UG怎样一次把多个刀路编程出多个程序？

UG怎样一次把多个刀路编程出多个程序？
谢谢。

用CTRL+你想要的程序点后处理就可以了，

我问的是一次编出多个程序，就像PM那样？多个，而不是把多个刀路编出一个程序。

最多只能一次转出CLSF文件，然后在生成G代码时则由控制CLSF文件来实现，但是还是不能达到你所说的那样，一次出多个程序，不过这样也会省不少时间。

mc 可以。UG不知到

xjx wrote:
UG怎样一次把多个刀路编程出多个程序？  
  谢谢。

  
    晕! 你可十天学会CIM, 这简单的东西都不会用POSEBUILDER做？
给你一个提示: 象CIM 一样， 在换刀时改为生成文件就可以。

老大，你的意思是不是要修改后处理？
不知用MDFG可不可做到？

This option allows you to define how your post handles groups. You can organize your operations into groups in Unigraphics NX to create more than one NC program in a part file. The system considers each group as one program and you should considered it as one complete NC tape. The default setting for this option is OFF. You should not use this option unless you want to postprocess more than one NC program at a time.  
  
If you select more than one group and you have this option turned ON you get one file that contains all of the groups (programs) that you have selected. The system names this file my_file.ptp. You also get an NC program file for each group or program you have selected. The system names them my_file_group.ptp. If your base file name is "nctape" and your group or program name is "O1234" then the name of your file will be nctape_O1234.ptp.  
  
Do not mix operations in groups with operations outside of groups when you have set the group output to on. This causes unpredictable output. When you set the group output to off, you only get a single NC output file called my_file.ptp. The system outputs all operations in any selected group in a single NC file. The system ignores all group organization.  
  
You can use the name of the group or program in Unigraphics NX as the program name in the Start of Program event. The system passes this to you as the variable name mom_group_name.

,  
  
可以的, 在UG的POSTBUILDER中 import  一个"custom_command" -----pb_cmd_tape_utils.tcl, 其中有一个TCL 程序"B_CMD_output_tape_per_operation"的程序,调用它就可以同时将多个操作处理成单独的NC程序,即一次处理出多个程序

我是打開這個地方,不知道有啥不同??