3D tool compensation during peripheral milling (#9 / #4-01-1)

Application

Peripheral milling is a machining operation carried out with the lateral surface of the tool.

The control offsets the tool perpendicular to the direction of movement and perpendicular to the tool direction by the total of the delta values from the tool management, the tool call and the compensation tables.

Requirements

Description of function

The variants below are possible with peripheral milling:

  • L block with programmed rotary axes, M128 or FUNCTION TCPM active, define compensation direction with radius compensation RL or RR
  • LN block with tool orientation T perpendicular to the N vector, M128 or FUNCTION TCPM is active
  • LN block with tool orientation T without N vector, M128, or FUNCTION TCPM is active

The TNC7 basic can move up to four axes simultaneously. If an NC block commands movement of more than four axes, the control displays an error message. If the axis position does not change, you can nevertheless program more than four axes.

Example

11 M128

* - ...

21 L X+48.4074 Y+102.4717 Z-7.1088 C+0 B-20.0115 RL

; Compensation is possible, compensation direction RL

11 LN X+60.6593 Y+102.4690 Z-7.1012 NX0.0000 NY0.9397 NZ0.3420 TX-0.0807 TY0 TZ0.9366 R0 M128

; Compensation is possible

11 LN X+60.6593 Y+102.4690 Z-7.1012 TX-0.0807 TY0 TZ0.9366 M128

; Compensation is possible

Notes

 
Notice
Danger of collision!
The rotary axes of a machine may have limited ranges of traverse (e.g., between –90° and +10° for the B head axis). Changing the tilt angle to a value of more than +10° may result in a 180° rotation of the table axis. There is a danger of collision during the tilting movement!
  1. Program a safe tool position before the tilting movement, if necessary.
  2. Carefully test the NC program or program section in the Single Block mode

Example

Compensate re-worked end mill
CAM output at tool center

You use a re-worked Ø 11.8 mm end mill instead of Ø 12 mm.

The NC program has the following structure:

  • CAM output for Ø 12 mm end mill
  • NC points output on the tool center
  • Vector program with surface normal vectors and tool vectors
  • Alternative:

  • Klartext program with active tool radius compensation RL/RR

Proposed solution:

  • Tool measurement on tool tip
  • Suppress the error message with M107
  • Enter the tool compensation into the tool table:
    • R and R2 the theoretical tool data as from the CAM system
    • DR and DL the difference between the nominal value and the actual value

R

R2

DL

DR

DR2

CAM

+6

+0

Tool table

+6

+0

+0

-0.1

+0