CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   bubble diameter definition in multi phase flow boiling simulation FLUENT (https://www.cfd-online.com/Forums/fluent/92778-bubble-diameter-definition-multi-phase-flow-boiling-simulation-fluent.html)

 Abishek September 25, 2011 05:55

bubble diameter definition in multi phase flow boiling simulation FLUENT

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

 libdemsci January 15, 2013 02:17

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.

 Abishek January 15, 2013 04:43

@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.

 Ganapathy January 15, 2013 07:18

Success using RPI Model

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 ?

 Abishek January 15, 2013 08:04

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.

 cfd seeker January 15, 2013 13:44

Quote:
 Originally Posted by Ganapathy (Post 401934) 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?

 Abishek January 15, 2013 22:55

well, yes CFX still has RPI model in ansys 14.0. but its implementation is slightly different from that included in fluent.

 Ganapathy January 15, 2013 23:26

RPI Boiling

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.

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.

 mzy012100 March 2, 2013 03:26

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.

 lbrumf2 August 13, 2013 15:10

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.

Hi Abishek,
Can I have your developed UDF?my email: alirezaqdr@gmail.com
Thank you.:(

 soumitra2102 October 25, 2018 23:06

Can I get to see the UDF you developed?

Quote:
 Originally Posted by Abishek (Post 401942) 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.

Can I get to refer the UDF model you developed?
I am learning multiphase boiling simulation with ANSYS CFX.
My email id is: soumitra2102@gmail.com

Thank You.

 mo30raincity July 1, 2019 12:12

Quote:
 Originally Posted by Abishek (Post 401906) @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.
would you put this subroutine udf here?

 All times are GMT -4. The time now is 12:04.