Hi,

I need help with simulating surface tension driven flow at low wall contact angles.

I am simulating capillary rise in a 2D straight channel. The initial condition is a flow front at z = 0 and we are tracking how the flow front evolves in time.

The expected results is that the velocity of the flow front direction should be proportional to cos(wall angle) since the wall adhesion is the only driving force and the flow is completely laminar.

The results look nice for contact angles around 40 - 60 degrees, but when the contact angle is reduced below 40deg, the velocity remains unchanged. It seems like the curvature of the flow front is not fully captured in the simulations and an increase in curvature close to the wall does not increase the surface tension force.

I tried to reduce both mesh size and time step but this made the flow front unstable and wavy.

Does anyone have any ideas on how to simulate capillary rise at low contact angles.

Thank you for your help!

- Terje

Hi,

CFX does not do surface tension very well in my experience and is particularly bad at small wall contact angles. Having said that all CFD codes I have played with are bad with small wall contact angles.

To get it to work in CFX, have a look at the free surface smoothing - my modelling worked a lot better after turning the free surface smoothing off. Other hints include don't use the coupled VF solver and use adaptive timestepping aiming for 3-6 iterations per timestep.

Glenn Horrocks

Hi,

thank you Glenn! I am already using the inhomogenous model and have also, as you, experienced better results with no smoothing. I will try using adaptive time stepping, (so far I have been using a constant time value based on how far the flow front should move) but not spend too much more time on trying to get these simulations right.

- Terje

Hi,

Sorry, I did not say to use the inhomogeneous model. Only use that if you don't have a clear interface between liquid and gas. But if you are using surface tension (which you have to be using if you are modelling capilliary flow) then you should have a clear interface. In other words you should be using the homogeneous model.

I was trying to say you should not use the coupled VF solver. This was introduced in V11 with much fanfare for free surface flows but I have found it does not conserve VF. I have been working with the developers to fix this in V12 and it looks like it will be fixed. But for the time being in V11 if you want good conservation of VF you need to use the segregated VF solver (which is the default option - unless you have explicitly asked for the Coupled VF solver you are running the segregated one).

Glenn Horrocks

Hi Terje,

I think we exchanged a few emails about an year ago. Now I'm doing again some simulations of mould filling, and would like to ask you some questions:

When you employ the Inhomogeneous Model, which value do you use for the Drag Coefficient (Cd) between the phases, and why? Have you found any way to figure out what value to use? Could you obtain some good results with the Homogeneous Model?

What time step do you use? I have to use a very small time step, and if I reduce the injection velocity I cannot increase the time step ... This leads to very long CPU times

When I made some comparisons between CFX 5.6, 5.7 and 10, I found the CPU time necessary to run the simulations with CFX 5.7 and 10 was significantly (~60%, if I rember well) longer than with CFX 5.6. Have you experienced something similar? Or have noticed some other differences between simulations run with different versions of CFX?

And last Do you have some reports, papers, etc with your results? (I found this one: Multiscale simulations of the injection moulding of a diffractive optical element)

Thanks,

Rui

Hi,

Drag Coefficient: In my simulations I am not really interested in the air. It is just there because there needs to be two materials in CFX. I have been using the default value for the drag coefficient. At this value the air flow does not seem to influence the flow of polymer and is thus low enough for my use.

Capillary filling can be done using the homogenous model and so far I have not seen not much difference in the results. I have not looked deeply into this though. I used the inhomogenous model because of the problems I encountered using normal pressure driven filling.

Time step: in my experience setting a time step too short may cause as much problems as setting it too long. Using a too short timestep in multiphase simulations have led to unphysical eddies in some of my problems. I am usually using a constant timestep which I figure out by making a manual calculation of the Courant number, typically around 0.3-0.5. That is, the flow front spends 2-3 time steps passing through an element.

When it comes to presentations they are mostly collected here:

http://www.sintef.no/Projectweb/mpc/Publications/

Best regards Terje