Cycle Parameters - HEIDENHAIN TNC 620 User Manual

18
Touch Probe Cycles: Automatic Tool Measurement
18.5 Measuring tool radius (Cycle 482)

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 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).
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 (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.
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)
488
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
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
NC blocks in new format
6 TOOL CALL 12 Z
7 TCH PROBE 482 TOOL RADIUS
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