HEIDENHAIN ITNC 530 - CYCLE PROGRAMMING User Manual page 504

Cycle parameters
U 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 in the
central tool file TOOL.T by the delta value DR = 0. If
you wish to inspect a tool, the TNC compares the
measured radius with the tool radius R that is stored
in TOOL.T. It then calculates the positive or negative
deviation from the stored value and enters it into
TOOL.T as the delta value DR. The deviation can also
be used for Q parameter Q116. If the delta value is
greater than the permissible tool radius tolerance for
wear or break detection, the TNC will lock the tool
(status L in TOOL.T).
U
Parameter number for result?: Parameter number in
which the TNC stores the status of the
measurement:
0.0: Tool is within the tolerance
1.0: Tool is worn (RTOL exceeded)
2.0: Tool is broken (RBREAK exceeded). If you do not
wish to use the result of measurement within the
program, answer the dialog prompt with NO ENT.
U 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 MP6540).
Input range -99999.9999 to 99999.9999, alternatively
PREDEF
U Cutter measurement? 0=No / 1=Yes: Choose whether
the control is also to measure the individual teeth
(maximum of 99 teeth)
504
Example: Measuring a rotating tool for the first
time; old format
6 TOOL CALL 12 Z
7 TCH PROBE 32.0 TOOL RADIUS
8 TCH PROBE 32.1 CHECK: 0
9 TCH PROBE 32.2 HEIGHT: +120
10 TCH PROBE 32.3 PROBING THE TEETH: 0
Example: Inspecting a tool and measuring the
individual teeth and saving the status in Q5; old
format
6 TOOL CALL 12 Z
7 TCH PROBE 32.0 TOOL RADIUS
8 TCH PROBE 32.1 CHECK: 1 Q5
9 TCH PROBE 32.2 HEIGHT: +120
10 TCH PROBE 32.3 PROBING THE TEETH: 1
Example: NC blocks in new format
6 TOOL CALL 12 Z
7 TCH PROBE 482 TOOL RADIUS
Q340=1 ;CHECK
Q260=+100 ;CLEARANCE HEIGHT
Q341=1 ;PROBING THE TEETH
Touch Probe Cycles: Automatic Tool Measurement