Cycle 12 PGM CALL

ISO programming

G39

Application

NC programs that you have created (such as special drilling cycles or geometrical modules) can be written as machining cycles. These NC programs can then be called like normal cycles.

Note

  • You can execute this cycle in the following operating modes: FUNCTION MODE MILL.
  • As a rule, Q parameters are globally effective when called with Cycle 12. So please note that changes to Q parameters in the called NC program can also influence the calling NC program.

Notes on programming

  • The NC program you are calling must be stored in the internal memory of your control.
  • If the NC program you are defining to be a cycle is located in the same directory as the NC program you are calling it from, you need only enter the program name.
  • If the NC program you are defining to be a cycle is not located in the same directory as the NC program you are calling it from, you must enter the complete path, for example TNC:\KLAR35\FK1\50.H.
  • If you want to define an ISO program to be a cycle, add the .I file type to the program name.

Cycle parameters

Help graphic

Parameter

Program name

Enter the name of the NC program to be called and, if necessary, the path where it is located,

Use the Select File Select in the action bar of the NC program to be called.

Call the NC program with:

  • CYCL CALL (separate NC block) or
  • M99 (blockwise) or
  • M89 (executed after every positioning block)

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Declare NC program 1_Plate.h as a cycle and call it with M99

11 CYCL DEF 12.0 PGM CALL

12 CYCL DEF 12.1 PGM TNC:\nc_prog\demo\OCM\1_Plate.h

13 L X+20 Y+50 R0 FMAX M99