Machinery's Handbook, 31st Edition
CNC TURNING AND BORING 1373 The I and K parameters are not available on all machines. They control the amount of cut for semi finishing, the last continuous cut before final roughing motions. Newer controls require a two-block data entry for the G71 cycle, and the programming format is: G71 U__ R__; G71 P__ Q__ U__ W__ F__ S__ where the parameters in the first block are: U__ = depth of roughing cut, R__ = amount of retract from each cut. where the parameters in the second block are:
P__ = first block number of the finishing profile, Q__ = last block number of the finishing profile, U__ = stock amount for finishing on the X axis diameter, W__ = stock left for finishing on the Z axis, F__ = cutting feed rate per revolution, S__ = spindle speed in ft/min or m/min (cutting speed).
The U-address in the first block is independent of the U-address in the second block. The I and K parameters may be used only on some controls and the retract amount R is set by a system parameter. G71 cycle can be used for external roughing (turning) as well as for internal roughing (boring). The control system determines the type of machining by comparing the start point SP with the point P.
Cutting direction
Q
SP
SP to P direction is negative for external cutting
P P
internal cutting is positive for SP to P direction
SP
Q
Fig. 28. G71 Roughing Cycle. A typical program segment will have the following structure (tool 01 used): N1 G20 T0100; N2 G96 S__ M03; N3 G00 X__ Z__ T0101 M08 (START POINT SP); N4 G71 U0.15 R0.04; N5 G71 P6 Q11 U0.06 W0.005 F0.015; N6 G00 X__ (POINT P BLOCK); N7 ..; N8 … N9 … N10 … N11 U0.2 (POINT Q BLOCK); N12 G28 U0 W0; N13 M30; %; G72 Roughing cycle is similar, but applies for vertical direction of cut. There are two types of G71 and G72—Type I and Type II. Type I does not allow for a change of direction, whereby Type II allows for a change in one axis only. Repeated Finish Counting (G73): G73 pattern repeating cycle is used to machine a fin ishing contour repeatedly, by a given distance, in specified number of steps. Finish Cycle (G70): G70 is programmed after G71, G72, and G73 as a finishing cycle, and has a simple format: N__ G70 P__ Q__ F__ S__
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online