Machinery's Handbook, 31st Edition
1366 CNC MACHINING HOLE Example: N44 G01 Z-0.5 F15.0; N45 G41 X0.25 D51 F20.0; N46 Y__ Cutter radius offset uses a so called look-ahead type of radius compensation. During program execution, the control stores the next motion block in the buffer—it “looks ahead” in the program in order to compensate correctly and consistently. Machining Holes Virtually all applications of CNC machining include machining holes. Regardless of what type of machining takes place at a single hole location, there are similarities import ant to CNC programming, particularly for CNC milling machines and machining centers. In the majority of applications, machining holes is not a complicated procedure. The only cutting tool motion that takes place is along the Z axis, after a required XY location has been applied. This type of machining is commonly known as point-to-point machining and is applied to operations such as drilling, spot drilling, spot facing, counter-boring, counter-sinking, tapping, boring, and reaming. Each toolpath step relating to a particular machining operation on a hole is always consis tent and can be preset within the control system software (built-in software routine). This is the basis for shortening programming holes by using fixed cycles. As the name suggests, these cycles contain an internal set order of tool motions and cannot be changed. Table 4 shows symbols and abbreviations used in the following cycle descriptions. Table 4. Fixed Cycle Descriptions Symbol Description
Rapid Motion and Direction Cutting Motion and Direction Manual Motion and Direction Boring Bar Shift and Direction Programmed Coordinate (XY) Depth of Peck / Shift Amount Clearance Value (built in) Spindle Rotation Direction Oriented Spindle Stop
Q d
CW / CCW
OSS
DWELL Dwell Function Executed Fixed Cycles.— “Fixed cycles” sometimes called canned cycles, are series of preset se- quences of toolpath motions, allowing consecutive motions to be performed with a single block of program. Typical fixed cycles are: Table 5. Fixed Cycle Codes G-Code Description G-Code Description G81 Drilling cycle G86 Boring cycle G82 Drilling cycle with dwell (spot drilling cycle) G76 Fine boring cycle G83 Deep hole drilling cycle (peck drilling cycle) G87 Back boring cycle G73 Chip-breaking cycle G88 Boring cycle (with manual action)
G84 Right hand tapping cycle G74 Left hand tapping cycle
G89 Boring cycle G80 Fixed cycle cancel
G85 Boring cycle In addition, two preparatory commands are also used with fixed cycles see Fig. 14: G98 Retract to initial level G99 Retract to R-level
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online