[Knight.]

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!

[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!

[xkang]

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

[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!

[xkang]

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,
thank for your reply. finally my model get work...
but i have another question.will Fluent consider gravity by itself or we need to enable the gravity option??

waiting for your reply!!

[stiboo]

You have to define it in the Solution setup/General. Tick the gravity and then define a value.

[xkang]

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

[mashimaro_star]

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

[lalith]

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?

[stiboo]

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!

[lalith]

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???

[nurfatinas]

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.

[lalith]

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.

[nurfatinas]

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).

[lalith]

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.

[nurfatinas]

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?

[stiboo]

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.

[nurfatinas]

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.

[lalith]

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!!

[sircorp]

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