Tool Compensation; Introduction; Tool Length Compensation - HEIDENHAIN TNC 620 User Manual

Tools | Tool compensation
4.3

Tool compensation

Introduction

The control adjusts the tool path by the compensation value
for the tool length in the spindle axis. In the machining plane, it
compensates the tool radius.
If you are writing the NC program directly on the control, the tool
radius compensation is effective only in the working plane.
The control accounts for the compensation value in up to five axes
including the rotary axes.

Tool length compensation

Length compensation becomes effective automatically as soon as
a tool is called. To cancel length compensation, call a tool with the
length L=0 (e.g. TOOL CALL 0).
Danger of collision!
The control uses the defined tool lengths for tool length
compensation. Incorrect tool lengths will result in an incorrect
tool length compensation. The control does not perform a length
compensation and a collision check for tools with a length of 0
and after TOOL CALL 0. Danger of collision during subsequent
tool positioning movements!
Always define the actual tool length of a tool (not just the
difference)
Use TOOL CALL 0 only to empty the spindle
With length compensation, delta values from both the NC program
and the tool table are considered.
Compensation value = L + DL
Tool length L from TOOL DEF block or tool table
L:
: Oversize for length DL in the tool table
DL
TAB
: Oversize DL for length from TOOL CALL block or
DL
Prog
from the compensation table
The most recently programmed value takes effect.
Further information: "Compensation table",
Page 398
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022
NOTICE
+ DL with
TAB Prog
4
133