
[Sponsors] 
November 7, 2008, 04:31 
Parallel UDF problem

#1 
Guest
Posts: n/a

Hi,
Im having a couple of problems with running a UDF in parallel. When I compile the UDF on 2 processors, the library's are built and loaded but the simulation does not start. I receive a couple of warning signs during the build. In the host build: modified_drag.c: In function `modified_drag_EMMS': modified_drag.c:5: warning: 'k_g_s' might be used uninitialized in this function In the node build: modified_drag.c: In function `modified_drag_EMMS': modified_drag.c:80: warning: control reaches end of nonvoid function modified_drag.c:10: warning: 'w' might be used uninitialized in this function modified_drag.c:10: warning: 'cd' might be used uninitialized in this function Firstly, I have initialised 'k_g_s', 'w' and 'cd' which confused me a bit and secondly I thought the 'warning: control reaches end of nonvoid function' might be why the simulation seems to stop before producing the first line of iteration. The UDF is given as follows: #include "udf.h" DEFINE_EXCHANGE_PROPERTY(modified_drag_EMMS,cell,m ix_thread,s_col,f_col) { real k_g_s; #if !RP_HOST Thread *thread_g, *thread_s; real x_vel_g, x_vel_s, y_vel_g, y_vel_s, abs_v, slip_x, slip_y, rho_g, mu_g, Re, vf_g, vf_s, dp, w, cd; /* find the threads for the gas (primary) */ /* and solids (secondary phases) */ thread_g = THREAD_SUB_THREAD(mix_thread, s_col); /* gas phase */ thread_s = THREAD_SUB_THREAD(mix_thread, f_col); /* solid phase*/ /* find phase velocities and properties*/ x_vel_g = C_U(cell, thread_g); y_vel_g = C_V(cell, thread_g); x_vel_s = C_U(cell, thread_s); y_vel_s = C_V(cell, thread_s); slip_x = x_vel_g  x_vel_s; /* velocity slip in the x direction */ slip_y = y_vel_g  y_vel_s; /* velocity slip in the y direction */ rho_g = C_R(cell, thread_g); /* gas density */ mu_g = C_MU_L(cell, thread_g); /* viscosity of gas */ dp = C_PHASE_DIAMETER(cell, thread_s); /* particle diameter */ vf_g = C_VOF(cell, thread_g); /* gas volume fraction */ vf_s = C_VOF(cell, thread_s); /* solid volume fraction */ /* Absolute slip velocity */ abs_v = sqrt(slip_x*slip_x + slip_y*slip_y); /* Reynold's number */ Re = vf_g*rho_g*abs_v*dp/mu_g; /* Reynolds conditions */ if (Re < 960) cd = (24./(vf_g*Re))*(1+0.15*pow(vf_g*Re,0.687)); if (Re > 960) cd = 0.44; /* compute drag coefficient for dilute region */ if (0.74 < vf_g <= 0.82) w = 0.1680+(0.0679/(4*pow(vf_g0.7463,2)+0.0044)); if (0.82 < vf_g <= 0.97) w = 0.8601+(0.0823/(4*pow(vf_g0.7789,2)+0.0040)); if (0.97 < vf_g) w = 31.8295+32.9895*vf_g; k_g_s = 0.75*cd*((rho_g*vf_s*abs_v)/dp)*w; /* drag coefficient for the dense region */ if(vf_g <= 0.74) k_g_s = 150*((pow(vf_s,2)*mu_g)/(pow(vf_g,2)*pow(dp,2)))+1.75*((vf_s*rho_g*abs_v)/(vf_g*dp)); node_to_host_real_1(k_g_s); #endif #if !RP_NODE return k_g_s; #endif } I would really appreciate some guidence as to why the iterations are not starting as I am new to all this. Thanks in advance, Lindsay 

June 9, 2016, 14:16 

#2  
Member
xin
Join Date: Dec 2013
Posts: 33
Rep Power: 12 
I have the same problem
Quote:


June 10, 2016, 10:08 

#3 
Senior Member
Join Date: Nov 2013
Posts: 1,965
Rep Power: 26 
I'll assume you use the same code as Lindsay, because you did not supply any other information.
This code uses compiler directives. Look for this term in the Fluent manual. In the host build, RP_HOST is true and RP_NODE is false. So the code simplifies to: Code:
#include "udf.h" DEFINE_EXCHANGE_PROPERTY(modified_drag_EMMS,cell,m ix_thread,s_col,f_col) { real k_g_s; return k_g_s; } In the node build, RP_HOST is false and RP_NODE is true. So the code simplifies to: Code:
#include "udf.h" DEFINE_EXCHANGE_PROPERTY(modified_drag_EMMS,cell,m ix_thread,s_col,f_col) { real k_g_s; Thread *thread_g, *thread_s; real x_vel_g, x_vel_s, y_vel_g, y_vel_s, abs_v, slip_x, slip_y, rho_g, mu_g, Re, vf_g, vf_s, dp, w, cd; /* find the threads for the gas (primary) */ /* and solids (secondary phases) */ thread_g = THREAD_SUB_THREAD(mix_thread, s_col); /* gas phase */ thread_s = THREAD_SUB_THREAD(mix_thread, f_col); /* solid phase*/ /* find phase velocities and properties*/ x_vel_g = C_U(cell, thread_g); y_vel_g = C_V(cell, thread_g); x_vel_s = C_U(cell, thread_s); y_vel_s = C_V(cell, thread_s); slip_x = x_vel_g  x_vel_s; /* velocity slip in the x direction */ slip_y = y_vel_g  y_vel_s; /* velocity slip in the y direction */ rho_g = C_R(cell, thread_g); /* gas density */ mu_g = C_MU_L(cell, thread_g); /* viscosity of gas */ dp = C_PHASE_DIAMETER(cell, thread_s); /* particle diameter */ vf_g = C_VOF(cell, thread_g); /* gas volume fraction */ vf_s = C_VOF(cell, thread_s); /* solid volume fraction */ /* Absolute slip velocity */ abs_v = sqrt(slip_x*slip_x + slip_y*slip_y); /* Reynold's number */ Re = vf_g*rho_g*abs_v*dp/mu_g; /* Reynolds conditions */ if (Re < 960) cd = (24./(vf_g*Re))*(1+0.15*pow(vf_g*Re,0.687)); if (Re > 960) cd = 0.44; /* compute drag coefficient for dilute region */ if (0.74 < vf_g <= 0.82) w = 0.1680+(0.0679/(4*pow(vf_g0.7463,2)+0.0044)); if (0.82 < vf_g <= 0.97) w = 0.8601+(0.0823/(4*pow(vf_g0.7789,2)+0.0040)); if (0.97 < vf_g) w = 31.8295+32.9895*vf_g; k_g_s = 0.75*cd*((rho_g*vf_s*abs_v)/dp)*w; /* drag coefficient for the dense region */ if(vf_g <= 0.74) k_g_s = 150*((pow(vf_s,2)*mu_g)/(pow(vf_g,2)*pow(dp,2)))+1.75*((vf_s*rho_g*abs_v)/(vf_g*dp)); node_to_host_real_1(k_g_s); } Furthermore, you have a problem when Re is exactly 960: cd is undefined. And when vf is smaller than 0.74, w is undefined. I guess that your first problems can be solved by changing RP_NODE to RP_HOST. I don't really see why that one was used. And the other problems: define cd when Re is exactly 960, and define w when vf is smaller than 0.74. 

June 20, 2016, 09:19 

#4 
Member
xin
Join Date: Dec 2013
Posts: 33
Rep Power: 12 
Thank you very much!!
I have code like this, it is strange that before I didn't have any error, but now I have same problem as mentioned before. Code:
#include <stdio.h> #include<math.h> #include "udf.h" DEFINE_SOURCE(plasmasourcez,c,t,dS,eqn) { #if !RP_HOST double source; source=C_UDMI(c,t,1); dS[eqn] = 0; return source; #endif } 

June 20, 2016, 09:37 

#5 
Senior Member
Join Date: Nov 2013
Posts: 1,965
Rep Power: 26 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Parallel UDF Problem  Dimitris  Fluent UDF and Scheme Programming  7  September 20, 2013 01:51 
parallel problem  siyu  Siemens  6  March 6, 2009 23:38 
Problem in Parallel UDF  Giacomo de Renzi  FLUENT  12  June 18, 2008 12:19 
parallel problem  rui  Siemens  2  July 31, 2007 13:23 
parallel UDF problem  kerem  FLUENT  2  June 20, 2006 06:56 