HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 234)

234
4.21 Simple T
u
rn
ing Cy
cles
Simple contour repeat cycle G83
G83 carries out the functions programmed in the following blocks
(simple traverses or cycles without a contour definition) more than
once. G80 ends the machining cycle.
If the number of infeeds differs for the X and Z axes, the tool first
advances in both axes with the programmed values. The infeed is set
to zero if the target value for one direction is reached.
Programming:
„ G83 is alone in the block
„ G83 must not be programmed with K variables
„ G83 must not be nested, not even by calling subprograms
Example: 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
Parameters
X Contour target point (diameter)—(default: Load the last X
coordinate)
Z Contour target point—(default: Load the last Z coordinate)
I Maximum infeed in X direction (radius)—(default: 0)
K Maximum infeed in Z direction (default: 0)
„ The tool radius compensation is not active. You can
program the TRC separately with G40 to G42.
„ Safety clearance after each pass: 1 mm
„ A G57 oversize
„ Is calculated with algebraic sign (oversizes are
therefore impossible for inside contour machining)
„ Remains effective after cycle end
„ A G58 oversize
„ Is taken into account if you work with TRC
„ Remains effective after cycle end
Cycle run
1 Starts the cycle execution from the current tool position.
2 Advances by the infeed distance defined in I and K.
3 Executes the machining operation which is programmed in the
blocks after G83, taking the distance from the tool position to the
contour start point as an “oversize.”
4 Returns on a diagonal path.
5 Repeats 2 to 4 until the contour target point has been reached.
6 Returns to the starting point of the cycle.