Cycle 482 CAL. TOOL RADIUS (#17 / #1-05-1)

ISO programming

G482

Application

 
Machine

Refer to your machine manual!

If you want to measure the tool radius, program the touch probe cycle 482. Select via input parameters by which of two methods the tool radius is to be measured:

  • 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 for individual tooth measurement Q341=1

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 be executed only 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.
  • Cycle 482 supports neither turning tools nor dressing tools nor touch probes.

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.
  • 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.

Notes for individual tooth measurement Q341=1

 
Notice
Caution: Danger to the tool and workpiece!
Individual tooth measurement of tools with a large angle of twist may result in a failure of the control to identify tool wear or a broken tool. In this case, tool and workpiece damage may result during subsequent machining operations.
  1. Check the workpiece dimensions (for example, by using a workpiece touch probe)
  2. Check the workpiece optically in order to exclude broken tools

If the maximum angle of twist is exceeded, you should not carry out individual tooth measurement.

On tools with an even distribution of teeth, a maximum angle of twist can be defined as follows:

Abbreviation

Definition

ε

Maximum angle of twist

h[tt]

Height of tool touch probe contact

R

Tool radius

x

Number of teeth of tool

 
Tip

On tools with an uneven distribution of teeth, there is no calculation formula for the maximum angle of twist Check these tools optically in order to exclude breaks. You can measure wear indirectly by measuring the workpiece.

 
Notice
Caution: Possible material damage!
Individual tooth measurement of tools with an uneven distribution of teeth may cause the control to identify non-existing wear. The higher the angle deviation and the larger the tool radius, the more probably this behavior can occur. If the control compensates for the tool incorrectly after individual tooth measurement, the workpiece may have to be rejected.
  1. Check the workpiece dimensions during subsequent machining operations

Individual tooth measurement of tools with an uneven distribution of teeth may cause the control to identify non-existing breakage and lock the tool.

The higher the angle deviation 1 and the larger the tool radius, the more probably this behavior can occur.

1 Angle deviation

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

11 TOOL CALL 12 Z

12 TCH PROBE 482 CAL. TOOL RADIUS ~

Q340=+1

;CHECK ~

Q260=+100

;CLEARANCE HEIGHT ~

Q341=+1

;PROBING THE TEETH