
[Sponsors] 
November 28, 2016, 07:53 
(simple) Capillary Rise issue

#1 
New Member
Join Date: Nov 2016
Posts: 5
Rep Power: 5 
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 1e8 s  Num Coeff Loops  Max Timestep 1 s  Min Timestep 1e8 s  Target Max Loops 5  Target Min Loops 3 Domain Tank  Fluid Domain  Water, Air (25°C), 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 = 1vfwater. 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. Last edited by Simsey; December 1, 2016 at 08:29. 

November 28, 2016, 16:04 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,349
Rep Power: 126 
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. 

November 29, 2016, 15:22 

#3 
New Member
Join Date: Nov 2016
Posts: 5
Rep Power: 5 
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 10e6, so the answer should be no, in this case. When the capillar was dipped into the tank it was in the area of 10e4 to 10e5. 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 

November 29, 2016, 17:28 

#4  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,349
Rep Power: 126 
Quote:
Convergence criteria: You need to establish that you are converging tightly enough that you have converged in your case. Do a simulation converging to 1e4, then 1e5 then 1e6. You want to use the loosest criteria which gives you a converged result. Quote:
Quote:
Quote:
Quote:
Regarding mesh: To get good surface tension modelling you need extremely high quality mesh. The mesh quality guidelines in the documentation and preprocessor 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. 

Thread Tools  Search this Thread 
Display Modes  


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 