HEIDENHAIN MANUALplus 4110 - Manual (Page 321)

HEIDENHAIN MANUALplus 4110 321
6.12 Simple T
u
rn
ing Cy
cles
Simple contour repeat cycle G83
G83 repeatedly executes the machining cycle programmed in the sub-
sequent blocks. The machining cycle may contain simple traverse paths
or cycles (without contour definition). G80 ends the machining cycle.
"X, Z" define the starting point of the contour. G83 starts the cycle
execution from the current tool position. Before each pass, the tool
advances by the infeed distance defined in "I, K." The control then
executes the machining operation which is programmed in the blocks
after G83, taking the distance from the tool position to the contour
starting point as an "oversize." G83 repeats this operation until the
"starting point" is reached.
G83 is used for:
„ Machining contour-parallel workpiece sections (roughing of pre-
shaped workpiece blanks).
„ Repeating machining operations (for example, for slot-cutting).
Parameters
 X starting point (diameter value)
 Z starting point
 I maximum infeed in X direction (I is entered without the algebraic
sign)
 K maximum infeed in Z direction (K is entered without the algebraic
sign)
Note on the execution of the cycle:
„ If the number of infeeds differs for the X and Z axes, the tool first
advances in both axes with the programmed values. As soon as the
target dimension is reached in one axis, the tool no longer advances
in this axis.
„ MANUALplus automatically determines the cutting and infeed
directions from the current tool position relative to the starting point
of the contour area.
„ Tool position at the end of the cycle: Starting point of contour
Example: G83
%83.nc
[G83]
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G83 X80 Z0 I4 K0.3
N4 G0 X80 Z0
N5 G1 Z-15 B-1
N6 G1 X102 B2
N7 G1 Z-22
N8 G1 X90 Zi-12 B1
N9 G1 Zi-6
N10 G1 X100 A80 B-1
N11 G1 Z-47
N12 G1 X110
N13 G0 Z2
N14 G80
END
„ G83 must not be nested, not even by calling
subprograms.
„ At the start of the cycle, the tool must be located outside
the defined contour area.
„ Cutter radius compensation: is not carried out—You
can program TRC separately.
„ Oversizes: Oversizes programmed with G57 are taken
into account. An oversize programmed with G58 is
accounted for, provided that the TRC function is active.
The oversizes remain in effect after execution of the cycle.
Danger of collision!
After each pass, the tool returns on a diagonal path before
it advances for the next pass. If there is danger of collision,
you must program an additional path of rapid traverse to
avoid a collision.