Measuring Tool Length (Cycle 31 Or 481, Din/Iso: G481, Option 17); Cycle Run - HEIDENHAIN TNC 620 User Manual

18
Touch Probe Cycles: Automatic Tool Measurement | Measuring tool length (Cycle 31 or 481, DIN/ISO: G481,
18.4 Measuring tool length (Cycle 31 or 481,
DIN/ISO: G481, Option 17)

Cycle run

To measure the tool length, program the measuring cycle TCH
PROBE 31 or TCH PROBE 481 (see "Differences between Cycles
31 to 33 and Cycles 481 to 483"). Via input parameters you can
measure the length of a tool by three methods:
If the tool diameter is larger than the diameter of the measuring
surface of the TT, you measure the tool while it is rotating.
If the tool diameter is smaller than the diameter of the
measuring surface of the TT, or if you are measuring the length
of a drill or spherical cutter, you measure the tool while it is at
standstill.
If the tool diameter is larger than the diameter of the measuring
surface of the TT, you measure the individual teeth of the tool
while it is at standstill.
Cycle for measuring a tool during rotation
The control determines the longest tooth of a rotating tool by
positioning the tool to be measured at an offset to the center of the
touch probe and then moving it toward the measuring surface of
the TT until it contacts the surface. The offset is programmed in the
tool table under Tool offset: Radius (TT: R_OFFS).
Cycle for measuring a tool during standstill (e.g. for drills)
The control positions the tool to be measured over the center of
the measuring surface. It then moves the non-rotating tool toward
the measuring surface of the TT until contact is made. To activate
this function, enter zero for the tool offset: Radius (TT: R_OFFS) in
the tool table.
Cycle for measuring individual teeth
The TNC pre-positions the tool to be measured to a position at
the side of the touch probe head. The distance from the tip of
the tool to the upper edge of the touch probe head is defined
in offsetToolAxis. You can enter an additional offset with tool
offset: Length (TT: L_OFFS) in the tool table. The TNC probes
the tool radially during rotation to determine the starting angle for
measuring the individual teeth. It then measures the length of each
tooth by changing the corresponding angle of spindle orientation.
To activate this function, program TCH PROBE 31 = 1 for CUTTER
MEASUREMENT.
532
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
Option 17)