CNC FIXED CYCLE CODES Machinery's Handbook, 31st Edition
1367
Initial level - G98
R-level - G99 Z0
Z (Z-depth)
Fig. 14. Initial Level and R-level. All cycles are modal and are typically canceled by G80. Between the cycle call and the cycle cancel block, only the data that changed is programmed, usually the XY position, occasionally the R-level, or the Z-depth. The general and most commonly used format for all fixed cycles is: N__ G98 (G99) G__ X__ Y__ R__ Z__ P__ Q__ F__ where: N__ = block number, G__ = cycle number, X__Y__ = hole location, R__ = start position from where feed rate mode starts, Z__ = final depth, P__ = amount time delay (dwell) for G82 and G89, Q__ = either the depth of each peck for G83 and G73, or the shift amount for G76 and G87, F__ = cutting feed rate in feed per minute mode. Fixed Cycle (G81): The G81 code is used mainly for drilling, and has the following for mat see Fig. 15: N__ G99 (G98) G81 X__ Y__ R__ Z__ F__ In the G81 cycle, the tool rapids to XY location first, than to the R-level (feed plane). From that position it feeds to the depth, followed by a rapid retract to the R-level in G99 mode or the initial level, in G98 mode.
G98
G98
G99
G99
Z0
Z0
Dwell
Z-depth
Z-depth
Fig. 15. G81 Fixed Cycle. Fig. 16. G82 Fixed Cycle. Spot Drilling, Facing, Counterboring-sinking (G82): The G82 fixed cycle is used for spot drilling, spot facing, counter boring, countersinking, and any other operation where a dwell at the bottom of the hole is required. It has the following format Fig. 16: N__ G99 (G98) G82 X__ Y__ R__ Z__ P__ F__ All tool motions are identical to G81 cycle, with the added pause P__ (dwell). Pause is programmed in milliseconds (ms), without decimal a point. Its purpose is to smooth out
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online