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

(simple) Capillary Rise issue

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 28, 2016, 07:53
Default (simple) Capillary Rise issue
  #1
New Member
 
Join Date: Nov 2016
Posts: 5
Rep Power: 5
Simsey is on a distinguished road
Hey guys,

I'm new to CFX - CFD in general - and I'm trying to simulate a (simple) capillary rise problem of a capillar with a 0.1 mm radius which is dipped 2mm into a 4x4 mm tank. The capillar is 25mm high.

It keeps calculating without errors. My setup might not be the best as it takes ages to reach 0.01 to 0.05 s (a time where i expect to see a rise in the capillar). I followed the discussion in this thread but without a real success. From my point of view there is a lot of unneccessary detailed meshing at the dipped in capillar wall which is only important at the bottom, however, it should only be a "problem" in terms of simulation time, I guess.

I would be really thankful if someone could point me into the right direction.


Some details about the setup:

Analysis type
- Transient
- Total Time 1.5 s
- Adaptive Time steps
- First update Time 0s
- Update Freq. 1
- Initial Timestep 1e-8 s
- Num Coeff Loops
- Max Timestep 1 s
- Min Timestep 1e-8 s
- Target Max Loops 5
- Target Min Loops 3

Domain Tank
- Fluid Domain
- Water, Air (25C), Continuous Fluid
- Reference Pressure 1 atm
- Buoyat 0, -g, 0
- Ref. Dens. 1.2 (for air)

Fluid Models
- Homogenous Model, Free surface model option: Standard, Interface Compression level: 2
- Heat transfer: homogenous model, Option: none
- Turbulence model: Laminar (also tried SST)

Fluid Pair Models
- Surface Tension Coeff: 0.073 N m^-1
- Surface Tension Model: continuum surface force
- Primary fluid: Water
- Interphase transfer: free surface

Initialization
- u,v,w -> 0
- static pressure: 0 Pa
- Volume fractions: Air 0, Water 1

Domain Capillar
as above but volume fractions changed to => Air 1, Water 0 (initialization)

Domain Interface
- Connection of capillar inlet (bottom) + surface of tank under the inlet
- General Connection
- Mesh Connection: CGI

Boundary tank opening (surface on top of the tank & tank surface parallel to the dipped in capillar wall)
- Opening Pres. and Dirn, Relative Pressure: 0 Pa
- Flow Direction: Normal to Boundary Condition

Boundary tank wall (nothing special)

Boundary tank_symmetry (nothing special)

Boundary capillar_symmetry (nothing special)

Boundary capillar_wall
- adhesive: 20

Boundary capillar_opening (top)
- Opening Pres. and Dirn, Relative Pressure: 0 Pa
- Volume Fractions: Air 1, Water 0


Following the free surface tension tutorial (9), I am unsure if the Buoyat Ref. Density should be water or air. The statement in the help is "Always set Buoyancy Reference Density to the density of the least dense fluid in free surface calculations" and my buoyancy medium is water and not air? And thereby the primary fluid should also be set to water or air? or is this unrelated?

Furthermore, I'm not sure if it is okay to set 1 atm as ref. pressure and define 0 Pa for the opening on top of the capillar and at the initialization of both domains.

The picture "end" is similar to a run at 0.05s, unfortunately i did not take a screenshot last time. From my expectations the capillar should be initially flushed with water to be on the same level as the tank? I tried to set an initial level of 5 mm (1mm above the tank) by using an expression for the water but without success. For instance: vfwater = 5 [mm], and define water = vfwater and air = 1-vfwater.

Sorry maybe a bit too much information but often the devil lies in the detail.. Hopefully I didnt miss an important one.

Thanks in advance!

Best regards



edit: solver was run with double precision activated, added two more screenshots.
Attached Images
File Type: jpg geom.jpg (91.0 KB, 63 views)
File Type: jpg mesh.jpg (178.0 KB, 72 views)
File Type: jpg setup.jpg (84.3 KB, 52 views)
File Type: jpg momentum and mass.jpg (146.4 KB, 39 views)
File Type: png end.png (84.1 KB, 40 views)

Last edited by Simsey; December 1, 2016 at 08:29.
Simsey is offline   Reply With Quote

Old   November 28, 2016, 16:04
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,349
Rep Power: 126
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Thanks for the detailed post. The only problem with your post is I don't know exactly what your question is - can you state what your question is?

Assuming the model is running but the results are inaccurate:

Have you checked that you have converged tightly enough?
Have you checked that your mesh is fine enough?

If you investigate the mesh convergence issue you will find that this sort of simulation does not converge with mesh refinement. This is a fundamental inconsistency with the Navier Stokes equations, the no slip boundary condition and moving contact lines at walls (in short: how does a contact line move along a wall when the wall is a no slip condition?). Clearly the contact line does move along the wall but the equations CFX is solving does not allow it. Numerical solvers "fudge" their way around this by smearing the effect across the elements at the wall, but this has the effect that it is mesh dependent and does not converge with mesh refinement.
ghorrocks is offline   Reply With Quote

Old   November 29, 2016, 15:22
Default
  #3
New Member
 
Join Date: Nov 2016
Posts: 5
Rep Power: 5
Simsey is on a distinguished road
Hey, thanks for your reply. I experimented a bit with a different geometry and mesh and could finally observe some kind of a rise in the water level.

However, I am a bit confused that I only observe a rise when I place the capillar on top of the tank instead of dipping it 2mm into it. The mesh is more simple in this case which might explain why it's not a perfect parabolic shape but is in contrast to the above post, where the mesh was much finer.

By tightly enough, I guess you mean 10e-6, so the answer should be no, in this case. When the capillar was dipped into the tank it was in the area of 10e-4 to 10e-5.

Basically my questions are:

1) Are the assumptions I made in my first post correct?
2) Why is the water level asymmetric? (screenshot)
3) Is the way how I model the case (2 domains) the wrong approach?
4) Why is the water not increasing when the capillar is dipped into the tank? I expected the water level to rise immediately to the same level as the water next to it. Or is this only mesh related?
5) Should I use expressions (e.g. initial water level, hydrostatic pressure) - I thought it will be fine to add them later, to refine the results as soon as I have acceptable results..

Thank you for your explanation on the moving contact angle! I really appreciate your help!

Best regards
Attached Images
File Type: jpg contour plot water vf.jpg (79.4 KB, 40 views)
File Type: png mesh.PNG (34.6 KB, 32 views)
File Type: jpg momentum and mass.jpg (113.7 KB, 28 views)
File Type: jpg volume friction.jpg (137.4 KB, 28 views)
Simsey is offline   Reply With Quote

Old   November 29, 2016, 17:28
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,349
Rep Power: 126
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
I am a bit confused that I only observe a rise when I place the capillar on top of the tank instead of dipping it 2mm into it.
This is strange, it suggests something is wrong in your setup.

Convergence criteria: You need to establish that you are converging tightly enough that you have converged in your case. Do a simulation converging to 1e-4, then 1e-5 then 1e-6. You want to use the loosest criteria which gives you a converged result.

Quote:
Are the assumptions I made in my first post correct?
What assumptions? You made many, many assumptions and I do not know which ones you are referring to.

Quote:
Why is the water level asymmetric? (screenshot)
Your mesh in the water reservior looks way too coarse. I think this causes it.

Quote:
Is the way how I model the case (2 domains) the wrong approach?
It is not wrong but it is not necessary and leads to problems (eg previous question). Just put it all in one domain.

Quote:
Why is the water not increasing when the capillar is dipped into the tank? I expected the water level to rise immediately to the same level as the water next to it. Or is this only mesh related?
I don't know, it could be many things.

Regarding mesh: To get good surface tension modelling you need extremely high quality mesh. The mesh quality guidelines in the documentation and pre-processor are nowhere near adequate for surface tension modelling. Anywhere the free surface will travel over will need a high quality hex mesh, with an aspect ratio no worse than 1.2. So you cannot use tet mesh + inflation in the capillar.
Simsey likes this.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Simple channel case using cyclicAMI will not converge cbcoutinho OpenFOAM Running, Solving & CFD 3 August 4, 2015 12:28
The correction on pressure equation of SIMPLE algorithm in MRFSimpleFOAM solver renyun0511 OpenFOAM Running, Solving & CFD 0 November 10, 2010 01:47
How to add correcting pressure equation in SIMPLE of MRFSimpleFOAM? renyun0511 OpenFOAM Programming & Development 0 November 4, 2010 01:38
compressible SIMPLE method fakor Main CFD Forum 1 August 30, 2010 11:21
temperature rise due to viscous dissipation Marek Main CFD Forum 6 December 30, 2004 16:24


All times are GMT -4. The time now is 03:48.