新代机床带刀尖跟随怎么输出G43.4 L2指令？

冰火2009

老师好，新代机床售后说需要支持G43.4 L2五联动平滑功能，请问后处理怎么修改呢？

G43.4 H01 L2
G43.4  L2  H01
H是刀号，跟随CAM刀具指定刀号输出

王榕慧

您好，这个可以自定义，记事本打开YSUG5.def文件，Ctrl+F 搜索BLOCK_TEMPLATE length_compensation 然后在H[$mom_tool_adjust_register]另起一行，输入Text[L2]
如截图所示：
BLOCK_TEMPLATE length_compensation
  {
       G_adjust[43.4]
       H[$mom_tool_adjust_register]
       Text[L2]
}

最终效果呈现：
%
(2025/06/03 15:10 DAY2)
(TIME=0.95 MIN)
(==========TOOL LIST START=========)
(刀号--刀补--径补--切削深度--刀具名称)
(T06 | H06 | D00 | 19.581 | EMC-6E)
(==========TOOL LIST END===========)
G17 G40 G49 G80
G00 G90 G53 Z0.
(CONTOUR_PROFILE)
G00 G90 G53 X0.Y0.
N1 T06 M06
S1000 M03
(EMC-6E D=6.00 R=0.00)
G49
G54
G00 G90 B1. C-180.
G68.2 X0.0 Y0.0 Z0.0 I-90. J1. K-90.
G53.1 P1
G00 G90 X-25.8412 Y20.644 M08
G49
G69
G43.4 H06 L2
G00 G90 X25.4955 Y-20.644 Z20.03 B1. C-180.
X25.9174 Z-4.1413
G01 X26.0964 Z-14.3958 F250.
X25.4815 Y-20.7788 Z-14.4066
X25.0313 Y-21.229 Z-14.4144
X24.8966 Y-21.844 Z-14.4168
Y-33.274
X24.8704 Y-33.6724 B.9984 C-181.8757
X24.8442 Y-34.0709 B.9979 C-183.7555
X24.8181 Y-34.4693 B.9984 C-185.6352
X24.7919 Y-34.8678 B1. C-187.5109
X24.714 Y-35.2589 B.9984 C-189.3845
X24.6362 Y-35.6501 B.9979 C-191.2622
X24.5583 Y-36.0413 B.9984 C-193.1398
X24.4804 Y-36.4325 B1. C-195.0135
X24.3521 Y-36.81 B.9984 C-196.8867