Machinery's Handbook, 31st Edition
1364
CNC MILLING OFFSETS Offsets for Milling
In CNC terms, the word offset means an adjustment. The primary purpose of offsets is to provide a link between the known information at the time of programming and the un- known situation at the time of setup and machining. The single most important purpose of offsets is to provide adjustments necessary to keep precise part dimensions. Such adjust ments allow corrections for tool wear, cutter length, or radius at the machine. Offsets can also be used for machining applications, for example, to use the same program for a rough ing contour and a finishing contour, or to use a tool with a different diameter or length. Offsets allow the programmer to virtually ignore tool dimensions.There are three groups of offsets for milling applications:
Work Offset = Offset to link machine zero and part zero. Tool Length Offset = Offset to link tool tip and part zero. Cutter Radius Offset = Offset to link tool radius and drawing dimensions.
Work Offset (G54 through G59).— Every CNC machine has a built-in location called the machine reference point (also known as machine zero or home position). By default, this location has coordinates of X0Y0Z0. The purpose of work offset is to establish the differ ence between machine zero and part zero. All machine axes can be set, although only X and Y axes are normally used.
Y
Machine X0Y0
G54 (X)
X
G54 (Y)
Part X0Y0
Machine table
Fig. 10. Work Offset Using G54. Work offset allows the programmer to use the dimensions from the drawing without considering the actual position of the part on the machine table. There are six standard work offsets defined by G54 through G59 commands, with additional sets available optionally. Fig. 10 shows the most commonly used work offset, G54. Note the direction is from machine zero to part zero, along an axis. A typical program entry combines the work offset with other data, for example: N3 G90 G54 G00 X__ Y__ S__ M03 T__ Tool Length Offset (G43, G44).— The tool length offset is a setting that specifies the dis tance between the tool reference point and part zero, along the Z-axis. Two methods are available—the preset method and the touch-off method . The preset method requires addi tional equipment and is used off-machine. The touch-off method is much simpler, and is done at the CNC machine. Each tool used in the program normally requires one tool length offset. A specific offset number is necessary to include with the G43 command. For example, N5 G43 Z0.1 H01 M08 G44 is used by only a very few programmers, for specific applications only. Fig. 11 shows typical tool length offset measurement using the touch-off method with G43 command.
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online