UDF to measure Mass Flow Rate
 

Hi everyone,
I am trying to measure the mass flow rate through a pressure outlet using a UDF. I realise there are easier way to get the mass flow rate at the outlet, rather than using the UDF but this is to be incorperated into a larger UDF later (hopefully :o). I have attached the code below that i have writen. The UDF interpetes okay and runs, however the problem is this code is giving me the mass flow rate throughout the whole volume and not at the pressure outlet ID 12 as required. I believe the problem is to do with the line: Lookup_Thread(d, 12);

#include "udf.h"
DEFINE_EXECUTE_AT_END(measure_mass_flow)
{
Domain *d;
real flow=0.;
face_t f;
Thread *t;
t= Lookup_Thread(d, 12);
d = Get_Domain(1);

thread_loop_f(t,d)
{
begin_f_loop(f,t)
{
flow+=F_FLUX(f,t);
}
end_f_loop(f,t)
}
printf("MASS Flow Rate: %g\n",flow);
flow=0.;
}

Please can anyone point me in the right direction?

1) thread_loop_f(d,t) loops over all face threads in your domain and neglects your previous specification of t as the pointer to outlet. Skip this loop.
2) You have to retrieve *d before using it in Lookup_Thread: Switch corresponding lines 8 and 9

cheers

Thanks a million Coglione. That worked great!
Cheers

Continuing on from the above UDF. I am trying to measure the flow rate and pressure at a pressure outlet. The goal is to compare the measured mass flow rate to a set value and if diffferent adjust the pressure at the outlet until the mass flow rate reaches the desire value. Therefore i want to know what pressure is required to give me a desired flow rate. I am also using a pressure inlet. The code i ahve writen is shown below.

#include "udf.h"
real flow=0.;
real p=0;
DEFINE_EXECUTE_AT_END(funny)
{
Domain *d;
cell_t c;
face_t f;
Thread *t;
d = Get_Domain(1);
t= Lookup_Thread(d, 12);
begin_f_loop(f,t)
{
flow+=F_FLUX(f,t);
}
end_f_loop(f,t)
p=C_P(c,t);
printf("Static Pressure at outlet: %f\n",p);
printf("MASS Flow Rate: %f\n",flow);
}

DEFINE_PROFILE(pressure_out,t,i)
{
real set_point=1;
real pressure;
face_t f;

if (flow < set_point)

pressure=p-1;
else if (flow > set_point)
pressure=p+1;

else
pressure=p;
begin_f_loop(f,t)
{
F_PROFILE(f,t,i) = pressure;
}
end_f_loop(f,t)
printf("Adjusted pressure: %f\n",pressure);
flow = 0;
}

This UDF measure the correct pressure and mass flow rate, but the problem is that, no matter whether the flow rate is greater than or less than the set point, the pressure still reduces by 1. I believe this is something to do with the way the global variables are used but can manage to fix it.
Can anyone shed some light on this problem for me, please:confused:.

Thanks for the help.

I manage to solve the problem and write the code;)!

Hi Lynch,

I am trying to write a UDF too where in the boundary condition at one zone affects the BC at the other which is similar to yours.
Could you tell me how u resolved the problem? Did you set the global variables as STATIC or was there something else to be modified?

Hi Kartn
The problem with the previous code that I posted was in getting the value for the variable “flow” from the DEFINE_EXECUTE_AT_END section and using it in the DEFINE_PROFILE. The way it was set as a global variable was okay but what was happening was it was been set to zero after the DEFINE_EXECTUE_AT_END loop so the DEFINE_PROFILE function was seeing a value of flow=0. Sorry if what I am saying is hard to follow, but I have attached the working code below and maybe from comparing the two you will be able to understand.
The only real different is in introducing the flow_tot variable as the global variable instead of using the flow variable.

#include"udf.h"
real flow_tot;
real p ;

DEFINE_EXECUTE_AT_END(funny)
{
Domain *d;

real flow;
cell_t c;
Thread *t;
face_t f;
d = Get_Domain(1);
t= Lookup_Thread(d, 12);

begin_f_loop(f,t)
{
flow+=F_FLUX(f,t);
}
end_f_loop(f,t)
p = C_P(c,t);
printf("static pressure = %g\n", p);
printf("MASS Flow Rate: %g\n",flow);
flow_tot =flow;
flow=0.;
}

DEFINE_PROFILE(pressure_out,t,i)
{
real set_point = 1;
real pressure;
face_t f;




printf("MASS Flow Rate: %g\n",flow_tot);
if (flow_tot < set_point)

pressure = p - 1;

elseif (flow_tot > set_point)

pressure = p + 1;

else
pressure = p;



begin_f_loop(f,t)
{
F_PROFILE(f,t,i) = pressure;
}
end_f_loop(f,t)
printf("Adjusted pressure = %g\n", pressure);
}

Hope this helps!:)

Udf for applying transient mass flow rate
 

I am trying to figure out how to write a udf for applying a transient mass flow rate at the inlet. In my case study the mass flow rate varies with time from 0 to 40L/min and then comes down to zero in one cycle that ranges from 0 to 4 sec.

If anybody have a ready made udf, i wud be grateful if u could plz post it in this link or pass on through my email id.

I admit i am have a bad programming knowledge but since it is bit urgent, i have to seek ur opinion and help without having to take the pain to learn it myself.

Plz do help

What I'm curious is how you can find out the ID=12 for your t? Can you please tell me? I need to do sort of the same thing.
Thanks

Hi aleisia,

The ID (=12 in this case) could be found from the FLUENT GUI in the "Boundary Conditions" section. Every boundary zone has its own ID.

Hi aleisia,

Yes like Kartn said i found the ID in the Boundary Conditions section of Fluent. Just highlight the zone you require and below the the list you will see the ID No. in box.
Best of Luck with the Work!:)

Thank you for your post, and I found it following your direction, and thanks Kartn too.

Actually I'm working on modelling an imperfect filter, say, there is a cuboid (four side walls being 'wall', one inlet and one outlet as 'interior')in a room with SO2-air gaseous mixture. I model the cuboid as an imperfect filter in the following way: I first got the mass flow rate of SO2 from the inlet surface of the cuboid, and multiply this mass flow rate with a factor (<1) and set it as the volumetric sink rate (kg/m^3/s), below is the code and some errors I found:

#include "udf.h"
#include "mem.h"
#include "unsteady.h"

#define inlet_ID 12;
#define filter_ID 2;

real source;
real tepflowrate;
real vol_tot;
real ti;
Thread *t;
Thread *thread;
face_t f;
cell_t c;


DEFINE_ADJUST(adjust, d)
{
#if !RP_HOST

int i=0;
/* real A[ND_ND]; */
/* real flux[ND_ND]; */
real NV_VEC(flux);
real NV_VEC(A); /* declaring vectors flux and A */
/* real source; */
real massflowrate=0.;
real vol=0.;
/* real ti = RP_Get_Real("flow-time"); */ /* ti = CURRENT_TIME;*/

/* Thread *t; */
thread=Lookup_Thread(d,filter_ID);
t=Lookup_Thread(d,inlet_ID);
/* defining the filter volume thread by specifying the Zone_ID*/
/* defining the inlet surface thread by specifying the Zone_ID*/

/* Send the ID value to all the nodes */
/* host_to_node_real_4(f, t, c, thread);Does nothing in serial, t is the thread of inlet surface, thread is the thread of the filter volume */

/*Start to calculate the mass flow rate through the inlet surface and store it in UDM*/
/* begin_f_loop(f,t) */
if PRINCIPAL_FACE_P(f,t) /* tests if the face is the principle face FOR COMPILED UDFs ONLY */
{
NV_D(flux, =, F_U(f,t), F_V(f,t), F_W(f,t)); /* defining flux in terms of velocity field */
NV_S(flux, *=, F_R(f,t)); /* multiplying density to get flux vector */
F_AREA(A,f,t); /* face normal vector returned from F_AREA */
massflowrate = F_YI(f,t,i)*NV_DOT(flux,A); /* dot product of the inlet surface flux and area vector, multiplied by the mass fraction of species i */
}
/* end_f_loop(f,t) */

# if RP_NODE /* Perform node synchronized actions here, Does nothing in Serial */
massflowrate = PRF_GRSUM1(massflowrate);
# endif /* RP_NODE */


begin_f_loop(f,t)
if PRINCIPAL_FACE_P(f,t) /* tests if the face is the principle face FOR COMPILED UDFs ONLY */
{
F_UDMI(f, t, 0)= massflowrate; /* YOU MAY NEED TO CHECK THE NODE AS THE SUMMED UP VALUE OF massflowrate IS DONE AT node0. */
}
end_f_loop(f,t)

/*Start to calculate the total volume of filter volume and store it in UDM */
begin_c_loop(c,thread)
{
vol += C_VOLUME(c,thread); /* get cell volume */
}
end_c_loop(c,thread)

#if RP_NODE /* Perform node synchronized actions here, Does nothing in Serial */
vol= PRF_GRSUM1(vol);
# endif /* RP_NODE */

begin_c_loop(c,thread)
{
C_UDMI(c, thread, 1)= vol; /* YOU MAY NEED TO CHECK THE NODE AS THE SUMMED UP VALUE OF massflowrate IS DONE AT node0. */
}
end_c_loop(c,thread)
#endif /* !RP_HOST */
}

DEFINE_SOURCE(cell_SO2mass_source, c, thread, dS, eqn)
{
#if !RP_HOST


/* face_t f; */
/* int i; */
/* real A[ND_ND]; */
/* real flux[ND_ND]; */
/* real NV_VEC(flux); */
/* real NV_VEC(A); */ /* declaring vectors flux and A */

/* Thread *thread=Lookup_Thread(d,filter_ID); */


Domain *d;

d=Get_Domain(1);
t=Lookup_Thread(d,inlet_ID);
ti=RP_Get_Real("flow-time"); /* ti = CURRENT_TIME;*/
/* Thread *thread; */

/* #endif */ /* !RP_HOST */

/* #if !RP_HOST */

tepflowrate= F_UDMI(f, t, 0);
vol_tot = C_UDMI(c, thread, 1);

#endif /* !RP_HOST */

/* Pass the node's SO2 mass flow rate and volume to the Host for calculating source */
node_to_host_real_2(tepflowrate, vol_tot); /* Does nothing in SERIAL */

#if !RP_NODE /* SERIAL or HOST */
source=-0.999989*tepflowrate/vol_tot;
dS[eqn]=0.0;
return source;
Message("Sink Rate in Filter %d is %f (kg/m^3/s)\n", filter_ID, source);
#endif /* !RP_NODE */

}

Deleted old libudf\win64\3d_host\libudf.dll
libudf\win64\3d_node\libudf.dll
1 file(s) copied.
(system "copy "c:\ANSYSI~1\v121\fluent"\fluent12.1.4\src\makefil e_nt.udf libudf\win64\3d_host\makefile")
1 file(s) copied.
(chdir "libudf")()
(chdir "win64\3d_host")()
# Generating ud_io1.h
udfsource1.c
..\..\src\udfsource1.c(121) : error C2143: syntax error : missing ')' before ';'
..\..\src\udfsource1.c(121) : error C2143: syntax error : missing ';' before ','
..\..\src\udfsource1.c(121) : error C2059: syntax error : ')'
(system "copy "c:\ANSYSI~1\v121\fluent"\fluent12.1.4\src\makefil e_nt.udf libudf\win64\3d_node\makefile")
1 file(s) copied.
(chdir "libudf")()
(chdir "win64\3d_node")()
# Generating ud_io1.h
udfsource1.c
..\..\src\udfsource1.c(33) : error C2143: syntax error : missing ')' before ';'
..\..\src\udfsource1.c(33) : error C2059: syntax error : ')'
..\..\src\udfsource1.c(34) : error C2143: syntax error : missing ')' before ';'
..\..\src\udfsource1.c(34) : error C2059: syntax error : ')'
..\..\src\udfsource1.c(101) : error C2143: syntax error : missing ')' before ';'
..\..\src\udfsource1.c(101) : error C2059: syntax error : ')'

Done.

The four errors are in red color, if convenient, can you please take a look at it? thanks!

Hi Kartn, thanks for your reply and I found it out.
BTW, if convenient, can you please check out my problem? I post it by replying to a.lynchy's post. thanks!

I think about it again, and found this in your code:
begin_f_loop(f,t)
{
flow+=F_FLUX(f,t);
}
end_f_loop(f,t)

Here the F_FLUX(f,t) is a vector, I believe, so what if you want to get the mass flow rate, instead of the flux, can I write:
begin_f_loop(f,t)
{
flow+=F_YI(f,t,i)*F_FLUX(f,t)*F_AREA(A,f,t);
}
end_f_loop(f,t)

or

real A[ND_ND], flux(ND_ND)
begin_f_loop(f,t)
{
flux=F_FLUX(f,t);
F_AREA(A,f,t);
mf=F_YI(f,t,i);
flow+=mf*NV_DOT(flux, A);
}
end_f_loop(f,t)

As I understand, F_YI(f,t,i), F_FLUX(f,t) and F_AREA(A,f,t) just get one patch of the surface 'f' corresponding to the thread 't', so the area 'A' is the area of that patch, that's why we need the begin_f_loop and end_f_loop, am I getting this right?

thanks!

Hi Aleisia,

F_FLUX(f,t) by itself outputs the mass flow rate entering or leaving a face in a cell. It is a scalar quantity and it outputs the result of the dot product of the mass flux vector and area normal vector.
So all u have to do in order to calculate the mass flow rate of a particular species is find the product of total flux of the mass flux vector and the mass fraction.

begin_f_loop(f,t)
{
flow+=F_FLUX(f,t)*F_YI(f,t);
}
end_f_loop(f,t)

Thanks a million Kartn!

So, if I have some fluid entering into a surface, F_FLUX should be a negative scalar, right?

I remembered I've seen it somewhere, the result we see from the GUI values are actually the opposite of the F_FLUX , because they have different definitions of the 'normal' direction.
What I mean, from GUI, the value should be positive, because the fluid is entering into the surface, so it should be positive, but according to the definition of F_FLUX, it should be negative. Am I getting this right?

Thanks!

Good morning everybody,

I was reading your post and I think I've the same problem as all of you. I'm analyzing journal bearings. The problems seams easy but i can't have the convergence if the "pressure-inlet" vs "pressure-outlet" are imposed. If I try to impose "mass flow inlet" vs "pressure-outlet" i can reach a good convergence. The problem is: I don't know the mass flow!!!! My idea is: impose a mass flow, calculate the total pressure (known data) and then recompute the mass flow at any iteration.

I've to write an UDF like yours:

1. Calculate the total average total pressure on the inlet and with an algorithm calculate the next mass flow (this is easy like a bisection algorithm will work sure, remember i had an aimed total pressure).

2. Input the new mass flow.

So the first UDF must be an DEFINE_EXECUTE_AT_END, to calculate for example "mass_flow", and the next will be an DEFINE_PROFILE.

My question is: how to calculate the average total pressure on a face (of course Ptot=Pstat+0.5*rho*v^2) but i don't know how to implement it as an average on the boundary.

when u do this:

begin_f_loop(f,t)
{
flow+=F_FLUX(f,t);
}
end_f_loop(f,t)

means that fluent is going to give u "flow" as the summatory of all the face fluxes of the boundary with the same ID?

thanks for your help!

Dear Adrian

Thanks For sharing your work. Could you please help me.
I want to calaculate the mass flow rate on a surface diffrent that the outlet boundary and then i want to modify the pressure at outlet according to that mass flow.
I dont have that surface as a boundary seprately. I just creat that surface as an isosurface in Fluent and I was calculataing the mass flow in GUI.

I appriciate your help.

Best
Mehdi

Hi Adrian,

I would like to read the massflow in outlet and save it in UDMI. I used similiar code to yours but it seems nothing happens. is it possible to save the outlet mass flow and use it as in inlet mass flow. thanks in advance!!!!!!

Hi ALL,

I want to calculate solid phase mass flow rate at outlet and I wrote following code to it but it only read primary phase even though I pointed secondary phase. is there any one to help me why?
thanks a lot!!
#include "udf.h"
DEFINE_EXECUTE_AT_END(measure_mass_flow)
{
real mass_flow;
real abs_v;
Domain *d=Get_Domain(2);
face_t f;
Thread *mixture_thread = Lookup_Thread(d,2);
Thread **pt = THREAD_SUB_THREADS(mixture_thread);
Thread *tp = pt[0];
Thread *ts = pt[1];

mass_flow=0.;
mp_thread_loop_f(tp,d,pt)
{
if( THREAD_ID(tp) == 4 )

{
begin_f_loop(f,tp)
{

mass_flow+=F_FLUX(f,tp);

}
end_f_loop(f,tp)
}



}
Message("mass_flow:%g/n",mass_flow);
}
thanks again..

UDF for keep water height constant at inlet for a VOF model
 

Hi, does anybody have UDF for keeping the water height constant at inlet for VOF ( 2 phase) model? Or can anyone can give an idea from where I can learn how to write UDF ?


I badly need of it. It will be very great if anyone can help me . Thanks a ton in advance.

If you show a specific picture, Maybe I can help you :)

I tried to use this UDF initially and modify according to my case. Prior to any modification, I got the following error after the first iteration on "DEFINE_EXECUTE_AT_END".

How can I fix this error?!!
Thanks.
PS: I interpret the UDF.

Hello everyone i am using the similar UDF to alter the inlet boundary condition of my simulation. Basically i am also calculating the mass flow rate at the outlet of my valve and using this flow rate to calculate the pressure drop in feed line. Can someone help to find out what is problem wit this UDF..


Following UDF i am using to modify the inlet pressure......
#include "udf.h"
FILE *fp;
real flow_tot;

DEFINE_EXECUTE_AT_END(pressure)
{
Domain *d;
float flow;
cell_t c;
Thread *t;
face_t f;
d = Get_Domain(1);
t= Lookup_Thread(d, 12);

begin_f_loop(f,t)
{
flow+=F_FLUX(f,t);
}
end_f_loop(f,t)

flow_tot =flow;
flow=0.;
}
DEFINE_PROFILE(inlet_pressure, thread, position)
{
face_t f;
float P_i=903063;/* 199625Pa steady state pressure drop in feed circuit*/
real t= CURRENT_TIME;/* steady state inlet pressure 703438Pa*/
/*float flow_t=0;*/
float Del_P=0;
fp = fopen("output.txt","a");
fprintf(fp,"MASS Flow Rate: %f kg/s \n",flow_tot);
fclose(fp);
Del_P=(0.79215*flow_tot*flow_tot);
begin_f_loop(f, thread)
{

F_PROFILE(f, thread, position)=P_i-Del_P;
}
end_f_loop(f, thread)
}

can someone tells why i am getting Pi=9 bar at t=0 when mass flow is max. this should be 7.0 bar (Pi-Delta_p) but at t=0 i am getting initial pressure as 9.0 bar........where is the problem????can anyone tell....

Delta_P in steady state is given by Del_P=(0.79215*flow_tot*flow_tot); hence in steady state flow rate is maximum hence Pi should be minimum but surface monitor will start reading from 9.0 bar

UDF for mass flow rate at a pressure outlet
 

Can someone find where is the mistake in following udf. It is always printing zero flow rate at all time steps while mass flow rate from surface monitor is coming total different....???


#include "udf.h"
FILE *fp;
real flow_tot=0.;
DEFINE_EXECUTE_AT_END(fun)
{
Domain *d;
real flow=0.;
cell_t c;
Thread *t;
face_t f;
d = Get_Domain(1);
t= Lookup_Thread(d, 12);

begin_f_loop(f,t)
{
flow+=F_FLUX(f,t);
}
end_f_loop(f,t)
printf("MASS Flow Rate is: %g kg/s \n",flow_tot);
flow_tot =flow;
flow=0.;
}

Hi Wasim_03,

Your latest question is easy: you are printing the value of "flow_tot" *before* you copy the value of "flow" into it -- it should be after.

I haven't looked in detail at your previous questions. I do know that commands involving writing to file (fopen(fp...) fprintf(fp...)) are dangerous in parallel. Much better to print to the Fluent window using Message(...), which has a similar syntax to printf(...).

You are presumably trying to print out the value of "flow_tot" because you are not sure whether the value calculated by one UDF will survive when the next UDF is called. This is a valid concern -- you probably want to declare "static real flow_tot=0.;".

I worry whether your intended linkage between flowrate and pressure will be stable -- you might want to apply some home-made under-relaxation. (If you do this, you should be aware that DEFINE_PROFILE is sometimes called many times per iteration, for reasons that are not clear to me.)

The other stability issue is that DEFINE_PROFILE will be called before DEFINE_EXECUTE_AT_END, so the first iteration might go mad.

Udf
 

Hi OBSCUREED....Thanks for your reply...

i am able to compiled and run this UDF, your concerned regarding initial time step i have well taken care when Define_profile is called and Execute_at_end is still on hold and to be called subsequently, at this time i have implemented if else logic to define the initial value flow rate to avoid the function go made and both function are working perfectly.......


Thanks and regards
Wasim

Hi, Kanarya,
i'm trying to build a circulating fluidized bed, and encourtered a problems like yours. can you plz give some suggestions?
thanks a million in advance

Hi
Is the mass flow rate that you tried to measure is an output of the simulation?

Hi a.lynchy
Is the mass flow rate that you tried to measure is an output of the simulation?

Hi Oula,

You seem to be replying to the original post -- this is confusing, because that post was answered completely by coglione in 2010. If you have your own question, it is probably better to start a new thread. (The content of a.lynchy's question was good, by the way, and worth emulating -- it included descriptions of the goal, the current progress, the problem and a possible route towards a solution.)

Good luck!
Ed