HEIDENHAIN CNC Pilot 4290 - Manual (Page 148)

4 DIN PLUS 136
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.
Note on programming G83
■ G83 must be alone in a block.
■ G83 must not be programmed with K variables.
■ G83 must not be nested, not even by calling subprograms.
Oversizes:
■ G57 oversizes
■ are calculated with algebraic sign (oversizes are therefore
impossible for inside contour machining)
■ G58 oversizes: are taken into account if you are working with TRC
■ G57 and G58 oversizes stay in effect after cycle end
Cycle run
1 Start the cycle execution from the current tool position.
2 Advance by the infeed distance defined in I and K.
3 Execute 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 Return on a diagonal path.
5 Repeat 2 to 4 until the contour target point has been reached.
6 Return to the starting point of the cycle.
Parameters
X/Z: Contour target point (X diameter) - default: Transfer the last X/Z
coordinate
lI: Maximum infeed in X direction (radius) – default: 0
K: Maximum infeed in Z direction – default: 0
■ Cutter radius compensation: Not
active. – You can program the TRC
separately with G40..G42.
■ Safety clearance After every step:
1 mm.
Danger of collision!
After each pass, the tool returns on a
diagonal path before it advances for the
next pass. If required, program an
additional rapid traverse path to avoid a
collision.
4.7 T
u
rning Cy
cles