# bubble diameter definition in multi phase flow boiling simulation FLUENT

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

 September 25, 2011, 05:55 bubble diameter definition in multi phase flow boiling simulation FLUENT #1 New Member   Abishek Join Date: Sep 2011 Posts: 8 Rep Power: 7 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

 January 15, 2013, 03:17 #2 New Member   libdemsci Join Date: Jan 2013 Posts: 1 Rep Power: 0 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.

 January 15, 2013, 05:43 #3 New Member   Abishek Join Date: Sep 2011 Posts: 8 Rep Power: 7 @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.

 January 15, 2013, 08:18 Success using RPI Model #4 New Member   Ganapathy Iyer Join Date: Mar 2009 Location: Pune, Maharashtra, India Posts: 25 Rep Power: 9 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 ?

 January 15, 2013, 09:04 #5 New Member   Abishek Join Date: Sep 2011 Posts: 8 Rep Power: 7 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.

January 15, 2013, 14:44
#6
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 422
Rep Power: 12
Quote:
 Originally Posted by Ganapathy 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?

 January 15, 2013, 23:55 #7 New Member   Abishek Join Date: Sep 2011 Posts: 8 Rep Power: 7 well, yes CFX still has RPI model in ansys 14.0. but its implementation is slightly different from that included in fluent.

 January 16, 2013, 00:26 RPI Boiling #8 New Member   Ganapathy Iyer Join Date: Mar 2009 Location: Pune, Maharashtra, India Posts: 25 Rep Power: 9 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.

 January 17, 2013, 15:12 #9 New Member   Join Date: Sep 2010 Location: Windsor, Ontario Posts: 17 Rep Power: 8 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.

 March 2, 2013, 04:26 #10 New Member   zhongying ma Join Date: Nov 2012 Location: Beijing Posts: 5 Rep Power: 5 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.

 August 13, 2013, 15:10 #11 New Member   Louisiana Join Date: May 2013 Posts: 8 Rep Power: 5 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.

 February 3, 2016, 08:41 #12 New Member   Alireza Join Date: Feb 2015 Posts: 2 Rep Power: 0 Hi Abishek, Can I have your developed UDF?my email: alirezaqdr@gmail.com Thank you.

 Tags boiling, bubble diameter, fluent, rpi, udf

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post sincity FLUENT 0 July 21, 2011 03:05 sincity FLUENT 0 July 20, 2011 00:19 Jimmy FLUENT 0 March 2, 2011 13:30 ram Main CFD Forum 5 June 17, 2000 21:31 Mohammad Al-Shannag Main CFD Forum 1 July 16, 1999 11:28

All times are GMT -4. The time now is 00:34.