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

Patching Second Phase Region in Fluent V13 VOF Model

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

Like Tree23Likes
  • 2 Post By sda
  • 8 Post By ElanMorin
  • 11 Post By ghost82
  • 1 Post By ghost82
  • 1 Post By thermal energy

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 14, 2011, 19:39
Default Patching Second Phase Region in Fluent V13 VOF Model
  #1
sda
New Member
 
Join Date: Apr 2010
Posts: 16
Rep Power: 15
sda is on a distinguished road
Hello Fellow CFD Users,

I am trying to set up a VOF model with air and water in Fluent V13. Does anybody know how to use the patch function to designate the region occupied by the water phase?

Step by step please.

If you have a worked example that would be ideal.


Thanks for your help.

SDA
nasser and vavnoon like this.
sda is offline   Reply With Quote

Old   March 16, 2011, 08:38
Default
  #2
New Member
 
Join Date: Mar 2011
Posts: 3
Rep Power: 14
ElanMorin is on a distinguished road
Hi,

I have a method of doing this that works (though whether it's the best way I don't know) but is first completed using gambit (or your meshing program).

In Gambit:

-Make a separate face or volume of the area that you want to patch.
-In the boundary conditions, name each separate volume (something like iniAir as the initally air section and iniWater as the initally water section).
-The lines or faces between these areas can be set in the boundary conditions as "Interior" meaning it is treated as not being there (alternatively you can just not include it as a boundary condition and then it will be ignored).
-Do all the other boundary conditions etc. as normal and export the msh.

In Fluent.

-Do everything you need to do with setting up the model that you would need to do (this step comes after initilizing the model).
-Once the model is initialized.
-> Solve -> Initialize -> Patch
---Change the variable to Volume Fraction and set the drop down box to water.
---Set the value to 1.
---and the Zone to Patch as iniWater (or what you named the area you want as water).
-click PATCH

You can then check that the zone is patched by checking Contours -> Phases -> Display and you should see the field you want.

Hope this helps

Elan
ElanMorin is offline   Reply With Quote

Old   June 17, 2011, 18:38
Question Vof
  #3
New Member
 
Monty
Join Date: May 2011
Posts: 11
Rep Power: 14
monty_p20 is on a distinguished road
Hello all,

I need help regarding water droplet simulation on surface and in rectangular crosection pipe. Inlet is air.

Will you please help me in this case.

Thanks in advance.
monty_p20 is offline   Reply With Quote

Old   March 15, 2012, 11:49
Default
  #4
New Member
 
Join Date: Nov 2010
Posts: 10
Rep Power: 15
haka is on a distinguished road
Hi elan,
I did the same steps as you mentioned but in ansys mesh not gambit.
My problem is 2d axisymmetric when i name slected the faces for initial air and intial water and import the mesh to fluent i get the error (draw symmetries invalid thread).
If you could give any advice it will be nice.
haka is offline   Reply With Quote

Old   March 15, 2012, 12:17
Default
  #5
Senior Member
 
ghost82's Avatar
 
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26
ghost82 will become famous soon enough
It is also possible to patch a region directly into fluent, without create a zone in gambit or other prepprocessors: clik adapt->region, give min and max x and min and max y to identify a rectangular zone (shape hex), then click mark.
Then go to pach and choose as region something like Hexahedron in the lower window at right (http://hpce.iitm.ac.in/website/Manua...tg/img2098.gif) and click patch.

https://www.sharcnet.ca/Software/Flu...g/node1381.htm


Daniele
Blue, rgd, blgypeng and 8 others like this.
ghost82 is offline   Reply With Quote

Old   March 15, 2012, 12:22
Default
  #6
New Member
 
Join Date: Nov 2010
Posts: 10
Rep Power: 15
haka is on a distinguished road
Thanks for the quick reply,So in the solution initialization should i give any water volume fraction value or leave the default value(o) and initialize all zone and patch as you mention above. i should patch the water zone right?

my primary phase is air and sec phase is water.
haka is offline   Reply With Quote

Old   March 15, 2012, 12:28
Default
  #7
Senior Member
 
ghost82's Avatar
 
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26
ghost82 will become famous soon enough
Quote:
Originally Posted by haka View Post
Thanks for the quick reply,So in the solution initialization should i give any water volume fraction value or leave the default value(o) and initialize all zone and patch as you mention above. i should patch the water zone right?

my primary phase is air and sec phase is water.
haka I see your sketch in the other thread: it depends what you want to do;
1- you can patch only the convergent zone already with water (yes you patch the secondary phase, the rest will be primary phase) or
2- you can have your domain filled all with air and your simulation will start from this point and water will enter first the convergent zone.

Daniele
ghost82 is offline   Reply With Quote

Old   March 15, 2012, 12:58
Default
  #8
New Member
 
Join Date: Nov 2010
Posts: 10
Rep Power: 15
haka is on a distinguished road
Thank you again for the reply Daniele,
ok im doin the first one which nozzle filed with water, i patched as you mentioned waiting for the simulation to end.

if i want to do the 2nd one you mention , should i create a small convergent zone through adapt region (mark) or should i patch the face (nozzle inlet edge) like water start from the line .
haka is offline   Reply With Quote

Old   March 15, 2012, 23:26
Smile Patch for complex geometry
  #9
New Member
 
Nguyen
Join Date: Dec 2010
Posts: 21
Rep Power: 15
tringuyenttt is on a distinguished road
Dear alls,
I want to patch for complex geometry (such as triangle, cell, elliptic,...) but I can not how to create them, anyone know this, please help me or give me a tip. Thanks
tringuyenttt is offline   Reply With Quote

Old   March 29, 2012, 12:52
Unhappy tracking water surface in vof at wave tank
  #10
New Member
 
rz
Join Date: Mar 2012
Posts: 25
Rep Power: 0
rezacfd1361 is on a distinguished road
what s the meaning of selecting sum in "define surface monitor" for "Phrases" , "volume fraction" . I have a 2 phase domain, primary phase is air and secondary phase is water. I am going to track surface changes for water, in internet i read that I have to select sum when i intoduce monitors/surface/surface monitors/define surface monitor.
my case is a Neumerical Wave Tank.
please help me.
rezacfd1361 is offline   Reply With Quote

Old   June 12, 2012, 08:47
Default
  #11
Member
 
shuai_manlou's Avatar
 
CAO Liushuai
Join Date: Apr 2012
Posts: 30
Rep Power: 13
shuai_manlou is on a distinguished road
Hello Daniele, I need your help, I am wondering is there any difference between the solutions when I set the primary phase to air and the second phase to water, and on the other hand, set the primary phase to water and second phase to air ?

thanks a lot ~
shuai_manlou is offline   Reply With Quote

Old   June 12, 2012, 09:17
Default
  #12
Senior Member
 
ghost82's Avatar
 
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26
ghost82 will become famous soon enough
Hi,
you have to set the primary phase as the continuous phase and secondary phase as the disperse phase; this is how I setup my problems.

Daniele
soheil_r7 likes this.
ghost82 is offline   Reply With Quote

Old   November 13, 2013, 14:03
Default
  #13
New Member
 
Dimitris Romanas
Join Date: Sep 2013
Posts: 29
Rep Power: 12
Volumeoffluid is on a distinguished road
Hi all,
in my problem i have two cell regions(one with air, other with water) sharing internal boundaries and i try to use VOF in fluent. What shall i define this internal line???as moving wall?as interface??
thank you in advance!
Volumeoffluid is offline   Reply With Quote

Old   March 14, 2014, 12:34
Default
  #14
Member
 
Join Date: Jan 2014
Location: Turkey
Posts: 37
Rep Power: 12
thermal energy is on a distinguished road
Hello dear friends,

I try to simulate melting process using VOF model. Pcm is solid phase initialy. Upper part of the solid there is air. They do not mix eachother. Natural convection is active. My primary phase air, secondary phase is pcm (phase change material). I have some questions to be sure about my model.

First, I do not define interface between air and pcm. Mean, There are 3 cell zone: air, fin ,pcm but I do not create name selection for this interface in meshing. Is it ok?

Initial condition of Wholesystem temperature is 293K, but air temp is 300K. how to set air temp ?

For cell zone condition, all cell zone (air, pcm, fin ) show mixture. Also for example, if I change pcm to phase2, all of cell zone change to phase 2

Only for secondary phase (pcm), I patch within fluent by adapt-region-mark then patch. Ok? Value of volume fraction should be 1 or 0 while patching?? I am confused. Initialy pcm is solid.

For initial values phase-2 volume fraction is 0. Ok?

I did some iteration for a short time to check model. For results, in graphics-countors I can not see total temperature for phase 1 and 2 only entalphy values I see for phase1 and 2.

Also countors of solidification/melting it shows only mixture. Mixture show what?

Any interaction should I use like surface tension etc.

Thanks for your help.
tamil29oct likes this.
thermal energy is offline   Reply With Quote

Old   July 23, 2014, 09:34
Default I'm wondering !!
  #15
New Member
 
zain
Join Date: Jun 2014
Posts: 4
Rep Power: 11
zain ali is on a distinguished road
hi
I'm confused in patch function in multiphase problems !
why do we have to patch the secondary phase in whatever zone ?
why don't we just specify the continuous phase in the domain and the dispersed phase as inlet and solve the case ?
will it work if we do so ?

boundary conditions

interior zone ==> water (continuous phase )
inlet ====> air (dispersed phase )
and solve the case !!
zain ali is offline   Reply With Quote

Old   February 15, 2017, 07:44
Default 3 different fluid at 3 different inlet
  #16
New Member
 
karthikeyan subramaniam
Join Date: Jan 2017
Posts: 6
Rep Power: 9
kkn1494 is on a distinguished road
good morning
am dealing with multiphase flow,
my domain consist of 3 different inlets,.

at 1st inlet water vapour which is pumped into mixing chamber ,
2nd milk is sucked by suction pressure which created in mixing chamber
3rd inlet which is open to atomspere

my doubt is how to set this boundry condition in fluent fr diff fluid??

how to define that seperate phase alone in inlet? i need to define milk alone in one inlet,,vapour alone in different inlet

thank you
kkn1494 is offline   Reply With Quote

Old   June 8, 2018, 10:54
Default
  #17
New Member
 
J Philip
Join Date: May 2018
Location: A place where no one uses fluent
Posts: 4
Rep Power: 7
Jacee is on a distinguished road
Hi Danielle you seem to be alot better than me at fluent, could you please answer a few qeustions on some multi phase modeling i am doing?
Jacee is offline   Reply With Quote

Old   June 10, 2018, 19:11
Default
  #18
New Member
 
Join Date: May 2018
Posts: 20
Rep Power: 7
Cyrus69 is on a distinguished road
Quote:
Originally Posted by tringuyenttt View Post
Dear alls,
I want to patch for complex geometry (such as triangle, cell, elliptic,...) but I can not how to create them, anyone know this, please help me or give me a tip. Thanks
hi
did u find an answer? if yes plz help me!
Cyrus69 is offline   Reply With Quote

Old   February 20, 2019, 13:51
Default
  #19
New Member
 
Archana
Join Date: Feb 2019
Posts: 1
Rep Power: 0
KEERTHANA is on a distinguished road
Quote:
Originally Posted by haka View Post
Hi elan,
I did the same steps as you mentioned but in ansys mesh not gambit.
My problem is 2d axisymmetric when i name slected the faces for initial air and intial water and import the mesh to fluent i get the error (draw symmetries invalid thread).
If you could give any advice it will be nice.
Hi haka..I m too doing a analysis of water spray nozzle on fluent. I have created a domain (rectangular shaped) surrounding the nozzle. During initialization , I patched phase 2( water ) volume fraction to be 0 . Does that mean throughout the analysis no water will be present or allowed inside the domain
KEERTHANA is offline   Reply With Quote

Old   July 3, 2022, 07:00
Default Error in liquid fraction during solidification of droplet
  #20
New Member
 
Uttar Pradesh
Join Date: Jun 2022
Posts: 2
Rep Power: 0
Sura is on a distinguished road
Document attached below

animation-2_0016.jpeg

animation-2_0017.jpeg

animation-2_0018.jpeg

I am trying the simulation for droplet solidification over substrates. The setup condition is given below.
droplet ejecting from the nozzle at 1000K and substrate gave to 300K. region 1 patched to molten metal volume fraction 1 and region 2 patched to air volume fraction 0.

Problem:
When the droplet reaches the substrate it starts solidifying and becoming blue in liquid fraction because the temperature comes to 300K. then somehow it merges with the air domain because that is also blue. I want to ask that is there any way that the air domain can be made colorless or transparent so the proper droplet shape can be seen.

Please Reply.
Thanks in Advance.
Sura 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
How to access only one phase in multiphase model by UDF wersoe Fluent UDF and Scheme Programming 1 January 4, 2017 08:11
Extract primary phase thread in VOF with 3 phases Eric FLUENT 2 July 7, 2011 03:22
Simplified VOF Model gulbenkian FLUENT 1 June 10, 2010 17:52
[Gmsh] Import gmsh msh to Foam adorean OpenFOAM Meshing & Mesh Conversion 24 April 27, 2005 09:19
Moving mesh or VOF? Giovanni Main CFD Forum 16 September 24, 2001 09:25


All times are GMT -4. The time now is 04:40.