Cycle Parameters - HEIDENHAIN TNC 620 User Manual

18
Touch Probe Cycles: Automatic Tool Measurement
18.6 Measuring tool length and radius (Cycle 483)

Cycle parameters

Measure tool=0 / Check tool=1: Select whether
the tool is to be measured for the first time or
whether a tool that has already been measured
is to be inspected. If the tool is being measured
for the first time, the TNC overwrites the tool
radius R and the tool length L in the central tool file
TOOL.T by the delta values DR = 0 and DL = 0. If
you wish to inspect a tool, the TNC compares the
measured data with the tool data stored in TOOL.T.
The TNC calculates the deviations and enters them
as positive or negative delta values DR and DL in
TOOL.T. The deviations are also available in the Q
parameters Q115 and Q116. If the delta values are
greater than the permissible tool tolerances for wear
or break detection, the TNC will lock the tool (status
L in TOOL.T).
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 datum. 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
Cutter measurement? 0=No / 1=Yes: Choose
whether the control is also to measure the individual
teeth (maximum of 20 teeth)
490
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
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
NC blocks in new format
6 TOOL CALL 12 Z
7 TCH PROBE 483 MEASURE TOOL
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 9/2015
TEETH: 0
TEETH: 1
Q340=1 ;CHECK
Q260=+100;CLEARANCE HEIGHT
Q341=1 ;PROBING THE TEETH