# access velocity on xy-line in udf

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 April 20, 2010, 06:05 access velocity on xy-line in udf #1 New Member   harry Join Date: Sep 2009 Posts: 5 Rep Power: 9 Sponsored Links hi, i have created a grid and set it up for a vof calculation and created a horizontal line in fluent with the surface/line option. now i want to access the y-velocity on the line in the flow field and calculate the mean value for setting my bc depending on the results. this is my code: #include "udf.h" DEFINE_PROFILE(settau,thread,i) { Domain *d; Thread *t; face_t f,v; real v_sum, v_mean_wall=0, v_mean_xy=0; int count, zone_id_wall=THREAD_ID(thread), zone_id_xy=14; //i know the id of the line //velocity at xy line d=Get_Domain(1); t=Lookup_Thread(d,zone_id_xy); v_sum=0; count=1; begin_f_loop(v,t) { v_sum+=F_V(v,t); count++; } end_f_loop(v,t) v_mean_xy=v_sum/count; printf("mean y velocity at xy-line %i is: %g m/s with %d cells\n", zone_id_xy, v_mean_xy, count); //velocity at BC v_sum=0; count=1; begin_f_loop(f,thread) { v_sum+=F_V(f,thread); ++count; } end_f_loop(f,thread) v_mean_wall=v_sum/count; printf("mean y velocity at wall %i is: %g m/s with %d cells\n", zone_id_wall, v_mean_wall, count); //set bc depending on results if (v_mean_wall<=0 && v_mean_xy<=0) { begin_f_loop(f,thread) { F_PROFILE(f,thread,i)=-0.06; } end_f_loop(f,thread) printf("velocity is negative. set tau to -0.06\n"); } else { begin_f_loop(f,thread) { F_PROFILE(f,thread,i)=0.06; } end_f_loop(f,thread) printf("velocity is positive. set tau to 0.06\n"); } } i get an access violation because of the F_V(,t) command. i assume i can not access the y velocity on a xy-line like this with the face command. i searched the documentation, but i didn't found anything what kind of data type a line is and how i can access its values. maybe somebody knows? thanks a lot!
 Sponsored Links

 April 20, 2010, 18:48 #2 New Member   harry Join Date: Sep 2009 Posts: 5 Rep Power: 9 i found out that as far as i know it is not possible to access data with a face loop on a xy line like i tried to. it seems that a line of interest has to be defined in the mesh/grid generator (for example gambit), so it is getting its own fixed id that you can see in the BC panel. with this id you are able to access the "line" in udf with lookup_thread. but it is not working if the bc on this created line is set to "interior". in that case i still get access error.

 April 21, 2010, 05:55 #3 Senior Member   Max Join Date: Mar 2009 Posts: 133 Rep Power: 10 hello moe, a possible workaround would be to use solve/execute command to calculate the average and write it to a file at any intervals (e.g. every timestep). Just record a macro with the appropriate steps: report/surface integrals blablabla.... Then read the current value within your udf from the file and update your bc. cheers

 April 21, 2010, 15:36 #4 New Member   harry Join Date: Sep 2009 Posts: 5 Rep Power: 9 i have not tried the workaround, because it's not suitable in my case. but it might work. after having a conversation with some experts i found out that it is not possible to acces velocity at interior faces. http://my.fit.edu/itresources/manual...udf/node91.htm for interior faces you can only get the massflow rate and the pressure. other variables have to be computed by the user himself. the other properties you only can get on boundary lines. closed

 April 22, 2010, 07:13 #5 New Member   harry Join Date: Sep 2009 Posts: 5 Rep Power: 9 i found out that it is possible to get the velocities and other properties through the adjacent cells of the face. when the line is interior C0 and C1 exist, then the velocity can be accessed with F_C0(f,t)/F_C1(f,t) and THREAD_T0(t)/THREAD_T1(t). you can calculate an average value on different ways by yourself.

 October 23, 2010, 05:11 Hi. #6 New Member   Join Date: Aug 2010 Posts: 6 Rep Power: 9 Hello. I have a 2D (x,y) domain of size (0,0)(xmax,ymax) divided into a 50x50 grid. I want to find properties (e.g. y-velocity) of all cells at any given instant in the following manner. for (y=0,y=ymax,y++) { for(x=0,x=xmax,x++) { location[x][y]= ........ ? y_velocity[x][y]=........ ? } } It means that I fix y, then loop over all available x-cells to store values. Then increase y and repeat the process for x-cells. I need to store the values in arrays for further analysis or written to files. How do I add it to my UDF ? Thanx. NVD.

 Tags fluent, line, udf, velocity

 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 dm2747 FLUENT 0 April 17, 2009 01:29 erik_d OpenFOAM Bugs 13 September 13, 2008 21:45 derath OpenFOAM Mesh Utilities 44 September 4, 2008 05:09 Fahad Main CFD Forum 0 March 23, 2004 14:20 Martin J Main CFD Forum 8 August 14, 2003 23:19

 Sponsored Links

All times are GMT -4. The time now is 06:04.

 Contact Us - CFD Online - Top