Cycle 32 or 482 CAL. TOOL RADIUS

ISO programming

G482

Application

 
Machine

Refer to your machine manual!

If you want to measure the tool radius, program the touch probe cycle 32 or 482 (Differences between Cycles 30 to 33 and Cycles 480 to 483). Input parameters allow you to select which of the two following methods will be used to measure the tool radius:

  • Measuring the tool while it is rotating
  • Measuring the tool while it is rotating and subsequently measuring the individual teeth

The control pre-positions the tool to be measured to a position at the side of the touch probe head. The distance from the face of the milling tool to the upper edge of the touch probe head is defined in offsetToolAxis (no. 122707). The control probes the tool radially while it is rotating. If you have programmed a subsequent measurement of individual teeth, the control will measure the radius of each tooth with the aid of oriented spindle stops.

Notes

 
Notice
Danger of collision!
If you set stopOnCheck (no. 122717) to FALSE, the control does not evaluate the result parameter Q199 and the NC program is not stopped if the breakage tolerance is exceeded. There is a danger of collision!
  1. Set stopOnCheck (no. 122717) to TRUE
  2. You must then take steps to ensure that the NC program stops if the breakage tolerance is exceeded
  • This cycle can only be executed in the FUNCTION MODE MILL machining mode.
  • Before measuring a tool for the first time, enter the following data on the tool into the TOOL.T tool table: the approximate radius, the approximate length, the number of teeth, and the cutting direction.
  • Cycles 32 and 482 do not support touch probes, turning or dressing tools.

Measuring grinding tools

  • The cycle takes into account the basic and compensation data from the TOOLGRIND.GRD table, as well as the wear and compensation data (RBREAK and RTOL) from the TOOL.T table.
  • Q340: 0 and 1
  • This cycle will modify compensation or basic data, depending on whether or not an initial dressing operation (INIT_D) is defined. This cycle will enter the values automatically at the correct locations in the TOOLGRIND.GRD table.

Note the following sequence for setting up grinding tools

Tool data for the tool types

Notes about 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.
  • Cylindrical tools with diamond surfaces can be measured while the spindle is stationary. To do so, in the tool table define the number of teeth CUT as 0 and adjust the machine parameter CfgTT. Refer to your machine manual.

Cycle parameters

Help graphic

Parameter

Q340 Tool measurement mode (0-2)?

Define whether and how the measured data will be entered in the tool table.

0: The measured tool radius is written to column R of the TOOL.T tool table, and the tool compensation is set to DR = 0. If there is already a value in TOOL.T, it will be overwritten.

1: The measured tool radius is compared to the tool radius R from TOOL.T. The control calculates the deviation from the stored value and enters it into TOOL.T as the delta value DR. The deviation is also available in the Q parameter Q116. If the delta value is greater than the permissible tool radius tolerance for wear or break detection, the control will lock the tool (status L in TOOL.T).

2: The measured tool radius is compared to the tool radius from TOOL.T. The control calculates the deviation from the stored value and writes it to Q parameter Q116. Nothing is entered under R or DR in the tool table.

Input: 0, 1, 2

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 that the tool tip would lie below the top of the probe contact, the control automatically positions the tool above the top of the probe contact (safety zone from safetyDistStylus).

Input: –99999.9999...+99999.9999

Q341 Probe the teeth? 0=no/1=yes

Define whether the control will measure the individual teeth (maximum of 20 teeth)

Input: 0, 1

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 482 CAL. TOOL RADIUS ~

Q340=+1

;CHECK ~

Q260=+100

;CLEARANCE HEIGHT ~

Q341=+1

;PROBING THE TEETH

Cycle 32 includes an additional parameter:

Help graphic

Parameter

Parameter number for result?

Parameter number in which the control stores the status of the measurement:

0.0: Tool is within the tolerance

1.0: Tool is worn (RTOL exceeded)

2.0: Tool is broken (RBREAK exceeded). If you do not wish to use the result of measurement within the NC program, answer the dialog prompt with NO ENT

Input: 0...1999

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.

Measuring a rotating tool for the first time; old format

11 TOOL CALL 12 Z

12 TCH PROBE 32.0 CAL. TOOL RADIUS

13 TCH PROBE 32.1 CHECK:0

14 TCH PROBE 32.2 HEIGHT:+120

15 TCH PROBE 32.3 PROBING THE TEETH:0

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.

Inspecting a tool and measuring the individual teeth and saving the status in Q5; old format

11 TOOL CALL 12 Z

12 TCH PROBE 32.0 CAL. TOOL RADIUS

13 TCH PROBE 32.1 CHECK:1 Q5

14 TCH PROBE 32.2 HEIGHT:+120

15 TCH PROBE 32.3 PROBING THE TEETH:1