 m/s, the outlet is a "pressure outlet," and the wall is a wall. The wall BC has no slip and a contact angle of 20 (somewhat arbitrary). All three of these boundary conditions are specified somewhat arbitrary, because I would just like to see this model do SOMETHING, and I can tune it from there. Also I will have experimental velocity and calculated contact angle eventually, which is why I'm hoping that the actual number for these BCs can be somewhat arbitrary until I receive that data. But all of these BCs could potentially be a source of the problem. -The solution methods are as follows: SIMPLE for pressure-velocity coupling, Lease Squares Cell Based for gradient, PRESTO! for pressure, Second Order Upwind for momentum, and Geo-Reconstruct for volume fraction. -I then initialize the gauge pressure to 50600 and the axial velocity to 0.001 m/s. Then I go to patch, phase-2 (which is water), turn value to 1, click "surface_body" as zone to patch (which is the only zone) and then patch. This zone is another potential source of a problem, as even with reading much of the FLUENT manual, I'm not sure exactly what this is doing, other than that other people have done it. -The last thing is the time step size, which I am unsure of and which is also another probable source for the problem. Currently set on 1e-5 time steps. I was wondering if anyone has done a similar problem, as it seems so basic. I am trying to change many different parameters, but as you can tell, my lack of experience is making it difficult for me to narrow things down. Also this was done on a micro-scale channel. I would be fine if it was also done in a regular-sized pipe. Any help is appreciated! Thanks guys! rgd, 6863523 and dhaval patel like this.

 May 22, 2014, 04:27 Capillary flow modeling #2 New Member   Márton Stibrányi Join Date: Mar 2014 Location: Hungary Posts: 7 Rep Power: 5 Hi, I also simulate such problem in a vertical flow, so I try to give you some hints. You have to define the contact angle between the water and the wall, typically less than 90 degree. Absolute Pressure = Operating pressure + Gauge pressure You should define atmospheric pressure in the operating conditions, and 0 for gauge pressure at the boundaries. Why do you define an axial velocity? I think you should not define an initial velocity, because the surface tension will trigger the flow to move, and 0.001 m/s is very high anyway, since you are in microscale. Turn on double precision when you start fluent. Instead of the SIMPLE, you should use the PISO pressure-velocity coupling. Instead of the velocity-inlet, you should have a pressure-inlet with volume fraction of 1 for water, and a pressure-outlet with 0 backflow volume fraction for water. Set the gauge pressure to 0 for both. Define a domain initially filled with water (patch), and let the transient simulation begin. Good luck! sircorp, rgd and 6863523 like this. Last edited by stiboo; May 22, 2014 at 10:10.

 June 23, 2014, 21:37 capillary flow model #3 New Member   MI Join Date: Jan 2014 Location: Michigan Posts: 11 Rep Power: 6 Hi, i think i am in the same condition as you(without any experience).i am struggling with Fluent model too.So did you get your model work? if it is possible,i really hope you can give me some hint for the same simulation as yours. thanks ahead, kang

 June 26, 2014, 05:10 #4 New Member   Márton Stibrányi Join Date: Mar 2014 Location: Hungary Posts: 7 Rep Power: 5 My simulations are working now. See my suggestions related to the settings in #2. However, it is numerically unstable, so you have to keep the Courant number/Time step size low. I am using variable time stepping. Hope these help! rgd and chaitanyaarige like this.

June 26, 2014, 09:49
capillary flow model
#5
New Member

MI
Join Date: Jan 2014
Location: Michigan
Posts: 11
Rep Power: 6
Quote:
 Originally Posted by stiboo My simulations are working now. See my suggestions related to the settings in #2. However, it is numerically unstable, so you have to keep the Courant number/Time step size low. I am using variable time stepping. Hope these help!
Hi stiboo,
but i have another question.will Fluent consider gravity by itself or we need to enable the gravity option??

 June 26, 2014, 10:01 #6 New Member   Márton Stibrányi Join Date: Mar 2014 Location: Hungary Posts: 7 Rep Power: 5 You have to define it in the Solution setup/General. Tick the gravity and then define a value.

June 26, 2014, 10:21
capillary flow model
#7
New Member

MI
Join Date: Jan 2014
Location: Michigan
Posts: 11
Rep Power: 6
Quote:
 Originally Posted by stiboo You have to define it in the Solution setup/General. Tick the gravity and then define a value.
thanks for your reply! i will try it now. But i am also thinking should i consider gravity since it is a capillary tube. i post the simulation result in my another thread yesterday. if you have time please take a look

 July 8, 2014, 19:33 #8 New Member   yu feng Join Date: Jun 2010 Posts: 3 Rep Power: 9 Hi Knight, I am simulating a 2D transient capillary flow too using Fluent. right now, my velocity field seems weird. Are you able to share your velocity contour near the meniscus? If you have good velocity field result, could you please share some experience? Thank you very much. Best wishes, Yu

 August 12, 2014, 05:52 #9 New Member   syunary Join Date: Aug 2014 Posts: 7 Rep Power: 5 Hi Stiboo, I guess I have been modeling the problem as per your suggestions. I get nothing but the reversed flow at many faces and both at the inlet and outlet. And if we patch the whole domain with water how can we see the meniscus (at the air/water interface), though I have not been able to reach at the stage. What could be the mistake that introduces this reversed flow error?

 August 13, 2014, 07:49 #10 New Member   Márton Stibrányi Join Date: Mar 2014 Location: Hungary Posts: 7 Rep Power: 5 You have two options at the inlet: set the inlet to mixture, if you do not define the volume fraction of the incoming fluid, set it to "mixture" (the solver will find out which phase will come in), if you want water flowing in, than switch to water phase and set the volume fraction to 1. Do not fill the whole domain with water, initialize it with only a small amount, and see whether the capillary flow starts or not. You can initialize water in the middle of the domain as well, with air in front of and behind it. The shape of the meniscus and the magnitude of the capillary forces depends on the contact angle. Don't worry about reversed flow, you can't help it. Good luck!

 August 14, 2014, 07:37 #11 New Member   syunary Join Date: Aug 2014 Posts: 7 Rep Power: 5 The domain is initialized with water, only near the inlet with alpha=1 at inlet,rest is air. The problem is: with a coarse grid, the interface is not very well tracked and after adapting the grid I had to reduce the time interval to 1e-10. So now the simulation has been running for quite a long with just "REVERSED FLOW ....." on the screen. I doubt whether the wetted wall boundary condition is compatible with NO SLIP???

 December 7, 2014, 13:08 #12 New Member   nurfatin Join Date: Dec 2014 Location: malaysia Posts: 6 Rep Power: 5 Hi everyone, I'm working on 3d horizontal capillary flow. Basically I've tried the setting as Stiboo mentioned in #2 post. The setting are as below; Transient. VOF. explicit scheme. Pressure based solver. Surface Tension. Wall adhesion. CSF. Surface tension coeff. =0.03N/m. Primary phase: Air. Secondary phase: another fluid. BC's Operating pressure: 101325Pa (atmospheric) Pressure inlet & outlet = 0Pa Initialization of solution. I set inlet reference where pressure is zero since I working on capillary driven flow. I tried SIMPLE and also PISO scheme. Momentum: first order upwind VOF: compressive Energy: first order upwind I played around the urf value. I lowered them a bit because I thought it would help to keep solution from diverging. But as the simulation run, it became numerically unstable and there is warning that Global Courant Number exceed 250.00. I had tried variable time stepping too but it keep diverge. So I lowered the time step size up to 1e-10 s but it takes way too long to compute the flow. Is there any suggestion for this case? Implicit scheme seem to give weird solution ( is it even possible to use implicit for this case?). I'm also thinking about using NITA, but I don't really understand how it works, the solution seems weird too. Hoping for reply. Thanks in advance.

 December 8, 2014, 10:12 #13 New Member   syunary Join Date: Aug 2014 Posts: 7 Rep Power: 5 Hi nurfatinas I've been working on a similar problem. I chose to go with the default schemes, like the Geo Reconstruct for vof, except for pressure-velocity coupling, for which I chose PISO (read somewhere) Also you may try to solve just the capillary flow first, decoupling the energy equation, which you may add later. I could not really do anything for the issue of very low time steps and have to use a step of 1e-8. One thing is for sure that for such a problem we have to have a high end computational facility.

 December 8, 2014, 12:49 #14 New Member   nurfatin Join Date: Dec 2014 Location: malaysia Posts: 6 Rep Power: 5 Thanks Lalith for your response. May I know what type of mesh you're using for this problem. I find it hard to keep the solver iterating when using tetrahedral (and sometimes the flow seem unrealistic), when I changed the mesh to quadrilateral it works better except for it being unstable at times. The things is when I work further on the quadrilateral mesh model with the previous setting I had mentioned before, the fluid became static after a while (after quiet some time of iterations). Btw l'm modeling the fluid flow through two parallel plate (capillary driven flow).

 December 9, 2014, 13:29 #15 New Member   syunary Join Date: Aug 2014 Posts: 7 Rep Power: 5 The geometry I am working on is triangular and so I am using the Triangular mesh. I can't really comment on why the fluid becomes static. Can't really think of a physical reason for that in case of horizontal plates. You may look for the meniscus shape whether it is as per the contact angle specified or not. Also if the plate widths in your problem are larger than the gap between them you may try to solve a 2D model first.

 December 11, 2014, 02:32 #16 New Member   nurfatin Join Date: Dec 2014 Location: malaysia Posts: 6 Rep Power: 5 I managed to simulate the flow now, but the flow seems wavy. I guess it really need small time step size. For my case, the flow filling time is what I observed. So may I know which scheme should I use? Implicit or explicit, and why?

 December 11, 2014, 11:08 #17 New Member   Márton Stibrányi Join Date: Mar 2014 Location: Hungary Posts: 7 Rep Power: 5 For larger time steps the explicit scheme is more unstable. But this problem requires very small time steps to converge, and for small time steps, the explicit scheme is faster. I used variable time stepping with a constant Courant number of ~0.2. Structured meshes with hexa or quadrilateral elements worked better for me, but I also experienced that they are more unstable. In my simulations, after the capillary and the gravitational forces reached an equilibrium, the flow became static, but this has met my expectations.

 December 15, 2014, 06:50 #18 New Member   nurfatin Join Date: Dec 2014 Location: malaysia Posts: 6 Rep Power: 5 I had tried your suggestion but still I'm facing the same issue. The earlier iteration would results wavy flow as in the attached picture and it getting worsen through the rest of calculations. I'm using tetrahedral mesh (the inner had some spherical actually so I couldn't use the other type of mes) and the other setting are; 0.03 N/m surface tension coefficient and 30degree angle of wall adhesion. Boundary conditions at pressure inlet and outlet is set at 0 (to consider only capillary action). Initial condition are set as the inlet BC. If anyone can advise me, what is actually wrong with my model? Is the problem with mesh? Thanks.

 March 8, 2015, 12:01 #19 New Member   syunary Join Date: Aug 2014 Posts: 7 Rep Power: 5 Even for a finer mesh similar wavy INTERFACE can be seen, (after longer time steps though). It seems to be a demerit (numerical oscillations) of the vof scheme while solving two phase flows with large property differences (large density ratio, vicosity ratio etc.) as for water and water-vapour combination The interface may get more and more diffuse and impossible to track. Stuck with the same problem!!

June 7, 2015, 04:30
#20
Member

Shane
Join Date: Oct 2009
Posts: 52
Rep Power: 10
Quote:
 Originally Posted by stiboo Hi, I also simulate such problem in a vertical flow, so I try to give you some hints. You have to define the contact angle between the water and the wall, typically less than 90 degree. Absolute Pressure = Operating pressure + Gauge pressure You should define atmospheric pressure in the operating conditions, and 0 for gauge pressure at the boundaries. Why do you define an axial velocity? I think you should not define an initial velocity, because the surface tension will trigger the flow to move, and 0.001 m/s is very high anyway, since you are in microscale. Turn on double precision when you start fluent. Instead of the SIMPLE, you should use the PISO pressure-velocity coupling. Instead of the velocity-inlet, you should have a pressure-inlet with volume fraction of 1 for water, and a pressure-outlet with 0 backflow volume fraction for water. Set the gauge pressure to 0 for both. Define a domain initially filled with water (patch), and let the transient simulation begin. Good luck!
Thanks "Stiboo" Wonderful explanation

I am in same boat. I have vertical multi fluids system. Had some issue with pressure based system so I moved to density based solver.

(Pic Attached) http://www.cfd-online.com/Forums/mem...luidsystem.png

Now it has become bit inconsistent. Reverse flow is major issue and solver drops out after few iterations . What worked yesterday today dropped half way. May be Memory Allocation Issue. Bit frustrating.

Shane

 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 rsaha FLUENT 5 April 10, 2016 17:28 Jing Main CFD Forum 5 March 2, 2013 15:02 adam14qin FLUENT 0 July 28, 2012 04:02 CRT FLUENT 0 July 20, 2012 13:03 Luke1984 FLUENT 6 October 19, 2009 09:59

All times are GMT -4. The time now is 00:09.