HEIDENHAIN CNC PILOT 640 User Manual page 337

DIN/ISO programming | Contour-based turning cycles
B: TRC/MRC switch on – type of tool radius compensation
0: Automatic
1: Tool left (G41)
2: Tool right(G42)
3: Automatic w/o tool compens.
4: W/o tool compens. left (G41)
5: W/o tool compens. left (G42)
HR: Main machining direction
0: auto
1: +Z
2: +X
3: –Z
4: –X
The control uses the tool definition to distinguish between external
and internal machining.
Undercuts are machined if they are programmed and if tool geometry
permits.
Feed rate reduction
For chamfers and rounding arcs:
Feed rate is programmed with G95-Geo: No automatic feed rate
reduction
Feed rate is not programmed with G95-Geo: Automatic feed rate
reduction. Each chamfer/rounding is therefore machined with at
least three revolutions.
For chamfers/rounding arcs which, as a result of their size, are
machined with at least three revolutions, the feed rate is not
reduced automatically.
For circular elements:
For small circular elements, the feed rate is decreased until every
element is machined with at least four spindle revolutions. You
can switch this feed rate reduction off with O.
The tool radius compensation (TRC) results under certain
conditions to a feed rate reduction for circular elements. You can
switch this feed rate reduction off with O.
Further information:
A G57 oversize enlarges the contour (also inside
contours).
A G58 oversize
>0: Enlarges the contour
<0: Reduces the contour
G57/G58 oversizes are deleted after cycle end
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
"Fundamentals", Page 302
4
337