Cycle 30 or 480 CALIBRATE TT

ISO programming

G480

Application

 
Machine

Refer to your machine manual!

You calibrate the TT with touch probe cycle 30 or 480 (Differences between Cycles 30 to 33 and Cycles 480 to 483). The calibration process runs automatically. The control also measures the center misalignment 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 30 or 480 .

Touch probe

For the touch probe you use a spherical or cuboid probe contact

Cuboid probe contact

For a cuboid probe contact, the machine manufacturer can store in the optional machine parameters detectStylusRot (no. 114315) and tippingTolerance (no. 114319) whether the angle of misalignment and tilt angle are determined. Determining the angle of misalignment enables compensation for it when measuring tools. The control displays a warning if the tilt angle is exceeded. The values determined can be seen in the status display of the TT.

TT tab

 
Tip

When clamping the tool touch probe, make sure that the edges of the cuboid probe contact are aligned as parallel to the machine axes as possible. The angle of misalignment should be less than 1° and the tilt angle should be less than 0.3°.

Calibration tool

The calibration tool must be a precisely cylindrical part, for example a cylindrical pin. The resulting calibration values are stored in the control memory and are accounted for during subsequent tool measurement.

Cycle sequence

  1. Clamp the calibration tool. The calibration tool must be a precisely cylindrical part, for example a cylindrical pin
  2. Manually position the calibration tool in the working plane over the center of the TT
  3. Position the calibration tool in the tool axis at approximately 15 mm plus set-up clearance over the TT
  4. 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.
  5. The calibration process along the tool axis starts
  6. This is followed by calibration in the working plane
  7. The control positions the calibration tool in the working plane at a position of TT radius + set-up clearance + 11 mm
  8. Then the control moves the tool downwards along the tool axis and the calibration process starts
  9. During probing, the control moves in a square pattern
  10. The control saves the calibration values and considers them during subsequent tool measurement
  11. 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 only be executed 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.

 
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.

Example of new format

11 TOOL CALL 12 Z

12 TCH PROBE 480 CALIBRATE TT ~

Q260=+100

;CLEARANCE HEIGHT

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.

Example of old format

11 TOOL CALL 12 Z

12 TCH PROBE 30.0 CALIBRATE TT

13 TCH PROBE 30.1 HEIGHT:+90