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

bubble diameter definition in multi phase flow boiling simulation FLUENT

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

Like Tree2Likes
  • 2 Post By Abishek

Reply
 
LinkBack Thread Tools Display Modes
Old   September 25, 2011, 05:55
Default bubble diameter definition in multi phase flow boiling simulation FLUENT
  #1
New Member
 
Abishek
Join Date: Sep 2011
Posts: 8
Rep Power: 6
Abishek is on a distinguished road
hi.. i am using rpi wall boiling model with eulerian multiphase model in fluent to study subcooled flow boiling in a specific geometry. i am defining the bubble diameter in the domain according to a particular correlation with a udf and trying to call it under define -> phases -> secondary_phase -> bubble diameter.
the udf is as follows

#include "udf.h"
DEFINE_PROPERTY(db, c, ct)
{
real db; /* bubble diameter */
real temp_bulk = C_T(c, ct)-373.15; /* local variable */
if (temp_bulk > 13.5)
db = 0.00015;
else if (temp_bulk >= 0.0 && temp_bulk <= 13.5)
db = 0.0015 - 0.0001 * temp_bulk;
else
db = 0.0015;
return db;
}

When i interpret this udf, there are no errors, but i see a message that reads "db definition shadows previous definition"
I am unable to comprehend this message.
Also, i am trying to define this parameter db in terms of the bulk temperature at every cell (bulk temp = vof_1*temp_1 + vof_2*temp_2). I am not sure if the C_T(c,t) that i am using is the bulk temp at that cell of just the phase_2 temperature at that cell.

pls help. thanks
Abishek is offline   Reply With Quote

Old   January 15, 2013, 03:17
Default
  #2
New Member
 
libdemsci
Join Date: Jan 2013
Posts: 1
Rep Power: 0
libdemsci is on a distinguished road
i dont know if you have solved the problem.

what i want to say is the thread ct passed by fluent points to the secondary phase. you should take care of this if you want to get the temperature of the primary phase.
libdemsci is offline   Reply With Quote

Old   January 15, 2013, 05:43
Default
  #3
New Member
 
Abishek
Join Date: Sep 2011
Posts: 8
Rep Power: 6
Abishek is on a distinguished road
@libdemsci : thanks for the reply. that problem was solved a long time back.
I used a dummy DEFINE_ADJUST subroutine to access the values of liquid phase temperature and stored it into a C_UDMI, which I later used in the subroutine for bubble diameter.
there is correction in my post, i required liquid phase temperature and not bulk temperature.
Abishek is offline   Reply With Quote

Old   January 15, 2013, 08:18
Default Success using RPI Model
  #4
New Member
 
Ganapathy Iyer
Join Date: Mar 2009
Location: Pune, Maharashtra, India
Posts: 25
Rep Power: 9
Ganapathy is on a distinguished road
Dear Abhishek,
Were you successful using the RPI model ?
I was trying to use the model about 5 years ago, but the results that we got were not satisfactory.

Also CFX had RPI model as a beta feature, which they later removed because it wasnt a big success.

Can you share your experiences using this model ?
Ganapathy is offline   Reply With Quote

Old   January 15, 2013, 09:04
Default
  #5
New Member
 
Abishek
Join Date: Sep 2011
Posts: 8
Rep Power: 6
Abishek is on a distinguished road
haha. It now realize that I am not the only one killing himself to make sense of the results from the boiling simulations. RPI model is more or less the only well established computational framework so far for simulation of surface boiling. VOF can handle isolated bubble(s) nucleation problems (perhaps also bubble coalescence on surface) where bubbles are artificially induced into the domain. However, there are extreme limitations in terms of the usability of the various submodels of bubble departure diameter, frequency, nucleation site density etc for any particular application/ geometry or fluid when using the RPI model in an euler-euler framework. I have tried using CFX as well, but returned to fluent for several reasons involving ambiguity of inputs. I have now developed a UDF to include more appropriate submodels for the aforementioned parameters especially for flow boiling problems. The submodels are from more recent papers that are different from what is in the default fluent framework. However, there is still some ambiguity in using some characteristic temperature and velocity for the determination of some paraters such as bubble departure diameter, say, when using Unal's correlation. Fluent, as I believe is using a technique that seems to give some numbers in the reasonable range (that would keep the simulation stable), but the physics behind those numbers are highly questionable (for many applications, it would simply mean garbage). Nevertheless that is the, if we can say, only option available. Apparently the models seems to do a reasonable job (as several papers say) for tube boiling cases, but I am working on submerged jet impingement, where I am having a tough time getting trustable results. In gist, in my view, the limitations are purely due to the mechanistic/ experimental expressions for boiling model parameters being highly problem specific.
sduzjz and sandeep.siwach like this.
Abishek is offline   Reply With Quote

Old   January 15, 2013, 14:44
Default
  #6
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 417
Rep Power: 12
cfd seeker is on a distinguished road
Quote:
Originally Posted by Ganapathy View Post
Dear Abhishek,
Were you successful using the RPI model ?
I was trying to use the model about 5 years ago, but the results that we got were not satisfactory.

Also CFX had RPI model as a beta feature, which they later removed because it wasnt a big success.

Can you share your experiences using this model ?
I guess CFX still has RPI wall boiling model....isn't it?
cfd seeker is offline   Reply With Quote

Old   January 15, 2013, 23:55
Default
  #7
New Member
 
Abishek
Join Date: Sep 2011
Posts: 8
Rep Power: 6
Abishek is on a distinguished road
well, yes CFX still has RPI model in ansys 14.0. but its implementation is slightly different from that included in fluent.
Abishek is offline   Reply With Quote

Old   January 16, 2013, 00:26
Default RPI Boiling
  #8
New Member
 
Ganapathy Iyer
Join Date: Mar 2009
Location: Pune, Maharashtra, India
Posts: 25
Rep Power: 9
Ganapathy is on a distinguished road
I Started my CFD career with RPI wall Boiling Model in CFX 5.1
At that time Fluent RPI was not good. Even CFX RPI was in its Beta

We tried simulating Boiling in bent tubes in a high pressure boiler. The results were decent enough for an engineering analysis (i.e. qualitative).

But try as we may, we could never get to see the vapor lock or accumulation of vapor phase in bends which could match the experimental or other empirical correlations.
Ganapathy is offline   Reply With Quote

Old   January 17, 2013, 15:12
Default
  #9
New Member
 
Join Date: Sep 2010
Location: Windsor, Ontario
Posts: 17
Rep Power: 7
mehrdad_kbg is on a distinguished road
Hi Abishek,
Thank you very much for your precise description of the problem. I was wondering if it is possible to send me the udf you have developed. my email is: mehrdad_kbg@yahoo.com

Thank you very much.
mehrdad_kbg is offline   Reply With Quote

Old   March 2, 2013, 04:26
Default
  #10
New Member
 
zhongying ma
Join Date: Nov 2012
Location: Beijing
Posts: 5
Rep Power: 5
mzy012100 is on a distinguished road
Hi Abishek,
I was wondering if it is possible to send me the udf you have developed. my email is: mzy012100@163.com

Thank you very much.
mzy012100 is offline   Reply With Quote

Old   August 13, 2013, 15:10
Default
  #11
New Member
 
Louisiana
Join Date: May 2013
Posts: 8
Rep Power: 5
lbrumf2 is on a distinguished road
Hi Abishek,
Thank you very much for your precise description of the problem. I was wondering if it is possible to send me the udf you have developed. my email is: lbrumf2@gmail.com
Thank you very much.
lbrumf2 is offline   Reply With Quote

Old   February 3, 2016, 08:41
Default
  #12
New Member
 
Alireza
Join Date: Feb 2015
Posts: 2
Rep Power: 0
Alirezaqaderi is on a distinguished road
Hi Abishek,
Can I have your developed UDF?my email: alirezaqdr@gmail.com
Thank you.
Alirezaqaderi is offline   Reply With Quote

Reply

Tags
boiling, bubble diameter, fluent, rpi, udf

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
Three Phase simulation FLUENT (ASK) sincity FLUENT 0 July 21, 2011 03:05
(help) three phase simulation on fluent sincity FLUENT 0 July 20, 2011 00:19
Simulation of steam (CO2 and Water vapor mixture) flow through nozzle using Fluent. Jimmy FLUENT 0 March 2, 2011 13:30
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31
Simulation of Two Phase Fluid Flow Problem Using Fluent 5.0 Mohammad Al-Shannag Main CFD Forum 1 July 16, 1999 11:28


All times are GMT -4. The time now is 00:15.