CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Capillary forces at low contact angles

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 20, 2008, 04:35
Default Capillary forces at low contact angles
  #1
Terje
Guest
 
Posts: n/a
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

  Reply With Quote

Old   August 20, 2008, 21:21
Default Re: Capillary forces at low contact angles
  #2
Glenn Horrocks
Guest
 
Posts: n/a
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
  Reply With Quote

Old   August 21, 2008, 10:17
Default Re: Capillary forces at low contact angles
  #3
Terje
Guest
 
Posts: n/a
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
  Reply With Quote

Old   August 22, 2008, 00:35
Default Re: Capillary forces at low contact angles
  #4
Glenn Horrocks
Guest
 
Posts: n/a
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
  Reply With Quote

Old   August 31, 2008, 12:23
Default Re: Capillary forces at low contact angles
  #5
Rui
Guest
 
Posts: n/a
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

  Reply With Quote

Old   September 3, 2008, 04:21
Default Re: Capillary forces at low contact angles------We
  #6
Terje
Guest
 
Posts: n/a
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
  Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
help with UDF for contact angle based on contact line velocity gandesk Fluent UDF and Scheme Programming 14 October 29, 2012 14:58
About define different contact angles to each surface within one component herosimon FLOW-3D 3 September 28, 2010 22:12
Drag and Lift forces extremely low João Lourenço FLUENT 4 January 28, 2008 14:25
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12
Filling by capillary forces Jochen Main CFD Forum 0 November 4, 2002 05:00


All times are GMT -4. The time now is 19:04.