CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > CONVERGE

Exporting data for a section or couple of points

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 23, 2016, 21:55
Default Exporting data for a section or couple of points
  #1
New Member
 
amrrhm
Join Date: May 2016
Posts: 20
Rep Power: 9
amrrhm is on a distinguished road
Hi,

I understand that using udf we can do loops on nodes and etc. Is there any way to loop only on nodes in a section (e.g. xy plane) or couple of nodes and export data (velocity, pressure, temperature, ...) for only those points.

Thanks
amrrhm is offline   Reply With Quote

Old   May 24, 2016, 06:46
Default
  #2
Senior Member
 
Tobias
Join Date: May 2016
Location: Germany
Posts: 264
Rep Power: 10
MFGT is on a distinguished road
Hi amrrhm,

as far as I know, you can evaluate these values with cutplanes via EnSight only.

However, it would be cool if UDF Monitor Point function would work in a similar way like embedding (sphere, box, plane, boundary, ...whatever) and directly receive averaged values for the defined volumens/surfaces, without extra compiling the .dll file. And adding extra variables via a tab.
MFGT is offline   Reply With Quote

Old   May 24, 2016, 08:13
Default
  #3
New Member
 
amrrhm
Join Date: May 2016
Posts: 20
Rep Power: 9
amrrhm is on a distinguished road
Hi MFGT,

It would be really time saving if we can get variables for just a number of selected nodes.
amrrhm is offline   Reply With Quote

Old   May 24, 2016, 10:05
Default
  #4
Member
 
alemoine's Avatar
 
Allie Le Moine
Join Date: Jan 2016
Location: Convergent Science, Madison WI
Posts: 39
Rep Power: 10
alemoine is on a distinguished road
Hello all,

If you are interested in only a couple of points throughout the computational domain then you can define UDF Monitor Points. The UDF Monitor Points allow you to set an (x,y,z) location as well as a radius.

If the radius is set to 0.0, CONVERGE will output the nearest cell-center information.

If the radius is greater than 0.0, CONVERGE will average over all of the cell-centers located within the sphere that is defined by the radius and (x,y,z) location.

If you are interested in looking at averaged information on a plane or any non-spherical shape, then as previously mentioned you will need to use Ensight.

Thank you,
__________________
Allie Le Moine
Research Engineer | Applications
CONVERGECFD
alemoine is offline   Reply With Quote

Old   May 24, 2016, 12:09
Default
  #5
New Member
 
amrrhm
Join Date: May 2016
Posts: 20
Rep Power: 9
amrrhm is on a distinguished road
Thanks alemoine,

Is just defining points in UDF Monitor Points is enough or I have to tell Converge to output the information for those points (e.g. in user_post.c). If the second case is true, how should I do that? I see the coordinates of the points at the end of the udf.in, but is there a function to get the cell number for those coordinates.

It would be very appreciated if you would give more details on this.

Thanks
amrrhm is offline   Reply With Quote

Old   May 24, 2016, 16:57
Default
  #6
Senior Member
 
Tobias
Join Date: May 2016
Location: Germany
Posts: 264
Rep Power: 10
MFGT is on a distinguished road
Quote:
Originally Posted by amrrhm View Post
Thanks alemoine,

Is just defining points in UDF Monitor Points is enough or I have to tell Converge to output the information for those points (e.g. in user_post.c). If the second case is true, how should I do that? I see the coordinates of the points at the end of the udf.in, but is there a function to get the cell number for those coordinates.

It would be very appreciated if you would give more details on this.

Thanks
Have a look in the UDF Manual.
After including the UDF monitor points in the case setup, you have to compile a converge.dll and use the converge-udf executable instead of the normal one. If you dont want to add further variables, there is no need for modification of the original .c files (you get them from the converge download area). However, it might be more efficient to delete all unnecessary functions from the makefile and create a smaller converge.dll file.

Adding further variables of interest is not so easy to do, if you dont have a bit of programming background.
MFGT is offline   Reply With Quote

Old   May 26, 2016, 11:24
Default
  #7
New Member
 
amrrhm
Join Date: May 2016
Posts: 20
Rep Power: 9
amrrhm is on a distinguished road
There is no udf executable for 2.3, is that right or I am missing it?
amrrhm is offline   Reply With Quote

Old   May 27, 2016, 17:30
Default
  #8
Member
 
ywang89's Avatar
 
Yunliang Wang
Join Date: Dec 2015
Location: Convergent Science, Madison WI
Posts: 58
Rep Power: 10
ywang89 is on a distinguished road
Quote:
Originally Posted by amrrhm View Post
There is no udf executable for 2.3, is that right or I am missing it?
For Linux, there is only one CONVERGE 2.3 executable for the runs with UDFs and without UDFs. When udf_flag=1, the code will try to find the UDF library.

Thanks,
__________________
Yunliang Wang
Applications Manager

CONVERGECFD
ywang89 is offline   Reply With Quote

Old   June 1, 2016, 11:55
Default
  #9
New Member
 
amrrhm
Join Date: May 2016
Posts: 20
Rep Power: 9
amrrhm is on a distinguished road
Hi all and thank you all for your input.

I have selected couple of points to get output (velocity, temp, pressure) for only those points. I have followed the UDF manual, copied everything in a udf_dir folder, edited the object part in makefile so it only contains user_points.o and user_points_data.o and ran the make. I set the LD_LIBRARY_PATH as "export LD_LIBRARY_PATH=./udf_dir/"

After all, when I try check_inputs in the serial mode I get:

Loading CONVERGE UDF LIBRARY: libconverge_udf.so
./udf_dir/libconverge_udf.so: undefined symbol: user_load_csi_libraries

and if I use the mpi, I get:
error while loading shared libraries: libmpi.so.1: cannot open shared object file: No such file or directory


Any ideas where I am making mistake? Thanks
amrrhm is offline   Reply With Quote

Old   June 1, 2016, 17:44
Default
  #10
Member
 
alemoine's Avatar
 
Allie Le Moine
Join Date: Jan 2016
Location: Convergent Science, Madison WI
Posts: 39
Rep Power: 10
alemoine is on a distinguished road
Quote:
Originally Posted by amrrhm View Post
Hi all and thank you all for your input.

I have selected couple of points to get output (velocity, temp, pressure) for only those points. I have followed the UDF manual, copied everything in a udf_dir folder, edited the object part in makefile so it only contains user_points.o and user_points_data.o and ran the make. I set the LD_LIBRARY_PATH as "export LD_LIBRARY_PATH=./udf_dir/"

After all, when I try check_inputs in the serial mode I get:

Loading CONVERGE UDF LIBRARY: libconverge_udf.so
./udf_dir/libconverge_udf.so: undefined symbol: user_load_csi_libraries

and if I use the mpi, I get:
error while loading shared libraries: libmpi.so.1: cannot open shared object file: No such file or directory


Any ideas where I am making mistake? Thanks

Hi amrrhm,

If you are using CONVERGE v2.3, you will need to include the user_dynamic_routines.c in the directory. Therefore, your makefile should have the following object files:

OBJS = user_dynamic_routines.o\
user_points.o\
user_points_data.o

Please change the makefile and rerun make to see if this error message goes away.

It should be noted that ALL udf's in v2.3 require user_dynamic_routines.c.

Thank you,
__________________
Allie Le Moine
Research Engineer | Applications
CONVERGECFD
alemoine is offline   Reply With Quote

Old   June 3, 2016, 14:10
Default
  #11
New Member
 
amrrhm
Join Date: May 2016
Posts: 20
Rep Power: 9
amrrhm is on a distinguished road
It works now. Thank you very much.
amrrhm is offline   Reply With Quote

Reply

Tags
export data, udf

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] Error snappyhexmesh - Multiple outside loops avinashjagdale OpenFOAM Meshing & Mesh Conversion 53 March 8, 2019 09:42
Run OpenFoam in 2 nodes of a cluster WhiteW OpenFOAM Running, Solving & CFD 16 December 20, 2016 00:51
[Commercial meshers] fluentMeshToFoam multidomain mesh conversion problem Attesz OpenFOAM Meshing & Mesh Conversion 12 May 2, 2013 10:52
exporting data sourav FLUENT 2 August 16, 2005 15:05
Exporting data... Gustaf Mårtensson CFX 2 September 16, 2003 08:37


All times are GMT -4. The time now is 03:14.