Cycles
Fundamentals
In ISO programs, you can use selected cycles with Klartext syntax in addition to the NC functions with ISO syntax. Programming is identical to Klartext programming.
The numbers of the Klartext cycles correspond to the numbers of the G functions. There are exceptions for earlier cycles that have numbers below 200. In these cases, the corresponding G function number is mentioned in the cycle description.
The following cycles are not available in ISO programs:
- Cycle 1 POLAR PRESET
- Cycle 3 MEASURING
- Cycle 4 MEASURING IN 3-D
- Cycle 26 AXIS-SPECIFIC SCALING
HEIDENHAIN recommends using the more powerful PLANE functions instead of Cycle G80 WORKING PLANE. With the PLANE functions, you can choose freely between axis or spatial angles for programming.
Datum shift
With the G53 or G54 NC functions, you can program datum shifts. G54 shifts the workpiece datum to the coordinates you define directly within this function. G53 uses coordinate values from a datum table. A datum shift allows machining operations to be repeated at any locations on the workpiece.
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.
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.
N110 G54 X+0 Y+50 | ; Shift the workpiece datum to the defined coordinates |
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.
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.
N110 G53 P01 10 | ; Shift the workpiece datum to the coordinates of table row 10 |
To reset a datum shift:
- Define the value 0 for each axis in function G54
- In function G53, select a table row where all columns have the value 0
The control displays the following information in the Status workspace:
- Name and path of the active datum table
- Active datum number
- Comment from the DOC column of the active datum number
Notes
In the machine parameter CfgDisplayCoordSys (no. 127501) the machine manufacturer defines the coordinate system in which the status display shows an active datum shift.
- Datums from a datum table always reference the current workpiece preset.
- Before shifting the workpiece datum by means of a datum table, you need to activate the datum table with %:TAB:
- If you do not use %:TAB:, you have to activate the datum table manually.