HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual
Page 115
TNC 426/TNC 425/TNC 415 B/TNC 407
4 - 1 8
4
Programming
Fig. 4.9:
These drilling positions are entered without radius
compensation
Y
X
Y
X
Tool movement with radius compensation: G41, G42
• Between two program blocks with different radius compensations you must program at least one block
without radius compensation (that is, with G40).
• Radius compensation does not come into effect until the end of the block in which it is first programmed.
• Whenever radius compensation is activated or cancelled, the TNC positions the tool perpendicular to the
programmed starting or end position. Position the tool at a sufficient distance from the first (or last) contour point
to prevent the possibility of damaging the contour.
The tool center moves to the left (G41) or right (G42) of the programmed
contour at a distance equal to the radius. “Left” and “right” are to be
understood as based on the direction of tool movement, assuming a
stationary workpiece.
R
Y
X
R
G41
R
Y
X
R
G42
Movement without radius compensation: G40
The tool center moves to the programmed coordi-
nates.
Applications:
• Drilling and boring
• Pre-positioning
Fig. 4.10:
The tool moves to the left
(G41)
or right
(G42)
of the path during milling
Shortening or lengthening single-axis movements: G43, G44
This type of radius compensation is only possible for single-axis move-
ments in the working plane. The programmed tool path is lengthened
(G43) or shortened (G44) by the tool radius.
Applications:
• Single-axis machining
• Occasionally for pre-positioning the tool, such as for cycle G47 SLOT
MILLING.
• You can enable G43 and G44 by programming a positioning block with an axis key.
• The machine tool builder can set machine parameters to inhibit programming of single-axis positioning blocks.