WEIHONG ELECTRONIC Ncstudio, Programming Manual

Page: 26 / 74

上海维宏电子科技股份有限公司
Weihong Electronic Technology Co., Ltd.
Specialized, Concentrated, Focused 23
Tool Commands
G40, G41, G42 Cutter Radius Compensation
Command Format:
G41 D_
G42 D_
G40
Description:
G40: cutter radius compensation cancel
G41: left cutter compensation (the cutter offsets radius distance on the left side of cutter moving
direction)
G42: right cutter compensation (the cutter offsets radius distance on the right side of cutter
moving direction)
D_: parameter of G41/G42, i.e. tool compensation no. (D00~D07), denotes the radius
compensation value corresponding to the tool compensation list
The switch among cutter radius compensation planes must be executed when compensation is
off.
The establishment and cancel of cutter radius compensation can only use G00 or G01 command
instead of G02 or G03.
When using cutter radius compensation, the radius value must be measured accurately and then
saved into the memory as the cutter path offset (cutter radius value). D code is used in programming
to make cutter offset no. correspond to cutter radius value.
When G41 (G42) is used, the cutter will move a radius distance to the offset position. After the
execution of G41 (G42), the tool is immediately located to the perpendicular position of start position
of program block, and the value of movement depends on the offset.
T
o
o
l M
o
v
in
g
D
ir
e
c
tio
n
T
o
o
l M
o
v
in
g
D
ir
e
c
tio
n
Tool Rotary Direction
Offset
Left Compensation along
Tool Moving Direction
Tool Rotary Direction
Offset
Right Compensation along
Tool Moving Direction
(a) Left Compensation (b) Right Compensation
Fig. 4-13Cutter Compensation Direction