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

Initialising VOF model

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

Like Tree1Likes
  • 1 Post By Tron

Reply
 
LinkBack Thread Tools Display Modes
Old   November 25, 2010, 06:20
Default Initialising VOF model
  #1
Ste
New Member
 
Join Date: Nov 2010
Posts: 2
Rep Power: 0
Ste is on a distinguished road
Hi, does anyone know how to initialise the VOF model in STAR-CCM+ so that I can specify a particular area of the grid to one phase, and have the rest as the other phase.

It's the analagous case of the "adapt -> region -> mark cells" and then "patch" commands in FLUENT. I've attached an image of how it looks in FLUENT if I wasn't clear enough.

Any help at all would be appreciated
Ste
Attached Images
File Type: jpg example.jpg (22.9 KB, 82 views)
Ste is offline   Reply With Quote

Old   November 26, 2010, 04:04
Default Initializing VOF
  #2
New Member
 
Christian Jungreuthmayer
Join Date: Mar 2009
Posts: 9
Rep Power: 8
Tron is on a distinguished road
Hi Ste,

You will get an "Initial Conditions" branch in the "Region"-tree. There you can specify pressure, temperature, velocity, ... and also volume fraction. Usually, I use field functions to initialize the volume fraction. There you can do all sort of tricks, e. g. specify areas using the "Position" field function. For example:
($$Position[0] < 0.04 && $$Position[1] > 0.05 && $$Position[1] < 3.05) ? 1.0 : 0.0

Christian
Attached Images
File Type: jpg init_vof_1.jpg (29.2 KB, 56 views)
File Type: jpg init_vof_2.jpg (29.3 KB, 52 views)
DrZee likes this.
Tron is offline   Reply With Quote

Old   October 11, 2011, 18:49
Question Slug flow Initial Boundary Conditions
  #3
New Member
 
Leonardo
Join Date: Oct 2011
Posts: 4
Rep Power: 5
leonard is on a distinguished road
Hi,

I actually have kind of the same problem since it's difficult even to have the stratified flow when running constant velocity fraction. How do you come up with the equation? Where can I get information in specifying the equation to define?

Leonardo
leonard is offline   Reply With Quote

Old   October 15, 2011, 08:33
Default
  #4
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Quote:
Originally Posted by leonard View Post
Where can I get information in specifying the equation to define?
Have a look in the field function programming reference, there you will find the needed information.
The equation is just an if-clause.
For example if the coordinate in X-direction of a vertice of a cell ($$position[0]) is smaller than 0.04, the result should be 1. If not, the result should be 0.
Define this as initialisation field function and every cell will get the volume fraction according to this if-clause. That's all.

The example from Tron is just a combination of several if-clauses for different directions.
abdul099 is offline   Reply With Quote

Old   October 15, 2011, 08:37
Default
  #5
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
For complicated shapes it might be worth to create a cell set as you can pick every single cell you want to include to this set. When a cell set is created, there will be a new field function with the name of the cell set which is 1 for cells contained in the set and 0 for all other cells.
abdul099 is offline   Reply With Quote

Old   October 16, 2011, 18:55
Default Stratified flow 50% water 50 %air
  #6
New Member
 
Leonardo
Join Date: Oct 2011
Posts: 4
Rep Power: 5
leonard is on a distinguished road
Thank you very much for your help. I am getting the stratified flow. My model is a pipe with bends, so the idea is to have slug flow in the next sections of the pipe. I am running different cases to check if it forms. In case of any doubts I might ask for help. Thanks again.
leonard is offline   Reply With Quote

Old   October 16, 2011, 21:54
Default sine function user defined field function
  #7
New Member
 
Leonardo
Join Date: Oct 2011
Posts: 4
Rep Power: 5
leonard is on a distinguished road
Any of you know how to create a field function with the following condition? My CFD consultant told me to set that field function to be able to form slug flow.
if sin(wt)) >0; 1:0
I tried to set it first similar to the menu: (sin($x)>0)?1:0), but I still need to define the x, which in this case would be wt.
As you know w=2pif or 2pi/T, but how can I define this as a field function?

Thank you
leonard is offline   Reply With Quote

Old   October 20, 2011, 08:14
Default
  #8
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
(sin(omega*$Time)>0)?1:0)

Omega is a constant value and can here be given directly as a number.
abdul099 is offline   Reply With Quote

Old   October 24, 2011, 18:36
Default
  #9
New Member
 
Leonardo
Join Date: Oct 2011
Posts: 4
Rep Power: 5
leonard is on a distinguished road
Thanks for your help. It was really helpful.
leonard is offline   Reply With Quote

Old   October 24, 2011, 23:24
Default VOF wave
  #10
New Member
 
yanmei
Join Date: May 2011
Posts: 4
Rep Power: 6
ymz_0308 is on a distinguished road
Hi, need helps. I am seting the VOF wave in a flume, but i don't know why the result isn't correct. It should be regular wave propagation.
The wave should propagate from the left side to the right.

please see the attachment,
any one knows, and tell me why. Thanks.
Attached Images
File Type: jpg star_ccm.jpg (68.8 KB, 37 views)
ymz_0308 is offline   Reply With Quote

Reply

Tags
initialization, initiallisation, regions, slug flow, vof

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
VOF Model or Mixture Model mems21 FLUENT 2 March 9, 2010 11:37
HELP! UDF sinusoidal wave, VOF model, porous face! A8anato_psofimi FLUENT 2 November 10, 2009 15:42
A Problem with setting the time step in VOF model Le FLUENT 2 July 20, 2006 22:00
free surface of VOF and melting model? wanghong FLUENT 3 March 13, 2006 10:57
help needed for vof model yan FLUENT 3 December 16, 2005 02:17


All times are GMT -4. The time now is 04:11.