Cycle 484 CALIBRATE IR TT (#17 / #1-05-1)

ISO programming

G484

Application

Cycle 484 allows you to calibrate your tool touch probe (e.g., the wireless infrared TT 460 tool touch probe). You can perform the calibration process with or without manual intervention.

  • With manual intervention: If you define Q536 = 0, then the control will stop before the calibration process. You then need to position the calibration tool manually above the center of the tool touch probe.
  • Without manual intervention: If you define Q536 = 1, then the control will automatically execute the cycle. You may have to program a prepositioning movement before. This depends on the value of the parameter Q523 POSITION TT.

Cycle run

 
Machine

Refer to your machine manual.

The machine manufacturer defines the functionality of the cycle.

To calibrate the tool touch probe, program the touch probe cycle 484. In input parameter Q536, you can specify whether you want to run the cycle with or without manual intervention.

Q536 = 0: With manual intervention before calibration

Proceed as follows:

  1. Insert the calibration tool
  2. Start the calibration cycle
  3. The control interrupts the calibration cycle and displays a dialog.
  4. Manually position the calibration tool above the center of the tool touch probe.
  5.  
    Tip

    Ensure that the calibration tool is located above the measuring surface of the probe contact.

  6. Press NC Start to resume cycle run
  7. If you have programmed Q523 = 2, the control writes the calibrated position to the machine parameter centerPos (no. 114200)

Q536 = 1: Without manual intervention before calibration

Proceed as follows:

  1. Insert the calibrating tool
  2. Position the calibration tool above the center of the tool touch probe before the start of the cycle.
  3.  
    Tip
    • Ensure that the calibration tool is located above the measuring surface of the probe contact.
    • For a calibration process without manual intervention, you do not need to position the calibration tool above the center of the tool touch probe. The cycle adopts the position from the machine parameters and automatically moves the tool to this position.
  4. Start the calibration cycle
  5. The calibration cycle is executed without stopping.
  6. If you have programmed Q523 = 2, then the control writes the calibrated position to the machine parameter centerPos (no. 114200).

Notes

 
Notice
Danger of collision!
If you program Q536=1, the tool must be pre-positioned before calling the cycle. The control also measures the center misalignment of the calibrating tool by rotating the spindle by 180° after the first half of the calibration cycle. There is a danger of collision!
  1. Specify whether to stop before cycle start or run the cycle automatically without stopping.
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The calibration tool should have a diameter of more than 15 mm and protrude approx. 50 mm from the chuck. If you use a cylinder pin of these dimensions, the resulting deformation will only be 0.1 µm per 1 N of probing force. Major inaccuracies may occur if you use a calibration tool whose diameter is too small and/or that protrudes too far from the chuck.
  • Before calibrating the touch probe, you must enter the exact length and radius of the calibration tool into the TOOL.T tool table.
  • The TT needs to be recalibrated if you change its position on the table.

Note regarding machine parameters

  • 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

Q536 Stop before running (0=Stop)?

Define whether the control will stop before the calibration process or whether the cycle will automatically be executed without a stop:

0: Stop before the calibration process. The control prompts you to position the calibration tool manually above the tool touch probe. After moving the tool to the approximate position above the tool touch probe, press NC Start to continue the calibration process or press the the CANCEL button to cancel the calibration process.

1: Without stopping before the calibration process. The control starts the calibration process depending on Q523. Before running Cycle 484, you may have to position the tool above the tool touch probe.

Input: 0, 1

Q523 Position of tool probe (0-2)?

Position of the tool touch probe:

0: Current position of the calibration tool. The tool touch probe is below the current position of the calibration tool. If Q536 = 0, position the calibration tool manually above the center of the tool touch probe during the cycle. If Q536 = 1, you need to position the calibration tool above the center of the tool touch probe before the start of the cycle.

1: Configured position of the tool touch probe. The control adopts the position from the machine parameter centerPos (no. 114201). You do not need to pre-position the tool. The calibration tool approaches the position automatically.

2: Current position of the calibration tool. See Q523 = 0. 0. The control additionally writes the determined position (where applicable) to the machine parameter centerPos (no. 114201) after calibration.

Input: 0, 1, 2

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

11 TOOL CALL 12 Z

12 TCH PROBE 484 CALIBRATE IR TT ~

Q536=+0

;STOP BEFORE RUNNING ~

Q523=+0

;TT POSITION