Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Touch Probe Cycles: Automatic Tool Measurement | Measuring tool length and radius (Cycle 33 or 483, DIN/
ISO: G483)

Cycle parameters

Tool measurement mode (0-2)?: Specify whether
and how the determined data will be entered in
the tool table
0: The measured tool length and measured tool
radius are written to columns L and R of the tool
table TOOL.T, and the tool compensation is set to
DL=0 and DR=0. If there is already a value stored
in TOOL.T, it will be overwritten.
1: The measured tool length and measured tool
radius are compared to the tool length L and tool
radius R from TOOL.T. The TNC calculates the
deviation from the stored value and enters them
into TOOL.T as the delta values DL and DR. The
deviation is also available in Q parameters Q115
and Q116. If the delta value is greater than the
permissible tool length or radius tolerance for
wear or break detection, the TNC will lock the tool
(status L in TOOL.T)
2: The measured tool length and the measured
tool radius are compared to the tool length L and
tool radius R from TOOL.T. The TNC calculates the
deviation from the stored value and enters them in
Q parameters Q115 and Q116. Nothing is entered
under L, R, DL, or DR in the tool table.
Parameter number for result?: Parameter
number in which the TNC saves the status of the
measurement result:
0.0: Tool is within tolerance
1.0: Tool is worn (LTOL and/or RTOL exceeded)
2.0: Tool is broken (LBREAK and/or RBREAK
exceeded) If you do not wish to use the result of
measurement within the program, answer the
dialog prompt with NO ENT
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 level of the
probe contact, the TNC automatically positions
the tool above the level of the probe contact
(safety zone from safetyDistStylus). Input range
-99999.9999 to 99999.9999
Probe the teeth? 0=no/1=yes: Choose whether
the control is to measure the individual teeth
(maximum of 20 teeth)
HEIDENHAIN | User's manual for cycle programming | 10/2017
Measuring a rotating tool for the first
time; old format
6 TOOL CALL 12 Z
7 TCH PROBE 33.0 MEASURE TOOL
8 TCH PROBE 33.1 CHECK: 0
9 TCH PROBE 33.2 HEIGHT: +120
10 TCH PROBE 33.3 PROBING THE
TEETH: 0
Inspecting a tool and measuring the
individual teeth and saving the status
in Q5; old format
6 TOOL CALL 12 Z
7 TCH PROBE 33.0 MEASURE TOOL
8 TCH PROBE 33.1 CHECK: 1 q5
9 TCH PROBE 33.2 HEIGHT: +120
10 TCH PROBE 33.3 PROBING THE
TEETH: 1
NC blocks in new format
6 TOOL CALL 12 Z
7 TCH PROBE 483 MEASURE TOOL
Q340=1 ;CHECK
Q260=+100 ;CLEARANCE HEIGHT
Q341=1 ;PROBING THE TEETH
20
733