Tool radius compensation

Application

When tool radius compensation is active, the control will no longer reference the positions in the NC program to the tool center point, but to the cutting edge.

Use tool radius compensation to program drawing dimensions without having to consider the tool radius. This lets you use a tool with deviating dimensions without having to modify the program after a tool has broken.

Requirements

Description of function

The control takes the active tool radius into account during tool radius compensation. The active tool radius results from the tool radius R and the delta values DR from the tool management and the NC program.

Active tool radius = R + DRTAB + DRProg

Tool compensation for tool length and tool radius

Paraxial traverses can be corrected as follows:

  • R+: lengthens a paraxial traverse by the amount of the tool radius
  • R-: shortens a paraxial traverse by the amount of the tool radius

An NC block with path functions can contain the following types of tool radius compensation:

  • RL: tool radius compensation, on the left of the contour
  • RR: tool radius compensation, on the right of the contour
  • R0: resets an active tool radius compensation, positioning with the tool center point

Radius-compensated traverse with path functions

Radius-compensated traverse with paraxial movements

The tool center moves along the contour at a distance equal to the radius. Right or left are to be understood as based on the direction of tool movement along the workpiece contour.

RL: The tool moves on the left of the contour

RR: The tool moves on the right of the contour

Effect

Tool radius compensation is active starting from the NC block in which tool radius compensation is programmed. Tool radius compensation is effective modally and at the end of the block.

 
Tip

Program tool radius compensation only once, allowing for quicker implemention of changes, for example.

The control resets tool radius compensation in the following cases:

  • Positioning block with R0
  • DEP function for departing from the contour
  • Selection of a new NC program

Notes

 
Notice
Danger of collision!
The control needs safe positions for contour approach and departure. These positions must enable the control to perform compensating movements when radius compensation is activated and deactivated. Incorrect positions can lead to contour damage. Danger of collision during machining!
  1. Program safe approach and departure positions at a sufficient distance from the contour
  2. Consider the tool radius
  3. Consider the approach strategy
  • When tool radius compensation is active, the control displays an symbol in the Positions workspace.
  • The Positions workspace

  • If radius compensation is active and you execute the following functions, the control aborts program run and displays an error message:
    • PLANE functions (#8 / #1-01-1)
    • M128 (#9 / #4-01-1)
    • FUNCTION TCPM (#9 / #4-01-1)
    • CALL PGM
    • Cycle 12 PGM CALL
    • Cycle 32 TOLERANCE
    • Cycle 19 WORKING PLANE
    •  
      Tip

      You can still execute NC programs from earlier controls that contain Cycle 19 WORKING PLANE.

Notes in connection with the machining of corners

  • Outside corners:
    If you program radius compensation, the control moves the tool around outside corners on a transitional arc. If necessary, the control reduces the feed rate at outside corners during, for example, large changes in direction.
  • Inside corners:
    The control calculates the intersection of the tool center paths at inside corners under radius compensation. Starting at this point, the tool moves along the next contour element. This prevents damage to the workpiece at the inside corners. As a result, the tool radius for a certain contour cannot be selected to be just any size.