Simple Contour Repeat Cycle G83 - Simple Turning Cycles - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | G codes from previous controls
Simple contour repeat cycle G83 – simple turning
cycles
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.
Parameters:
X: Destinat. point of contour (diameter; default: Load the last X
coordinate)
Z: Destinat. point of contour (default: Load the last Z
coordinate)
I: Max. approach
K: Max. approach
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 nested, not even by calling subprograms
Tool radius compensation is inactive.
Safety clearance after each step: 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
Remains effective after cycle end
Danger of collision!
After each cut, the G83 function pre-positions the tool along the
shortest path (diagonally) for the next infeed. Danger of collision
during pre-positioning!
Check the NC program using the verification graphics in the
Simulation submode
Program an additional rapid traverse path to a safe position if
required
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
NOTICE
TRC
4
501