Machinery's Handbook, 31st Edition
CNC MILLING OFFSETS
1365
Z
Machine Z0
X
G43 Hxx
Part Z0
Hxx = Offset number - length
Machine table
Fig. 11. Tool Length of Offset. Cutter Radius Offset (G41, G42).— The cutter radius offset is an adjustment of the con tour toolpath from the part edge to the cutter center. It is also known as cutter radius com pensation or tool nose radius compensation for lathes (see page 1361). Point calculations based on the drawing dimensions are far more convenient and practi cal than programming coordinates to the center of a cutter. Fig. 12 illustrates a toolpath offset by the cutter radius. The toolpath generated on the basis of drawing dimensions may only be suitable for holes where the spindle centerline and hole centerline match. Such a toolpath cannot be used on a contour because the cutter centerline must be shifted— offset—away from the contour by the cutter radius. The purpose of the cutter radius offset is to provide automatic adjustment for the toolpath. This toolpath shifts the cutter center in such a way that the cutter edge is in constant contact with the programmed contour. This control generated toolpath is called an equidistant toolpath .
B/2
Y
X = tan(B/2) x R Y = tan(A/2) x R
X
X
R
Part
Dxx
A
A/2
B
Offset toolpath Programmed toolpath
Cutting tool
Y
Dxx = Offset number (radius)
R
Fig. 12. Cutter Radius Offset. Fig. 13. Manually Calculated Radius Offset. Programming to the center of the cutter requires tedious calculations for every point on the contour. Fig. 13 shows such a typical calculation. In addition, manually calculated center toolpaths cannot be adjusted at the machine. To activate a cutter radius offset, two preparatory commands are available—G41 (offset to the left) and G42 (offset to the right)—both left and right offsets are determined by the cutting direction. As more than one tool can use cutter radius offset, G41 or G42 has to be programmed together with corresponding offset number, using the D-address. Many con trol systems use only a single offset registry for both tool length offset and cutter radius offset. In such cases, the D-address must have a distinct number from the tool length offset, even if the addresses are different. Example: Tool 1 will be programmed as T01, using G43 H01 as the tool length offset, and G41 D51 as the cutter radius offset. G40 command cancels the cutter radius offset. Programming the cutter radius offset is relatively simple, but several rules have to be observed. The most important rule requires the G41/G42 command to be applied after completing the Z-depth motion and in G00 or G01 mode only (not on an arc).
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online