Cycle 480 CALIBRATE TT (#17 / #1-05-1)
ISO programming
G480
Application
Refer to your machine manual!
You calibrate the TT with touch probe cycle 480. The calibration process runs automatically. The control also measures the center offset of the calibration tool automatically by rotating the spindle by 180° after the first half of the calibration cycle.
You calibrate the TT with touch probe cycle 480.
Cycle run
- Clamp the calibration tool. The calibration tool must be a precisely cylindrical part, for example a cylindrical pin
- Manually position the calibration tool in the working plane over the center of the TT
- Position the calibration tool in the tool axis at approximately 15 mm plus set-up clearance over the TT
- The first movement of the tool is along the tool axis. The tool is first moved to clearance height, i.e. set-up clearance + 15 mm.
- The calibration process along the tool axis starts
- This is followed by calibration in the working plane
- The control positions the calibration tool in the working plane at a position of TT radius + set-up clearance + 11 mm
- Then the control moves the tool downwards along the tool axis and the calibration process starts
- During probing, the control moves in a square pattern
- The control saves the calibration values and considers them during subsequent tool measurement
- The control then retracts the stylus along the tool axis to set-up clearance and moves it to the center of the TT
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- Before calibrating the touch probe, you must enter the exact length and radius of the calibration tool into the TOOL.T tool table.
Notes about machine parameters
- Use the machine parameter CfgTTRoundStylus (no. 114200) or CfgTTRectStylus (no. 114300) to define the functionality of the calibration cycle. Refer to your machine manual.
- Use the machine parameter centerPos to define the position of the TT within the machine's working space.
- The TT needs to be recalibrated if you change the position of the TT on the table and/or a centerPos machine parameter.
- In the machine parameter probingCapability (no. 122723), the machine manufacturer defines the functionality of the cycle. This parameter allows you to permit tool length measurement with a stationary spindle and at the same time to inhibit tool radius and individual tooth measurements.
Cycle parameters
Help graphic | Parameter |
---|---|
Q260 Clearance height? Enter the position in the spindle axis at which there is no danger of collision with the workpiece or fixtures. The clearance height is referenced to the active workpiece preset. If you enter such a small clearance height value that the tool tip would lie below the top of the probe contact, the control automatically positions the calibration tool above the top of the probe contact (safety zone from safetyDistToolAx (no. 114203)). Input: –99999.9999...+99999.9999 |
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 TOOL CALL 12 Z | ||
12 TCH PROBE 480 CALIBRATE TT ~ | ||
|