Machinery's Handbook, 31st Edition
1362 CNC PROGRAMMING CODES non-cutting and non-productive motion available to the CNC programmer. Its single pur- pose is to move the cutter from one location to another at the highest speed possible, typi- cally between actual cuts. CNC manufacturers determine the maximum rapid motion rate.
Actual
45
Y-motion
X-motion
Fig. 5. Rapid Motion G00. Fig. 5 shows the effect of programmed and actual rapid motion applied on a machining center. As both X and Y axes have the same rapid rate—and the actual toolpath is not important—the resulting motion starts at 45 degrees. When one axis reaches its destination, the other axis continues as a single axis motion. Some machines can produce rapid motion as programmed. Linear Interpolation (G01).— In linear interpolation mode (programmed in G01 mode with a cutting feed rate in effect), the tool moves along a linear path, directly from one point to the next (traversing the shortest distance). This is a major departure from the rapid motion mode (programmed in G00 mode), where the shortest distance is disregarded and the result is the fastest motion available. The word interpolation defines a mathematical process that translates into synchronized feed rate for all programmed axes. This is done by the control system automatically. The programming command for linear interpolation is G01 (modal), which cancels any other active motion command. Feed Rate is required with G01 and its selection is based on cutting conditions. Circular Interpolation (G02, G03).— Circular interpolation applies to a cutting tool path moving along an arc or a circle. An arc (circle) can be programmed directly, without linear approximation. The cutting motion along an arc is two-dimensional and always takes place in a single plane. No arc or circle exists as a three-dimensional entity (it be- comes a helix). Depending on the required outcome, the desired plane can be defined using one of three specific G-codes ( Fig. 6- Fig. 8):
G17 = XY plane—arc/circle uses XY coordinates at a given Z-depth G18 = ZX plane—arc/circle uses ZX coordinates at a given Y-depth G19 = YZ plane—arc/circle uses YZ coordinates at a given X-depth
G03
G03
G03
G02
G02
G02
Mathematical Definition of Planes
G03
G02
G03
G02
G03
G02
Fig. 6. Planes on a CNC Vertical Machining Center.
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online