
[Sponsors] 
March 29, 2020, 12:05 
Axisymmetric Multiphase Model (VOF)

#1 
New Member
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 4 
Good afternoon,
I am new here in this forum. I hope that there is someone who can help me eventually. I simulate the flow of a liquid (oil) on a capillary surface.My model is 2D (axisimetric), Eulerian multiphase, VOF, laminar, Phase Interactions (surface tension force), Phase 1: Liquid (prime) Phase 2: Gas (Air, secondary). I am rebuilding a publication and have exactly the same domain (meshoptions, base size, number of cells). My problem: The system is under atmospheric pressure and there are 1 inlet (top) and 2 pressure outlets (one at the top next to the inlet and one at the bottom). The inlet is for the fluid and I have added a field function to the initial conditions in the physics: ((${RadialCoordinate} > 0.000475) && (${RadialCoordinate} < 0.001))? 0:1 This field function says for the liquid phase (composite N1) that at the beginning of the simulation my wire is partly covered with liquid and the rest is automatically lust (N1). This function is for the Volumefractions (Initial conditions). My Inlet from which only the liquid comes has a Volumefraction of 1natural and air is present in the system through the Initial Condition. But how do I define the volume fractions of both outlets? I get backflows all the time when I define the outlets, no matter how. No liquid should come out of the top of the outlet, but air can come out by displacement and air can come out of the bottom. Is there any physical explanation for this and maybe you can develop a field function for it. And of course I have taken gravity into account. Because I have an axissymmetric model around the xaxis, my gravity is [9.81,0.0] m/s. I have also included a piece of the capillary (imprint) and defined the capillary center as axis of rotation. Where is my error? And is there a possibility to display each phase in a different colour? Greeting CFD2D! 

March 30, 2020, 06:42 
News

#2 
New Member
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 4 
Hello,
I found something else in a publication that ran the exact same simulation with Ansys. I have added some pictures. 1. my mesh "picture1" 2. numerical setup from a puiblication "bild1" 3. numerical setup from another publication "bild2 Both have the same simulation. VOF, Surface Tension Force and and and, but in the 2nd publication he defined an inlet with v = 0 m/s (Air). Unfortunately I still have backflows with this setup. I said that the volume fraction at this inlet is 1 (Air) and at the outlet volume fraction [1,1]. Does anyone have any idea what my mistake is? Greetz 

April 2, 2020, 04:04 

#3 
Senior Member
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18 
your mesh image does not look like the geometry setup in the reference study so is it identical? and if not please upload a sketch of what you want to model with the required boundary conditions and dimensions so that the field function can be checked


April 2, 2020, 06:07 

#4  
New Member
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 4 
Quote:
My geometry: 0.3m length (capillary) 0.475mm radius capillary (the small solid part in my mesh. Capillary center is the rotation axis) 0.78mm inlet liquid (volume fraction 1) 1.50mm Pressure Outlet top (volume fraction 1 air) 2.28mm Pressure Outlet bottom (volume fraction 0.5:0.5) I extended the inlet of the liquid by 0.001m, as you can see in the picture, and the wall of the capillary (No Slip and the Surface Tension Force model). The other wall of the inlet is a slip wall. The outermost wall is a symmetry plane. The velocity of the inlet is given by a field function which is a sine function to simulate a wavelike motion. The initialization, that the capillary is wetted with a certain layer thickness of liquid at the start of the simulation works great. I had some problems with the simulation before, because I chose wrong boundary conditions. But now I would like to plot the radius of the drop running down the capillary at different points. Best over time. So I know that at a certain time the radius at this point takes on a certain value. I know that I have to create an isosurface with VOF = 0.5 and plan different sections. But where do I select the VOF = 0.5? and which field function do I use for the Isosurface? I also don't know how to plot this yet. My first attempt went wrong. Thank you 

April 2, 2020, 06:41 

#5 
Senior Member
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18 
sorry  I was not commenting on your mesh quality etc but on the geometry shown in that image  it is different to the one in the reference and thus my request for a sketch of your setup


April 2, 2020, 06:51 

#6  
New Member
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 4 
Quote:
how i can get the bead radius? 

April 11, 2020, 07:12 

#7 
Senior Member
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18 
you have not provided a requested sketch so i will answer your questions half blind
for your pressure outlets the volume fraction is to let the code know what to do for any reverse flow so in your case you set them to air the fact that you are getting reverse flow is quite common in some cases with pressure boundaries and it only takes a very small pressure change to create any flow and this is especially the case when there is no pressure drop across the domain with both at the same pressure. you could try running the case with the upper pressure bc being a wall and see if the flow stabilizes and then change it to pressure and carry on the solve. if even a forced flow velocity inlet of about the estimated flow rate of air and then swap to pressure as you say in you second posting and you cant get back flows at a velocity inlet so maybe you mean at the outlet which can still happen due to local flow features. a standard scalar scene displayer with the vof of water (or air) will show each phase in a different colour and if you dont like those colours you can create your our colour map in tools isosurface issue  use the volume fraction field or either water or air and then set 0.5 as one of the isosurface properties after selecting a single isosurface as its mode not sure what you mean by bead radius maybe drop size anyway if this is the case then you could create an xy plot with the isosurface as the input part and this would then have a dimension on the x and y axes to help in your mesh image there is a lump of fine mesh at the bottom left  why is this there since it looks nothing like you other diagrams and if used as part of the region will probably case problems you can have an axis boundary in any direction but i think you were limited by the way you chose to create a 2d mesh  eg read this help article on a better way than what you used which i think was extract from a 3d face: PreProcessing > Meshing > Two Dimensional and Axisymmetric Meshes > Creating a TwoDimensional Mesh 

April 21, 2020, 09:23 

#8 
New Member
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 4 
Hello,
so first of all, thank you very much for your answer. I'm a few steps ahead of you now. I have nice drops (see picture), but the drop course is irregular (see picture 2). It should be more uniform, because my inlet velocity is a field function with a sine function : Ux = U * (1+Fsin) Fsin = A*(2*pi*sin(f)) The course should be even. I think it is because I have wetted the capillary surface with liquid as initial conditions, but I have not given any velocity as initial conditions for the liquid on the capillary. I've done that with the isosurface. I have no more backflows because I have defined my Pressure Outlet at the bottom as normal outlet and my Pressure Outlet at the top as Velocity Inlet Gas (very low velocity). After consultation with the author, he told me that I have to define a velocity for my liquid initialized on the capillary surface in the physics, because otherwise the liquid will accumulate and backflows can occur. If I had to write a field function for the velocity (physics/initial condition) of the liquid, what do I have to consider? I've been sitting at the problem for a few hours now and nothing works :/. the field function of my inletvelocity is called "inlet velocity is the field function for the use of the wire: ((${RadialCoordinate} > 0.000475) && (${RadialCoordinate} < 0.0009))? 1:0 I want a field function that says that in this range of initialization the velocity = inlet velocity. do you have an idea? The lump of fine Mesh is a solid part. It is the wire radius. Its center is exactly on the xaxis and is defined as the rotation axis. Otherwise you don't calculate the wavelike drop shape but only a flow down the wall. Greeting 

Tags 
eulerian multiphase, gravity, multiphase flow, tension force, vof 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Which Multiphase Model Should be selected in Fluent for my below described simulation  oberstar  Fluent Multiphase  0  September 28, 2017 13:05 
How to simulate the eulerian multiphase model about particle  jhlee9622  STARCCM+  2  November 24, 2016 12:37 
VOF Multiphase can‘t get converget  yangpeisi  Fluent Multiphase  0  April 9, 2016 01:04 
New Phase Compressible Turbulence Model for multiphase system  vishal3  OpenFOAM Programming & Development  0  November 24, 2015 01:17 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 04:32 