Cycle 463 TS CALIBRATION ON STUD (#17 / #1-05-1)
ISO programming
G463
Application
Refer to your machine manual.
Before starting the calibration cycle, you need to pre-position the touch probe above the center of the calibration pin. Position the touch probe in the touch probe axis by approximately the set-up clearance (value from touch probe table + value from cycle) above the calibration pin.
When calibrating the ball-tip radius, the control executes an automatic probing routine. In the first run the control finds the midpoint of the calibration ring or stud (approximate measurement) and positions the touch probe in the center. Then, during the actual calibration process (fine measurement), the radius of the ball tip is determined. If the touch probe permits a reversal measurement, the center offset is determined during another run.
A measuring log is created automatically during calibration. The log file is named TCHPRAUTO.html. This file is stored in the same location as the original file. The measuring log can be displayed in the browser on the control. If an NC program uses more than one cycle to calibrate the touch probe, TCHPRAUTO.html will contain all the measuring logs.
The orientation of the touch probe determines the calibration routine:
- No orientation possible, or orientation in only one direction: The control executes one approximate and one fine measurement, and then ascertains the effective ball-tip radius (column R in tool.t).
- Orientation possible in two directions (e.g., HEIDENHAIN touch probes with cable): The control executes one approximate and one fine measurement, rotates the touch probe by 180°, and then executes four more probing routines. The reversal measurement determines now only the radius but also the center offset (CAL_OF in the touch-probe table).
- Any orientation possible (e.g., HEIDENHAIN infrared touch probes): Probing operation: see "Orientation possible in two directions"
Note:
In order to be able to determine the ball-tip center offset, the control needs to be specially prepared by the machine manufacturer.
Whether or how your touch probe can be oriented is predefined for HEIDENHAIN touch probes. Other touch probes are configured by the machine manufacturer.
HEIDENHAIN guarantees the proper operation of the touch probe cycles only in conjunction with HEIDENHAIN touch probes.
- Do not activate the following cycles before the use of touch probe cycles:
- Cycle 7 DATUM SHIFT
- Cycle 8 MIRRORING
- Cycle 10 ROTATION
- Cycle 11 SCALING FACTOR
- Cycle 26 AXIS-SPECIFIC SCALING
- Reset any coordinate transformations beforehand.
- This cycle can be executed only in the FUNCTION MODE MILL and FUNCTION MODE TURN machining modes.
- The center offset can be determined only with a suitable touch probe.
- A measuring log is created automatically during calibration. The log file is named TCHPRAUTO.html.
Note on programming
- Before defining this cycle, you must have programmed a tool call to define the touch probe axis.
Cycle parameters
Help graphic | Parameter |
---|---|
Q407 Radius of calibr. stud? Diameter of the calibration stud Input: 0.0001...99.9999 | |
Q320 Set-up clearance? Additional distance between touch point and ball tip. Q320 is active in addition to the SET_UP column in the touch probe table. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q301 Move to clearance height (0/1)? Define how the touch probe will move between the measuring points: 0: Move to measuring height between measuring points 1: Move to clearance height between measuring points Input: 0, 1 | |
Q423 Number of probes? Number of measuring points on the diameter. This value has an absolute effect. Input: 3...8 | |
Q380 Ref. angle in ref. axis? Angle between the main axis of the working plane and the first touch point. This value has an absolute effect. Input: 0...360 |
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.
11 TCH PROBE 463 TS CALIBRATION ON STUD ~ | ||
| ||
| ||
| ||
| ||
|