CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Axisymmetric Multiphase Model (VOF)

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

Like Tree1Likes
  • 1 Post By ping

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 29, 2020, 12:05
Default Axisymmetric Multiphase Model (VOF)
  #1
New Member
 
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 3
CFD2D! is on a distinguished road
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 N-1) that at the beginning of the simulation my wire is partly covered with liquid and the rest is automatically lust (N-1). 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 axis-symmetric model around the x-axis, 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!
CFD2D! is offline   Reply With Quote

Old   March 30, 2020, 06:42
Default News
  #2
New Member
 
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 3
CFD2D! is on a distinguished road
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 set-up 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
Attached Images
File Type: png bild2.PNG (107.8 KB, 24 views)
File Type: png bild.PNG (64.0 KB, 14 views)
File Type: png picture1.PNG (33.9 KB, 18 views)
CFD2D! is offline   Reply With Quote

Old   April 2, 2020, 04:04
Default
  #3
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 555
Rep Power: 17
ping is on a distinguished road
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
ping is offline   Reply With Quote

Old   April 2, 2020, 06:07
Default
  #4
New Member
 
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 3
CFD2D! is on a distinguished road
Quote:
Originally Posted by ping View Post
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
The mesh is fine so far. I have 208000 cells and trim cell. 0.125mm axial and 0.03mm radial size. The set up looks a bit different than in the one picture, because they worked with Fluent. In Fluent you can freely define a rotation axis. In Star CCM+ this must be on the x axis.

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
CFD2D! is offline   Reply With Quote

Old   April 2, 2020, 06:41
Default
  #5
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 555
Rep Power: 17
ping is on a distinguished road
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
ping is offline   Reply With Quote

Old   April 2, 2020, 06:51
Default
  #6
New Member
 
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 3
CFD2D! is on a distinguished road
Quote:
Originally Posted by ping View Post
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
it is only different because they used Fluent. And they used a Inlet air with 0m/s but i think than i will get Problems with the mass balance.

how i can get the bead radius?
CFD2D! is offline   Reply With Quote

Old   April 11, 2020, 07:12
Default
  #7
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 555
Rep Power: 17
ping is on a distinguished road
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: Pre-Processing > Meshing > Two Dimensional and Axisymmetric Meshes > Creating a Two-Dimensional Mesh
CFD2D! likes this.
ping is offline   Reply With Quote

Old   April 21, 2020, 09:23
Default
  #8
New Member
 
Marten
Join Date: Mar 2020
Posts: 5
Rep Power: 3
CFD2D! is on a distinguished road
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 x-axis and is defined as the rotation axis. Otherwise you don't calculate the wavelike drop shape but only a flow down the wall.

Greeting
Attached Images
File Type: png Picture 1.PNG (26.6 KB, 9 views)
File Type: jpg Picture 2.jpg (128.1 KB, 9 views)
CFD2D! is offline   Reply With Quote

Reply

Tags
eulerian multiphase, gravity, multi-phase flow, tension force, vof

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
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 STAR-CCM+ 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


All times are GMT -4. The time now is 02:20.