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.
Related topics
- Presets on the tool
Requirements
- Parameters have been defined in tool management
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.
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
- Program safe approach and departure positions at a sufficient distance from the contour
- Consider the tool radius
- Consider the approach strategy
- When tool radius compensation is active, the control displays an symbol in 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.