达风数控 DF-200T DF-300T 车床数控系统 用户手册

DF-200T/DF-300T

车床数控系统

用 户 手 册

南京达风数控技术有限公司

（第六版）

严谨地做好产品的每个细节

积极敏锐地跟踪先进技术

热诚有效地服务于每个客户

南京达风数控技术有限公司

公司地址：南京市江宁区科宁路789号

公司网址：

技术服务：151****1245,152****6577

DF-200T/DF-300T 用户使用手册 南京达风数控技术

第一章 概述··················································································································9

第二章 编程篇············································································································13

2.1 编程概要·······································································································13

2.1.1 轴定义································································································13

2.1.2 机械零点·····························································································13

2.1.3 工件坐标系设定·················································································13

2.1.4 直径指定和半径指定·········································································17

2.1.5 坐标单位及范围·················································································17

2.1.6 编程坐标值·························································································18

2.1.7 初态，模态·························································································19

2.1.8 插补功能·····························································································19

2.1.9 进给功能·····························································································20

2.1.10 切削速度—主轴功能·······································································21

2.1.11 各种加工时选用的刀具——刀具功能············································21

2.1.12 各种功能操作指令——辅助功能···················································22

2.1.13 刀具补偿功能···················································································22

2.2 G功能·············································································································22

2.2.1 定位（G00）······················································································24

2.2.2 直线插补（G01）··············································································25

2.2.3 倒角功能·····························································································26

2.2.4 圆弧插补（G02，G03）···································································28

2.2.5 暂停或准停（G04）··········································································31

2.2.6 准停定位（G09）··············································································32

2.2.7 自动返回机械零点（G28）······························································32

2.2.8 自动返回程序零点（G26）······························································33

2.2.9 跳段功能（G31）··············································································33

2.2.10单刀螺纹（G32）·············································································34

2.2.11 刚性攻丝（G33）············································································36

2.2.12 变螺距螺纹切削（G34）································································37

2.2.13端面螺纹（G35）·············································································37

2.2.14 螺纹切削单一循环（G92）····························································38

2.2.15 复合型螺纹切削循环（G76）························································42

2.2.16 公制螺纹切削复合循环（G86）····················································45

1

DF-200T/DF-300T 用户使用手册 南京达风数控技术

2.2.17 英制螺纹切削复合循环（G87）····················································46

2.2.18 刀尖半径补偿（G40，G41，G42）···············································46

2.2.19 坐标系设定（G50）········································································46

2.2.20 每分进给（G98）············································································47

2.2.21 每转进给（G99）············································································47

2.2.22 恒线速控制（G96，G97）·····························································48

2.2.23外圆，内圆车削循环（G90）·························································50

2.2.24端面车削循环（G94）·····································································54

2.2.25固定循环使用其他说明事项：························································57

2.2.26 端面深孔加工循环（G77）····························································58

2.2.27端面深孔或割槽加工循环（G74）··················································60

2.2.28 外圆/内圆切槽/割断循环（G75）··················································62

2.2.29外圆/内圆粗车循环（G71）····························································65

2.2.30端面粗车循环（G72）·····································································68

2.2.31 封闭切削循环G73··········································································71

2.2.32 精加工循环（G70）········································································74

2.3 主轴功能(S功能)···························································································75

2.3.1 主轴速度指令·····················································································75

2.4 刀具刀补功能·······························································································75

2.4.1 换刀过程（电动回转刀架）·····························································76

2.4.2 换刀相关参数·····················································································76

2.4.3 刀补功能·····························································································77

2.4.4 试切对刀·····························································································77

2.5 辅助功能·······································································································77

2.5.1 M00——暂停······················································································79

2.5.2 M01——条件暂停··············································································79

2.5.3 M30——程序结束··············································································79

2.5.4 M03——主轴正转··············································································79

2.5.5 M04——主轴反转··············································································80

2.5.6 M05——主轴停止旋转······································································80

2.5.7 M08 M09——冷却液控制··································································81

2.5.8 M10 M11——工件夹紧，松开控制··················································82

2.5.9 M78 M79——尾座进，尾座退控制··················································82

2

DF-200T/DF-300T 用户使用手册 南京达风数控技术

2.5.10 M20，M21，M22——输出口信号控制··········································82

2.5.11 M31——工件计数············································································83

2.5.12 M32 M33——润滑供油开，供油停················································83

2.5.13 M91 M92——程序跳转指令····························································83

2.5.14 M98 M99——子程序调用及子程序返回········································84

2.5.15 M26，M27，M28——旋转轴(Y轴)转速控制································85

2.5.16 M35 ——自动重复上料功能···························································85

2.5.17 M19——主轴准停控制····································································86

2.5.18 辅助机能代码调用子程序·······························································86

2.6 程序的构成···································································································86

2.6.1 程序····································································································86

2.6.2 程序名································································································89

2.6.3 程序段号·····························································································89

2.6.4 字和地址·····························································································89

2.6.5 程序结束·····························································································90

2.7 自动加减速···································································································90

2.7.1 程序段拐角处的速度控制·································································91

第三章 操作篇············································································································93

3.1 操作面板说明·······························································································93

3.1.1 显示和操作面板·················································································93

3.1.2 页面显示选择用按键·········································································94

3.2 位置显示画面·····························································································100

3.3 安全操作·····································································································104

3.3.1 急停··································································································104

3.3.2 超程··································································································105

3.3.3 报警处理···························································································105

3.4 手动操作·····································································································105

3.4.1 手动返回机床零点···········································································105

3.4.1.1 操作方法·······························································································105

3.4.1.2 返回机床零点的相关参数意义和注意事项·········································106

3.4.2 手动连续进给操作···········································································107

3.4.2.1 操作方法·······························································································107

3.4.2.2 手动快速进给设定················································································108

3

DF-200T/DF-300T 用户使用手册 南京达风数控技术

3.4.3 增量进给···························································································108

3.4.4 手轮进给···························································································108

3.4.5 返回程序零点···················································································109

3.4.6 手动辅助机能操作···········································································109

3.5 自动运行·····································································································111

3.5.1 运行方式···························································································111

3.5.2 自动运转的执行···············································································113

3.5.3 自动运转的停止···············································································113

3.5.4 进给暂停和主轴停止的顺序控制功能（三位开关功能）············113

3.5.5 进给速度倍率调节···········································································114

3.5.6 快速倍率调节···················································································114

3.6 试运转·········································································································114

3.6.1 机床锁功能·······················································································115

3.6.2 单段执行···························································································115

3.7 MDI执行方式·······························································································115

3.7.1 传统MDI方式···················································································115

3.7.2 快捷MDI方式···················································································117

3.8 程序存储、编辑··························································································118

3.8.1 程序存储、编辑操作前的准备·······················································118

3.8.2 建立新程序·······················································································118

3.8.3 程序名检索·······················································································119

3.8.4 程序的删除·······················································································119

3.8.5 删除全部程序···················································································120

3.8.6 程序复制···························································································120

3.8.7 程序的输出·······················································································120

3.8.8 程序段号检索···················································································121

3.8.9 字的插入、修改、删除···································································121

3.8.9.1 将光标定位到要编辑的字上································································121

3.8.9.2 字的插入·······························································································123

3.8.9.3 字的修改·······························································································125

3.8.9.4字的删除································································································125

3.8.10 存储程序的个数和存储容量·························································125

3.8.11 程序存储器信息显示·····································································125

4

DF-200T/DF-300T 用户使用手册 南京达风数控技术

3.9 刀具补偿·····································································································126

3.9.1 换刀时刀补的原理···········································································128

3.9.2 刀补和工件坐标系建立的方法·······················································129

3.9.2.1 X向、Z向单独对刀···············································································129

3.9.2.2 X向、Z向同时记忆对刀·······································································130

3.9.3 刀补修调（刀具磨损补偿）···························································131

3.9.4 刀补清零···························································································132

3.10 诊断···········································································································132

3.10.1 系统输入口状态的显示·································································133

3.10.2 系统输出口状态的显示·································································133

3.10.3 轴脉冲计数显示·············································································133

3.10.4 主轴编码器线数诊断显示·····························································133

3.10.5 主轴变频器模拟电压显示·····························································134

3.10.6 累计加工计件显示·········································································134

3.10.7 输入口信号定义显示·····································································134

3.10.8 输出口信号定义显示·····································································135

3.11 报警显示···································································································137

3.12 设置功能···································································································137

3.12.1参数开关及程序开关状态设置······················································138

3.12.2 当前时间设置·················································································138

3.12.3 密码设置·························································································139

3.12.4 格式化程序存储器·········································································139

3.13 参数···········································································································140

3.13.1 参数的显示·····················································································140

3.13.2 参数的设定·····················································································142

3.13.3 参数出厂值、参数备份、参数恢复等操作··································143

3.13.3.1 参数恢复为出厂值··············································································143

3.13.3.2 参数备份·····························································································144

3.13.3.3 参数备份内容恢复为当前参数··························································144

3.14 U盘操作·····································································································144

3.14.1 U盘操作界面说明···········································································144

3.14.2 如何将系统中的程序文件导出到U盘···········································145

3.14.3 如何将参数文件导出到U盘··························································145

5

DF-200T/DF-300T 用户使用手册 南京达风数控技术

3.14.4如何将U盘文件导入到系统···························································145

3.14.5如何将U盘中的参数文件导入到系统············································146

3.15 图形模拟显示和操作················································································146

3.15.1 图形模拟操作说明·········································································146

第四章 安装连接······································································································148

4.1 系统结构及安装··························································································148

4.1.1 系统组成···························································································148

4.1.2 系统安装连接···················································································148

4.1.3 数控系统安装尺寸图·······································································149

4.2设备间连接··································································································150

4.2.1系统接口框图和说明········································································150

4.2.2 系统与驱动单元的连接（XS30、XS31、XS33）·························151

4.2.3 主轴编码器的连接（XS32）··························································155

4.2.4 手轮接口（XS38）··········································································156

4.2.5 RS232－C串行通信口（XS36）······················································157

4.2.6 主轴模拟量接口（XS37）······························································158

4.3 输入输出接口·····························································································158

4.3.1 机床输入/输出接口管脚定义··························································158

4.3.2输入口·······························································································163

4.3.3 输出口······························································································167

第五章 常用功能使用说明·······················································································170

5.1 电子齿轮比参数设定··················································································170

5.2 线性加减速时间常数··················································································171

5.3 主轴设定·····································································································171

5.4卡盘控制······································································································173

5.5 手持手轮单元·····························································································175

5.6 尾座控制·····································································································176

5.7 润滑控制·····································································································176

5.8 软件限位设定·····························································································177

5.9 反向间隙补偿·····························································································177

第六章 刀补C功能····································································································179

6.1 刀补C功能基本概念···················································································179

6.1.1 假想刀尖概念···················································································179

6

DF-200T/DF-300T 用户使用手册 南京达风数控技术

6.1.2 假想刀尖的方向···············································································181

6.1.3 补偿值的设置···················································································184

6.1.4 刀具与工件的相对位置···································································184

6.1.5 内侧、外侧·······················································································186

6.1.6 G41、G42及G40的代码格式··························································187

6.2 刀补具体补偿情况······················································································187

6.2.1 刀尖半径补偿具体轨迹分解···························································187

6.2.2 刀补进行中变更补偿方向·······························································195

6.2.3 刀补暂时取消···················································································197

6.2.4 刀补中含有非移动指令···································································199

6.2.5 刀补干涉检查···················································································201

6.2.6 G90/G94代码中的刀尖半径补偿····················································203

6.2.7 G70代码中的刀尖半径补偿····························································205

6.3 刀补C的注意事项·······················································································205

6.4 刀补C加工范例···························································································206

附录1：DF-200T参数一览表···················································································209

1．位参数··········································································································209

2．数据参数······································································································214

附录2：常用参数按功能分类··················································································228

1．X/Z/Y轴控制部分························································································228

2．刀架控制······································································································229

3．螺纹功能参数······························································································230

4．回机械零点功能···························································································232

5．系统报警······································································································233

附录3：报警列表·····································································································234

1．报警列表······································································································234

2．常见报警的解除方法···················································································240

附录4：系统升级使用说明······················································································243

1．U盘方式升级数控系统软件········································································243

2．U盘方式升级开机界面················································································243

附录5：丝杠螺距误差补偿······················································································244

1．螺距补偿功能······························································································244

2．螺距补偿参数的设定步骤···········································································244

7

DF-200T/DF-300T 用户使用手册 南京达风数控技术

3．螺距误差补偿注意事项···············································································244

4．螺距误差补偿举例·······················································································245

附录6：急停复位时自动关闭输出口功能······························································246

1．

复位时关闭输出口定义··············································································246

2．

急停时关闭输出口定义··············································································247

附录7：外接按钮功能使用······················································································248

8

DF-200T/DF-300T 用户使用手册 南京达风数控技术

第一章

概述

DF-200T数控系统为数控车床专用控制系统，该系统应用32位高速CPU、超大规模可编程集成芯片构成控制核心,μm级精度控制，480x234点阵TFT真彩液晶显示,中文操作界面，操作简单直观。具有U盘管理功能，便于参数和程序的导入导出，以及系统软件升级。系统可配置三相混合式步进驱动器或数字交流伺服驱动器。通过编程可以实现快速定位、直线插补、圆弧插补、螺纹循环、攻丝循环、深孔钻循环、跳转循环加工、复合循环加工、变频主轴控制/伺服主轴控制、电动刀架/排刀刀架/液压刀架、扩展输入输出口控制等功能，具有很高的性价比。

主要技术指标：

功 能

控制轴

描 述

控制轴数

联动轴数

最小设定单位

2轴或3轴

规 格 指 标

2轴或3轴 （X、Z、Y轴）

X：0.001mm Z：0.001mm Y：0.001mm

0.001mm

±99999.999mm

60000mm/min

0.0001mm～500.000mm

直线，前加减速

0～150%

Fo～100%,Fo由参数设定

X,Y,Z；手动进给速度按键设定

三种回零：方式B（Z脉冲中断方式），方式C（回零定位开关），方式A（浮动零点）

快速回加工起始点

进给当量0.001mm,0.01mm,0.1mm，1mm

倍率：x1,x10,x100；轴选：X，Z，Y；按键或外部输入口选控倍率和轴选

直线、圆弧、螺纹循环、攻丝循环、钻孔循环、外圆、端面复合循环等功能

大容量，2M字节

9

输入指令

最小移动单位

最大指令值

最大移动速度

螺纹导程

进给

自动加减速

进给速度倍率

快速速度倍率

手动连续进给

返回机床零点

手动

返回程序零点

单步增量进给

手轮进给

插补 定位，插补功能

存储及编辑 程序存储容量

DF-200T/DF-300T 用户使用手册 南京达风数控技术

功 能 描 述

存储程序个数

程序编辑

参数存储

液晶显示

显示

位置，程序，刀补，报警，诊断，参数，设置，显示内容丰富，直观

U盘

程序导入导出

U盘功能

参数导入导出

系统U盘升级

串口通讯 RS232

输入口

输出口

主轴功能

M，S，T机能

刀具功能

有

有

有

19200bps，用于程序的输入输出以及系统升级

32路开关量，光电隔离输入

32路开关量输出（OC输出）

变频器模拟量控制或S1～S4档位控制；主轴模拟量输出倍率可调0～150%；

刀位号：T01～T08，刀补号：01～16；电动刀架，排刀刀架或专用刀架；运行中修整刀补值；程序控制动态刀补补偿。

辅助T功能

辅助M功能

MDI方式

补偿机能

固定循环功能

快捷MDI方式

传统MDI输入方式

补偿功能

G90

G94

G92

G86，G87

G70

G71

G72

有，特定T代码执行特定子程序

有，特定M代码执行特定子程序

在位置界面下直接输入要执行的程序段

进入MDI输入界面，按字段输入

刀具补偿、反向间隙补偿、丝杠螺距误差补偿

外圆，内圆车削循环（圆柱面，圆锥面）

端面车削循环（平面，锥面）

螺纹循环（直、锥螺纹，公、英制，单头、多头螺纹、任意螺纹切入角）

螺纹复合循环

精车循环

外圆粗车循环

端面粗车循环

480个

插入，修改，删除，复制

参数恢复，备份，恢复出厂值，参数U盘导入导出

7英寸，TFT真彩显示

规 格 指 标

10

DF-200T/DF-300T 用户使用手册 南京达风数控技术

功 能

G73

G74

G75

G76

G33

其他螺纹功能

倒角功能

信号跳转机能

G32

G34

G01 I/K/R

G31

描 述

封闭粗车循环

端面钻孔循环

切槽或割断循环

螺纹复合循环

刚性攻丝循环

单刀螺纹功能

变螺距螺纹功能

45度角或圆弧角

规 格 指 标

进给运行中遇信号跳转

程序段自动速度过渡功能，过渡曲线自动动态调整

程序或部分程序段进行无限次循环加工或有限次循环加工

根据外部条件信号，跳转到程序的不同指令流程执行。段平滑过渡 G61，G64

无限、有限循环功能

程序条件跳转机能

扩展输出口控制

外部条件等待机能

输出自动重复控制功能

旋转轴控制（Y轴）

M92

M91

M20,M21,M22 扩展输出口电平输出方式或脉冲输出方式控制

M01 等待外部有效信号输入，超时报警

适用于自动上下料的功能，检测上料状态，重复连续上料

进行旋转速度和方向设定，结合G09（快速准停）用于旋转停止后快速定位分度

内卡、外卡，脚踏开关输入和按键操作

持续润滑、间歇润滑

开机加工计时

单次开机计件和累计加工计件

有

有

有

M35

M26,M27,M28

卡盘功能

润滑功能

计时功能

其他功能

计件功能

三位开关功能

运行、暂停、报警状态指示灯功能

外部开关信号启动、暂11

DF-200T/DF-300T 用户使用手册 南京达风数控技术

功 能 描 述

停程序运行

输入口状态 有

规 格 指 标

输出口状态显示和控制 有，在诊断界面中可对输出口进行开关控制

轴移动脉冲数

诊断显示

主轴编码器线数

主轴模拟量电压

有

有

有

输入口接线和端口定义 有

输出口接线和端口定义 有

正、负方向硬件限位

安全机能

正、负方向软件限位

紧急停止

用户自定义报警

调试机能

驱动器接口

有

有

有

有，两路自定义报警输入

单段运行、机床锁功能 有

交流伺服或三相混合驱动器

控制方式：“方向+脉冲”或“双脉冲”模式

12

DF-200T/DF-300T 用户使用手册 南京达风数控技术

第二章

编程篇

2.1 编程概要

2.1.1 轴定义

DF-200T车床数控系统具有3轴控制功能，系统使用X轴，Z轴组成的直角坐标系进行定位和插补运动，Y轴用于进行伺服主轴控制或其他回转轴控制。

X轴为水平面的前后方向，Z轴为水平面的左右方向。向工件靠近的方向为负方向，离开工件的方向为正方向。如图示，前后刀座的坐标系，X方向正好相反，而Z方向是相同的。在以后的图示和例子中，用前刀座来说明编程的应用，而后刀座车床系统可以类推。

图示：前刀座的坐标系

图示：后刀座的坐标系

2.1.2 机械零点

机械零点为机床上固定位置的一点，通常机械零点设置在X轴和Z轴的正向或负向最大行程处，并安装相应的机械零点开关或撞块，如果机床上没有安装机械零点开关和撞块，请不要使用本系统中回机械零点功能(如G28），或将参数P006

Bit0～Bit2置成0以关闭各轴回零功能。

2.1.3 工件坐标系设定

1．试切对刀法建立坐标系和刀补

对于车床系统，一般X轴坐标零点建立在主轴卡盘轴心，Z轴坐标零点建立在工件端面或卡盘端面（见图2－1）。依此坐标位置模式，系统在试切对刀建立刀补时（输入测量值）同时建立工件坐标系，简化了操作，具体操作方法见第三章操作篇3.9.2节,推荐用户使用此方式建立坐标系。

13

DF-200T/DF-300T 用户使用手册 南京达风数控技术

(1) 把坐标系原点设在卡盘面上

44工件56Z工件Z4539XX

图2－1

加工图纸上的坐标和尺寸 车床上CNC指令的坐标

（同加工图纸上的坐标系）

(2) 把坐标系原点设在零件端面上

44工件56Z工件Z311484XX

图2－2

加工图纸上的坐标和尺寸 车床上CNC指令的坐标

（同加工图纸上的坐标系）

2．G50 设定工件坐标系

本系统可用G50指令设定坐标系：G50 X Z ；G50指令使刀具上某点（如刀尖或刀架中心点）的坐标位置为（X，Z）。

14

DF-200T/DF-300T 用户使用手册 南京达风数控技术

工件Z200起刀点=基准点X图2－3

如图2－3，用直径指令指定编程时，坐标系可以由 G50 X120 Z200 指令建立。

3．回机床零后自动设定工件坐标系

当参数P006 Bit6 ＝ 1时（回零后设定工件坐标系），回机床零点完成后，系统自动设定工件坐标系，其X、Z、Y坐标值分别由参数P044、P045、P178设定。

例如：参数P044 ＝ 2b；P045 ＝ a；回零完成后工件坐标自动为（2b，a）；

等同于回零完成后，执行了G50 X2b Za 指令，如图2－4。

工件Za起刀点=基准点Xb

图2－4

4．坐标系平移

用G50 U W 指令可以实现坐标系的平移。

15

60

DF-200T/DF-300T 用户使用手册 南京达风数控技术

执行G50 U W 指令后，刀架物理位置不变，但工件坐标系零点位置相对原位置平移了（U，W）。

如图2－5，原刀架中心位置为（120，200），执行G50 U－28 W－20 后，刀架中心坐标变为（92，180），如图2－6。

工件Z200X60

图2－5

工件Z180X46

图2－6

工件坐标系平移可应用于当刀架所有刀具在某方向偏差一致时，做整体偏差16

DF-200T/DF-300T 用户使用手册 南京达风数控技术

调整，这样不需要依次对每把刀进行刀补补偿。

2.1.4 直径指定和半径指定

车床控制系统的CNC编程时，有直径编程和半径编程两种方法，如图2－7。

通过设定参数P001 Bit2为0或1选择直径编程或半径编程：

当设定为直径编程时，X或U指令后的数值代表直径值；

当设定为半径编程时，X或U指令后的数值代表半径值；

ABD1D2ZR1R2D1,D2 ......

直径编程R1,R2 ......

半径编程X

图2－7

当用直径编程时，还应注意下表条件：

项 目

Z轴指令（地址Z或W）

X轴指令(地址X或U)

坐标系设定（G50）

X轴刀具补偿量

G90，G92，G94中的X轴的切削深度

圆弧插补的半径指令（R，I，K）

X轴方向的进给速度

注1: 在后面的说明中,没有特别指出直径或半径指定,当直径编程时,X轴为直径值；当半径编程时，X轴为半径值。

注 意 事 项

与直径和半径编程无关

用直径量编程

用直径指令X轴坐标值

用直径值设定

用半径值设定

用半径值设定

半径量变化

2.1.5 坐标单位及范围

17

DF-200T/DF-300T 用户使用手册 南京达风数控技术

本系统的最小编程单位为0.001mm，编程的最大移动范围是±99999.999mm

X轴： 最小设定单位0.001mm

Z轴： 最小设定单位0.001mm

Y轴： 最小设定单位0.001mm

2.1.6 编程坐标值

工件坐标系建立后，所有编程点的坐标位置都是相对于工件坐标系零点的坐标值，但定位到某点或进给到某点的程序编程值可以采用绝对坐标值（X，Z字段），相对坐标值（U，W字段），或混合坐标值（X/Z，U/W字段，绝对和相对坐标同时使用）方式进行编程。

1．绝对坐标值编程

“距坐标系原点的距离”即刀具要移到的坐标位置。

76工件BAX45Z3262

图2－8

如图2－8，刀具从A点移动到B点，使用B点的坐标值，其指令如下：

X32.0 Z76.0；

2．相对坐标值编程

指令从当前位置到下一位置的距离，（正负号表示方向）。

如上图，刀具同样由A点到B点，其指令如下：

U-30.0 W-45.0；

3．混合坐标值编程

如上图，刀具同样由A点到B点，其指令如下：

U-30.0 Z76.0；或X32.0 W-45.0；

18

DF-200T/DF-300T 用户使用手册 南京达风数控技术

2.1.7 初态，模态

初态是指系统上电后运行加工程序之前的系统编程状态。模态是指相应字段的值一旦设置，以后一直有效，直至某程序段又对该字段重新设置。模态设置之后，以后的程序段中若使用相同的功能，可以不必再输入该字段。

2.1.8 插补功能

把刀具沿着直线、圆弧运动以及螺纹加工的功能称为插补功能。

编程指令G01，G02，G92等被称为准备功能，用于指示数控系统进行何种插补运动。

1．刀具沿着直线运动

工件Z刀具X

程序指令：G01 Z__

2．刀具沿着圆弧运动

工件Z刀具X

程序指令：G02 X__ Z__ R__; 或G03 X__ Z__ R__;

3．切螺纹

依据螺纹导程，刀具运动与主轴旋转同步。

(1) 切直螺纹

19

DF-200T/DF-300T 用户使用手册 南京达风数控技术

程序指令：

螺纹循环加工： G92 X(U) Z（W） F/I

单刀螺纹加工： G32 Z（W） F/I

(2) 切锥螺纹

程序指令：

螺纹循环加工： G92 X(U) Z（W）R F/I

单刀螺纹加工： G32 X(U) Z（W）R F/I

2.1.9 进给功能

为了切削零件，用指定的速度使刀具运动称为进给，进给速度用数值指令。例如，让刀具以150毫米/分进给时，程序指令为：F150.0。

决定进给速度的功能称为进给功能。

20

DF-200T/DF-300T 用户使用手册 南京达风数控技术

2.1.10 切削速度—主轴功能

把切削工件时刀具相对工件的速度称为切削速度。CNC可以用主轴转速来指令这个切削速度。

例如：刀具直径为100毫米，切削速度用80米/分加工时，根据主轴转速N=1000V/лD的关系，主轴转速约为250RPM，指令为：S250

把有关主轴转速的指令称为主轴功能。

在设定为恒线速度切削模式时，当指定了切削速度V（米/分钟），即使在工件直径不断变化的锥面切削中，系统自动调节主轴转速，从而保持切削速度不变。

2.1.11 各种加工时选用的刀具——刀具功能

21

DF-200T/DF-300T 用户使用手册 南京达风数控技术

加工时需要选择粗加工，半精加工，精加工，切螺纹，切槽等各种刀具。各种刀具都带刀号，当程序中指定这个刀具号时，就自动选择对应的刀具。

例如某粗车用刀具号为01号，要在刀库01号的位置上选择刀具，此时指令为：

T0101；

就可以选出这把刀。把这个功能称为刀具功能。

2.1.12 各种功能操作指令——辅助功能

实际上，刀具开始加工工件时，要使主轴回转，供给冷却液，为此必须控制机床主轴电机和冷却油泵的开/关。

这些指令机床开/关动作的功能称为辅助功能，用M代码指令。

例如：若指令M03，主轴就以指令的回转速度顺时针回转。

2.1.13 刀具补偿功能

通常加工一个工件时，要使用几把刀具。各刀具有不同的形状，按照这些刀具来改变程序，非常麻烦。

为此，事先测量出各刀具的长度，然后把它们与标准刀具长度的差设定给CNC。这样，即使换刀，程序也不需要变更就可以加工了。这个功能称为刀具长度补偿功能。

2.2 G功能

G功能由字符G及其后2位数构成，其后的2位数定义了G代码的意义。

G代码表见表2－1。

根据G代码执行过程和功能类型，系统将G代码分为多个组别。一个程序段22

DF-200T/DF-300T 用户使用手册 南京达风数控技术

同组别的G代码只能有一个。

G代码有一次性代码和模态代码两种类型：

种类

一次性G代码

模态G代码

模态代码举例：G01和G00是同组的模态G代码

G01 X_； G01有效

Z_； G01有效

G00 Z_； G00有效

X_； G00有效

一次性模态代码举例：G04是一次性G代码，G00是模态G代码

G00 X_； G00有效

Z_； G00有效

G04 X_； G04有效

X_； G00有效

表2－1 G代码一览表

G代码

G00

*G01

G02

G03

01

组别 功能

定位（快速移动）

直线插补（切削进给）

圆弧插补CW（顺时针）

圆弧插补CCW（逆时针）

意义

只在其被指定的程序段有效

在指定同组其它G代码指令前一直有效

暂停，准停

G04 04

准停定位

G09 01

G26

G28

00

返回程序零点

返回机床零点

条件跳转加工

G31 00

螺纹切削

G32 01

刚性攻丝

G33 01

变螺距螺纹切削

G34 01

刀尖半径补偿取消

G40 07

23

DF-200T/DF-300T 用户使用手册 南京达风数控技术

G41

G42

*G61

G64

G70

G71

G72

G73

G74

G75

G86

G87

G90

G92

G94

G96

*G97

*G98

G99

注1：带有*记号的G代码，当电源接通时，系统处于这个G代码的状态。

注2：00组的G代码是一次性G代码。

注3：如果使用了G代码一览表中未列出的G代码，系统提示报警101；或指令了不具有的选择功能的G代码，也报警。

注4：在同一个程序段中可以指令几个不同组的G代码，如果在同一个程序段中指令了两个以上的同组G代码时，后一个G代码有效。

注5：在恒线速控制下，可设定主轴最大转速（G50）。

注6：G02，G03的顺逆方向由坐标系方向决定。

刀尖半径补偿（左）

刀尖半径补偿（右）

取消程序段间速度过渡

程序段间速度自动过渡

精加工复合循环

外圆粗车复合循环

00

端面粗车复合循环

封闭切削复合循环

端面深孔钻加工复合循环

外圆，内圆切槽复合循环

公制螺纹复合循环

英制螺纹复合循环

外圆，内圆车削单一循环

01

螺纹切削单一循环

端面，锥面切削单一循环

02

06

恒线速开

恒线速关

每分进给

每转进给

坐标系设定

G50 00

05

螺纹切削复合型循环

G76 01

01

2.2.1 定位（G00）

指令格式：G00 X(U)__Z(W)__；

24

DF-200T/DF-300T 用户使用手册 南京达风数控技术

用G00定位，刀具以快速移动速度到指定的位置，刀具以各轴独立的快速移动速度定位。

X(直径编程）Z非直线插补定位ZX

举例：如图2－9，快速定位编程如下：

42Z7640X20

25

图2－9

G0 X42.0 Z76.0 ；

或G0 U-20.0 W-40.0 ；

注：G00时各轴单独的快速移动速度由机床厂家设定（参数P021～022）。受快速倍率开关控制（F0，25%，50%，100%）。与F值指定的进给速度无关。

2.2.2 直线插补（G01）

指令格式：G01 X(U)__Z(W)__F__；

G01指令进行直线插补，指令中的X，Z或U，W值，分别定义了进给的绝

DF-200T/DF-300T 用户使用手册 南京达风数控技术

对值或增量值；由F指定进给速度，F值为模态值，在没有新的F指令以前总是有效的，因此不需要在每段中一一指定。

举例：如图2－10中刀具轨迹执行直线插补（直径编程）：

562860

图2－10

XG01 X56.0 Z28.0 F100；或

G01 U30.0 W-32.0 F100；

G01插补时，各轴进给速度计算如下：

G01 Uα Wβ Ff

X轴进给速度：Fx=a*f

L Z轴进给速度：Fz=βL*f

L=α2+β2

2.2.3 倒角功能

指令格式：G01 Z(W)__I__F__

G01 X(U)__K__F__

G01 Z(W)__R__F__

G01 X(U)__R__F__

G01直线插补时，在相交成直角的两个程序段间，通过编程可以实现两段间26

26Z

DF-200T/DF-300T 用户使用手册 南京达风数控技术

倒45度角或圆弧角。

编程格式为：

倒角方式 编程格式 倒角路线轨迹

Z

向Æ X向，G01 Z(W)__I__F__

其中I为X向倒角量，45度角

半径值，带符号，正负

号代表向X轴正向或负向倒角

C45°AD45°BC'

X

向Æ Z向，G01 X(U)__K__F__

其中K为Z向倒角量，45度角

半径值，带符号，正负

号代表向Z轴正向或负向倒角

C'KAD45°45°CBK

Z

向Æ X向，G01 Z(W)__R__F__

其中R为X向倒角半圆弧角

径值，带符号，正负号

代表向X轴正向或负向倒角

CC'iADBiiri

X

向Æ Z向，G01 X(U)__R__F__

其中R为Z向倒角半圆弧角

径值，带符号，正负号

代表向Z轴正向或负向倒角

ADC'kBk

27

rC

DF-200T/DF-300T 用户使用手册 南京达风数控技术

注：执行倒角的两个程序段必须为G01代码段，且两段相交为直角，否则系统产生报警或不执行倒角功能。

2.2.4 圆弧插补（G02，G03）

指令格式：G02 X_Z_ R_F

G02 X_Z_ I_K_F

G03 X_Z_ R_F

G03 X_Z_ I_K_F

字段

G02

G03

X，Z

U，W

I.K

R

F

指定内容

圆弧回转方向

圆弧回转方向

绝对坐标

相对坐标

圆心坐标

圆弧半径

进给速度

意义

顺时针圆弧CW

逆时针圆弧CCW

圆弧终点绝对坐标值

圆弧起点到终点的距离

圆心相对圆弧起点距离

圆弧上任一点到圆心的距离

沿圆弧的速度

所谓顺时针和逆时针是指在右手直角坐标系中，对于ZX平面，从Z轴的正方向往负方向看而言，如下图例。

右手坐标系

G02 X.. Z.. I.. K.. F.. G03 X.. Z.. I.. K.. F..

或

或

G02 X.. Z.. R.. F.. G03 X.. Z.. R.. F..

(绝对值指定) (绝对值指定)

（直径编程）

（直径编程）

28

DF-200T/DF-300T 用户使用手册 南京达风数控技术

用地址X，Z或者U，W指定圆弧的终点，用绝对值或增量值表示。增量值是从圆弧的始点到终点的距离值。圆弧中心用地址I，K指定。它们分别对应于X，Z轴。但I，K后面的数值是从圆弧始点到圆心的矢量分量，是增量值。如下图：

I、K根据方向带有符号。圆弧中心除用I，K指定外，还可以用半径R来指定。如下：

G02 X_Z_R_F_；

G03 X_Z_R_F_；

此时可画出下面两个圆弧，大于180°的圆弧和小于180°的圆弧。对于大于180°的圆弧不能指定。

29

DF-200T/DF-300T 用户使用手册 南京达风数控技术

如下图所示，刀具进行圆弧插补：

5030工件5818ZR20X

分别用绝对值方式和增量方式进行编程：

用I

、K编程：

G02 X58.0 Z30.0 I20.0 K0 F30；或

G02 U40.0 W-20.0 I20.0 K0 F30；

用半径R进行编程：

G02 X58.0 Z30.0 R20 F30；或

G02 U40.0 W-20.0 R20. F30；

30

DF-200T/DF-300T 用户使用手册 南京达风数控技术

圆弧插补的进给速度用F指定，为刀具沿着圆弧切线方向的速度。

注1.：采用I、K编程时，系统将对当前点坐标(起点)、终点坐标和圆心坐标进行验证；如果终点不在圆上，当终点到圆心的半径值与起点编程半径值相差绝对值大于参数P098（圆弧轮廓最大范围）时，系统产生117号报警提示：”圆弧终点不正确”。I，K编程可以编过象限圆和整圆。

注 2： 整圆不能用Ｒ编程。

注3： Ｒ为工件单边Ｒ弧的半径。Ｒ为带符号数，”＋”表示圆弧角小于180°； “－”表示圆弧角大于180°。

注4.：采用R编程时，如果直径2R小于当前点(起点)到终点的距离，系统将作出报警提示：”圆弧终点不正确”。

注5：圆弧加工过象限时X或Z轴可能会换向运动，若机床轴间隙过大，且反向间隙补偿功能未打开，可能会在工件上产生明显的切痕。开放间隙补偿功能并设定间隙补偿值参数，系统会自动进行间隙补偿，以减少圆弧过象限的误差。

注6：圆弧编程时若地址X 或Z未编，默认为上段坐标。I或K未编默认为0。

2.2.5 暂停或准停（G04）

指令格式：

G04 X__； //延时指令

G04 U__；

//延时指令

G04 P__； //延时指令

G04 ; //准停指令

G04指令地址为X或U或P时的延时单位：

指令地址

延时单位

X U P

秒

秒 0．001秒

暂停指令推迟下个程序段的执行，推迟时间为指令的时间。

时间范围从0.001～99999.999秒。

比如：G04 X10； //延时10秒

G04 P10； //延时0.010秒

如果省略了P，X，U指令则可看作是准确停，准确停指令可插入到需要保证轨迹尖角的两切削段间，以保证轨迹尖角。

比如：

N0010 G64； //程序段间速度过渡模式

N0020 G01 U－10 F100；

31

DF-200T/DF-300T 用户使用手册 南京达风数控技术

N0030 G04

N0040 W－20；

在N0020和N0040段间插入N0030 G04段后，当N0020段执行结束，速度降为0后，再执行N0040段，这样保证了轨迹尖角。

若没有N0030段，系统自动处理N0020和N0040段间的过渡速度，会在拐角处产生圆弧。

2.2.6 准停定位（G09）

指令格式：G09

G09用于旋转轴的准确快速定位。当Y轴作为旋转轴使用时，当需要快速定位时，使用该指令使Y轴快速回位到零位。

2.2.7 自动返回机械零点（G28）

指令格式：G28 X（U）__Z(W)__；

利用上面指令，可以使指令的轴自动返回到参考点。X（U）__Z(W)__指定返回到参考点路途经过的中间点，用绝对值指令或增量值指令。

（1） 以快速回零速度（由参数P109设定）从当前位置定位到指令轴的中间点位置（A点—B点），如图2-11。

（2） 以快速回零速度从中间点向参考点方向移动（B点—R点）。

（3） 检测到减速信号后，低速运行（由参数P043设定）寻找精定位信号。

（4） 检测到精定位信号后，返回零点执行完毕，回零灯亮。

ZA中间点B(42,56)参考点RX图2－11

32

DF-200T/DF-300T 用户使用手册 南京达风数控技术

注1：由中间点向零点位置移动的方向由参数P.005 Bit0，Bit1，Bit2设定。

注2：若程序加工起点与参考点（机械零点）不一致时，回零完成后，可通快速定位指令（G0指令）或回程序零点方式回程序加工起点（程序加工起点坐标由参数P192，P193，P194定义）。

2.2.8 自动返回程序零点（G26）

指令格式：G26 X Z；

其中：X

和Z后不需要带坐标值，X和Z的程序零点坐标位置由参数P192、P193确定。

系统执行G26时，由当前坐标位置以手动快速速度返回到程序零点位置。

2.2.9 跳段功能（G31）

指令格式：G31 X(U)__Z(W)__L/K__ F__

其中：X(U)，Z(W)：进给坐标位置

F：进给速度

L：检测低电平有效的输入口

K：检测高电平有效的输入口

功能说明：程序执行G31功能时，在未检测到外部有效信号前，保持F进给速度进给。若在到达目标坐标前检测到了有效信号，则停止进给，跳转到下段执行；若在到达目标坐标前未检测到有效信号，当到达目标坐标后，该段执行结束，执行下段。其中L__或K__参数后的值表示待测的输入口编号，L表示该输入口低电平为有效信号，K表示该输入口高电平为有效信号。有关各输入口的编程口号可在诊断界面中查看，具体查看方法见第三章操作篇第3.10.7节。

举例1：如下图2-12，轨迹A－B－D’：无跳转信号的运行轨迹

执行 G31 W160 L8 F100

G0 U60

程序执行时，以F100的速度进给Z轴，同时检测8号输入口，在走到C点位置时，系统检测到8号输入口的低电平信号，程序结束G31段执行，立刻跳转到G0 U60段执行。这样，实际运行轨迹为A－C－D。

若在Z轴走完W160后仍未检测到8号输入口的低电平信号，系统结束G31段，执行G0 U60段。

33

DF-200T/DF-300T 用户使用手册 南京达风数控技术

Z160ACB实际移动60无skip信号时的移动D'Xskip信号输入点D

图2-12

举例2：如下图2－13，轨迹A－B－D为无跳转信号的运行轨迹

执行 G31 W80 K6 F200

G01 X300 Z100

程序执行时，以F200的速度进给Z轴，同时检测6号输入口状态，在走到C点位置时，系统检测到6号输入口的高电平信号，程序结束G31段执行，立刻跳转到G01 X300 Z100段执行。这样，实际运行轨迹为A－C－D。

若Z轴到达B点后仍未检测到6号输入口的高电平信号，系统结束G31段，执行G01 X300 Z100段。

ZA(100,0)CB(100,80)D(300,100)skip信号输入点X

图2－13

2.2.10单刀螺纹（G32）

用G32指令，可以切削导程不变的直螺纹，锥螺纹。

直螺纹指令格式：G32 Z(W)__F/I__；

Z（W）：螺纹终点Z向位置；

F：公制螺纹，长轴方向的导程（0.001—500.000mm）。

I：英制螺纹，长轴方向的每英寸牙数（0.060—25400牙/英寸）

34

DF-200T/DF-300T 用户使用手册 南京达风数控技术

锥螺纹指令格式：G32 X（U）__Z(W)__F/I__；

X（U）：螺纹终点X向位置；

Z（W）：螺纹终点Z向位置；

F：公制螺纹，长轴方向的导程（0.001—500.000mm）。

I：英制螺纹，长轴方向的每英寸牙数（0.060—25400牙/英寸）

在螺纹切削开始及结束部分，一般由于升降速的原因，会出现导程不正确部分，考虑此因素影响，指令螺纹长度应当比需要的螺纹长度要长些。

例1：直螺纹切削

68Z2125X在Z方向：△1=3mm，△2=1.5mm

螺纹导程：3mm

在牙深共2mm（公制输入，直径编程）：

G00 U-25.0 //定位，进刀深度为2mm

G32 W-72.5 F3.0 //螺纹切削进给，长度74.5mm

G00 U25.0 //X向退刀

W72.5 //Z向返回进刀点

例2：锥螺纹切削

35

DF-200T/DF-300T 用户使用手册 南京达风数控技术

假设螺纹导程 4mm，螺纹起点坐标（15，40），螺纹终点坐标（30，10），

G00 Z40

X15.0 //定位到螺纹起点位置

G32 X30.0 Z10 F4 //锥螺纹切削

G00 X40.0

注1：在切削螺纹中，进给速度倍率和主轴倍率无效。

注2：在螺纹切削中，主轴不能停止，进给保持在螺纹切削中无效。

2.2.11 刚性攻丝（G33）

指令格式：G33 Z(W)__ F(I)__ J__；

Z：丝孔底绝对坐标

W：丝孔底相对坐标

F：公制丝攻牙距（单位mm）

I：英制丝攻每英寸牙数

J：攻到位置后，系统发出主轴停止信号，主轴降速，当降到J设定的速度时发出反转信号。不编则降速到0后反转。当主轴惯性较大降速较慢时，为了减少攻丝到位后跟随距离过长，可以编适当的J值以使主轴较快的制动并换向。（单位

转/分）

G33动作顺序：

执行G33前应当首先启动主轴，G33执行时由当前位置跟随主轴进给，当到Z轴达丝孔底部位置时，发出主轴停止信号。若编了J，则当转速降到J值时，发出反转信号。若未编J则降速到0后发出反转信号。然后Z轴跟随主轴反向退刀。当到达起刀点后，Z轴降速停止，同时恢复主轴原来旋转方向，G33指令段执行结束。

36

DF-200T/DF-300T 用户使用手册 南京达风数控技术

2.2.12 变螺距螺纹切削（G34）

指令格式： G34 X(U) Z(W) F/I K

其中：

X(U)：螺纹终点X向绝对（相对）坐标

Z(W)：螺纹终点Z向绝对（相对）坐标

F：公制螺纹，螺纹初始导程（0.001—500.000mm）。

I： 英制螺纹，螺纹初始每英寸牙数（0.060—25400牙/英寸）

K：每转螺距增量或减量，范围：0.001～500mm或0.0001～9.9999英寸/牙；当K值的增加或减少使螺距超出允许值或减少到0或负值时，系统产生报警。

2.2.13端面螺纹（G35）

用G35指令，可以切削导程不变的端面直螺纹，端面锥螺纹。

端面直螺纹指令格式：G35 X(U)__ F/I__；

X（U）：螺纹终点X向位置；

F：公制螺纹，X轴方向的导程（0.001—500.000mm），半径指定。

I：英制螺纹，长轴方向的每英寸牙数（0.060—25400牙/英寸），半径指定。

锥螺纹指令格式：G35 X（U）__Z(W)__F/I__；

X（U）：螺纹终点X向位置；

Z（W）：螺纹终点Z向位置（用于加工端面锥螺纹）；

F：公制螺纹，长轴方向的导程（0.001—500.000mm），半径指定。

I：英制螺纹，长轴方向的每英寸牙数（0.060—25400牙/英寸），半径指定。

在螺纹切削开始及结束部分，一般由于升降速的原因，会出现导程不正确部分，考虑此因素影响，指令螺纹长度应当比需要的螺纹长度要长些。

例1：端面直螺纹切削

X方向从直径100车到50，螺纹导程：2mm，牙深2mm;

M03S500；

G00 X102; //X定位

Z-1; //进刀深度为1mm

G35 X50 F2.0; //螺纹切削进给

G00 Z2 //Z向退刀

37

DF-200T/DF-300T 用户使用手册 南京达风数控技术

X102;

Z-2; //再次进刀

G35 X50 F2.0; //螺纹切削进给

G00 Z2 //Z向退刀

X102;

M30；

例2：锥螺纹切削

假设螺纹导程 3mm，螺纹起点坐标（150，-3），螺纹终点坐标（30， 0），

M03S500；

G00 X150; //X定位

Z-1.5; //进刀深度为1.5mm

G35 X30 W3 F3.0; //螺纹切削进给

G00 Z5 //Z向退刀

X150;

Z-3; //再次进刀

G35 X30 W3 F3.0; //螺纹切削进给

G00 Z2 //Z向退刀

X200;

M30；

注1：在切削螺纹中，进给速度倍率和主轴倍率无效。

注2：在螺纹切削中，主轴不能停止，进给保持在螺纹切削中无效。

2.2.14 螺纹切削单一循环（G92）

用G92指令编程，可以进行直螺纹、锥螺纹、多头螺纹、任意固定进刀角度的公英制螺纹切削，同时G92指令可以设定螺纹退尾长度（由参数K指定），因此螺纹切削时不需要退刀槽。

指令格式：G92 X(U) Z(W) R K F/I L Q

其中：Z（W）：螺纹终点Z向坐标，模态值

：螺纹切削终点X向坐标

X（U）R：

螺纹头部半径相对螺纹尾部半径的差值，用于锥螺纹编程。不编为直螺纹，模态值。

K：螺纹Z向退尾长度，不编由参数P068决定默认退尾长度，

38

DF-200T/DF-300T 用户使用手册 南京达风数控技术

其退尾长度

＝ P068

× 0.1

×

螺纹导程，模态值

F:

公制螺纹导程，单位mm,

模态值

I:

英制螺纹每英寸螺纹牙数，1英寸＝25.4mm，模态值。

L：多头螺纹头数，不编默认为单头螺纹，模态值。

Q：螺纹起始角，不编默认为0，非模态值。

一般加工螺纹时，从粗车到精车，用同一轨迹要进行多次螺纹切削。采用G92螺纹切削循环加工，简化了螺纹编程。因为螺纹切削的开始进刀是从检测出主轴位置编码器的零脉冲信号（Z脉冲）后才开始的，因此即使进行多次螺纹切削，零件圆周上的切削点仍是相同的，工件上的螺纹轨迹也是相同的。但是从粗车到精车，主轴的转速必须是稳定的。当主轴转速变化过大时，螺纹会或多或少产生偏差。

G92

指令为模态，其中的Z（W）值，F值/I值，K值，R值，L值均为模态，在多刀循环切削的螺纹加工中，只要螺纹首段编程时设置了必要的螺纹参数，其后的程序段中可以省略。比如若要三刀车削导程1.2mm，长度10mm的直螺纹可以这样简化编程：

……

N0090 G0 X10 Z0

；

长度10mm, X向进给0.5mm

N0100 G92 X9.5 Z-10 F1.2 //导程1.2mm，N0110 X9.0 //第2刀，X向进给0.5mm

N0120 X8.9 //第3刀，X向进给0.1mm，完成切削

N0130 G0 Z10

；

G92每执行切削一刀后，均返回到螺纹起刀点位置。

下面分别解释几种螺纹循环的编程：

（a） 直螺纹切削循环

G92 X（U）__Z(W)__F__；（公制螺纹）

G92 X（U）__Z(W)__I__；（英制螺纹）

39

DF-200T/DF-300T 用户使用手册 南京达风数控技术

图2－14

如图2－14所示，G92指令切削加工动作顺序为：

快速定位→等待头脉冲→切削进给→快速退尾→快速回刀

1―――――――――――2――――3―――――4

轨迹1：由当前位置快速定位到X（U）设定的位置，然后等待头脉冲

轨迹2：检测到头脉冲后，根据主轴旋转位置和速度进刀

轨迹3：到退尾位置后，开始快速退尾，并X轴快速回刀。

轨迹4：快速定位到起点位置，若下段仍为G92指令，则如此循环加工。若下段非G92指令，螺纹加工完成。

（b） 锥螺纹切削循环

G92X（U）__Z(W)___R__F__；

G92X（U）__Z(W)___R__I__；

其中R为螺纹头部半径相对于螺纹尾部半径的差值。（注意：半径差值而非直径差值）

40

DF-200T/DF-300T 用户使用手册 南京达风数控技术

快速定位→等待头脉冲→切削进给→快速退尾→快速回刀

1―――――――――――2――――3――――－4

轨迹1：由当前位置快速定位到X（U）设定的位置，然后等待头脉冲

轨迹2：检测到头脉冲后，根据主轴旋转位置和速度沿锥度方向进刀

轨迹3：到退尾位置后，开始快速退尾，并X轴快速回刀。

轨迹4：快速定位到起点位置，若下段仍为G92指令，则如此循环加工。若下段非G92指令，螺纹加工完成。

（c） 设定螺纹切削起始角

G92指令可以设定螺纹切削起始角度（相对于主轴编码器头脉冲位置的角度），由编程参数Q设定。

Q：螺纹起始角，范围为0～360，不编默认为0，非模态值。

Q值在当前段有效，当主轴转到Q设定的角度时，螺纹开始进刀。

（d） 多头螺纹

G92指令参数L用于设定螺纹头数，不编默认为1。

多头螺纹加工动作顺序：

快速定位→等待头脉冲→切削进给→快速退尾→快速回刀→快速定位→

1――――――――－――2―――――3――――4―――――1

41

DF-200T/DF-300T 用户使用手册 南京达风数控技术

等待分度角度→切削进给→快速退尾→快速回刀→快速定位→等待分度角度

―――――――2―――――3――――4―――――1―――――

如此循环，直到当前螺纹头数加工完毕。

举例：8mm导程4头螺纹加工，假设工件直径20.5mm，螺纹长度48mm，分5次循环切削

G0 X22 Z2

G92 X20 W－50 F8 L4 //切削深度0.5mm，分4次切削，每次进刀角度相差90度

X19.6 //切削深度0.4mm,分4次切削，每次进刀角度相90度

X19 //切削深度0.6mm,分4次切削，每次进刀角度相90度

X18.6 //切削深度0.4mm,分4次切削，每次进刀角度相90度

X18.4 //切削深度0.2mm,分4次切削，每次进刀角度相90度

G0 X30

注1：在切削螺纹中，进给速度倍率和主轴倍率无效。

注2：在螺纹切削中，主轴不能停止，进给保持在螺纹切削中无效。

注3：螺纹切削进给（动作2）过程中不响应进给保持。

注4：当单段功能打开时，螺纹按1，2，3，4的动作顺序单段执行。

2.2.15 复合型螺纹切削循环（G76）

指令格式： G76 P(m)(r)(a) Q(△dmin) R(d);

G76 X(U) Z(W) R(i) P(k) Q(△d) F(I)

其中：

m: 最后螺纹精加工循环次数，设定范围1～99次。此值为模态，在下次指定前一直有效；不编由参数P076默认设定。

r：螺纹退尾长度。设定范围01～99，以1/10螺纹导程（L）的为单位；

比如该值为4，表示螺纹退尾长度为0.4螺纹导程。不编由参数P068默认设定。

a:

刀尖角度（螺纹牙的角度），可以选择的角度为80。,60。,55。,30。,29。,0。共6种角度。此值由两位数指定。此值为模态值，在下次指定前保持有效。不编由参数P077默认设定。

m,r,a值用地址P一次指定，且均必须是两位数字：

例 m=2; r = 1.0, a = 60

用地址P如下编程指定 P021060。

△dmin：最小切入深度，单位mm。当一次切入深度（△dN － △dN−1）比△dmin还小时，则用△dmin最为一次切入量，该值为模态。

42

DF-200T/DF-300T 用户使用手册 南京达风数控技术

d：精加工余量，单位mm，模态。

X(U)：螺纹终点X向绝对（相对）坐标，单位：mm。

Z(W)：螺纹终点Z向绝对（相对）坐标，单位：mm。

i：螺纹头相对螺纹尾的半径差值，i＝0则表示为直螺纹，单位：mm。

k：螺纹牙高，X方向的值用半径值表示。单位mm。

△d：第一刀切入量，单位mm。

F：螺纹导程，单位：mm。

I：每英寸牙数，用于英制螺纹切削。

注：1. 用P、Q、R指定的数据，根据有无地址X（U）、Z（W）来区别；

2．循环动作由地址X(U)、Z（W）指定的G76指令进行；

3．此循环加工中，刀具为单侧刃加工，刀尖的负载较双刃减轻。

4．第一次切入深度为△d，第N次切入深度为（△dN － △dN−1），每次的切削量是一定的。

5．G76也可以加工内螺纹和锥螺纹。

6．m、r、a用地址P一次指定，不编地址P则由参数P076、P068、P077设定m、r、a的值。

7．关于切螺纹的注意事项，与G32切螺纹相同。

G76 加工轨迹图示：

G76切入方法轨迹详细说明：

43

DF-200T/DF-300T 用户使用手册 南京达风数控技术

例：G76螺纹复合切削循环示例：

用G76代码编下图程序，加工螺纹为M68x6.

程序加工编程如下：

M03 S300；

G00 X80 Z10；

G76 P011060 Q0.1 R0.2;

G76 X60.640 Z25.000 P3.680 Q1.800 F6.0;

G00 X100 Z50；

M05；

M30；

44

DF-200T/DF-300T 用户使用手册 南京达风数控技术

2.2.16 公制螺纹切削复合循环（G86）

指令格式： G86 X(U) Z(W) K R I/D J L P Q

其中： X(U)：螺纹终点X向绝对（相对）坐标

Z(W)：螺纹终点Z向绝对（相对）坐标

K：螺纹导程，单位mm

R：螺纹外径与根径的直径差，无符号

I： 螺纹X向退刀量，带符号，I值决定了螺纹X向退刀和进刀方向

D：螺纹X向渐进切入模式，用于设定进刀点相对螺纹牙顶的X向距离，直径值；I和D不能同时存在；

J：螺纹Z向退尾长度，不编由参数P068决定

L：螺纹切削循环次数

P：螺纹头数，不编默认为1

Q：螺纹第一刀进刀深度，直径值，单位mm

G86功能说明：

Z第二刀第一刀第二刀退尾第一刀退尾起刀点停刀点X

(1)

一般螺纹加工循环的起始位置为将刀尖对准螺纹的外径处，螺纹X向退刀量由I值决定；I值为正值表示切削外螺纹，I值为负值表示切削内螺纹，I值大小决定了螺纹X向的退刀距离。

（即X向起刀点位于螺纹牙顶之外进刀），(2)当需要进行螺纹X向渐进切入时使用参数D设置牙顶X向相对刀具的距离值，当编D时应注意：螺纹进刀的刀尖位置必须位于工件表面外距离D值的位置，若小于D值距离，则将撞刀或螺纹首刀进深过大；D同时也表示了X向退尾距离。X向渐进切入方式用于螺纹Z向进刀空间不足或在杆件中部进行螺纹切削。

(3)

系统根据P075参数决定是否增加最后一刀光整螺纹面。参数P075 = 0，不增加光刀；P075 != 0，增加一刀光整螺纹面，光整量为P075设定值，单位um.

45

DF-200T/DF-300T 用户使用手册 南京达风数控技术

(4)

当需要螺纹提前收尾时，可使用退尾功能，其格式为G86指令中增加J值，J后面的数字代表Z向退尾长度，即当刀尖离螺纹终点距离为J后面的值时（Z方向），X向开始退尾。J值不编时，一般Z向走到接近终点时X向才退尾。

一般设定范围为3000mm/min-5000mm/min.

(5)参数P073定义X向退尾的速度，(6) G86螺纹切削循环的进刀量可以设定为等距离进刀，也可指定第一刀进刀深度，剩余为等距离进刀。当参数P075= 0时：若不指定第一刀进刀量，则每次进刀量为R/L；若指定了第一刀进刀量，则第一刀进刀量为Q，则剩余循环进刀量为(R-Q)/(L-1)；当参数P075!＝0时：若不指定第一刀进刀量，每次进刀量为(R-P075)/L，最后增加一刀光刀；若指定了第一刀进刀量，则第一刀进刀量为Q，剩余循环进刀量为(R-Q-P075)/(L-1)；

(7)

螺纹加工的开始及结束时有升降速过程，在此过程中，螺纹的导程是不准确的，因此实际加工时必须避开这二个区域。参数P069定义了螺纹加工时Z向加速时间常数。

使用参数D设置牙顶相对刀具的距离值，(8)当需要进行螺纹X向渐进切入时，当编D时应注意：开始螺纹进刀时的刀尖必须位于工件表面外距离D值，若小于D值距离，则将撞刀或螺纹首刀进深过大；D同时也表示了X向退尾距离。X向渐进切入方式用于螺纹Z向进刀空间不足或在直杆件中部进行螺纹切削。

(9)

螺纹加工时Z轴步进/伺服电机的速度不应超过某一值，如8000mm/min，该速度与机床大小及电机功率有关，由参数P071决定。

(10)

螺纹在切削前，数控系统检测编码器的零信号，同时检测主轴转速波动程度，满足条件后刀具才开始运动，因此在螺纹加工的开头有停顿感。

2.2.17 英制螺纹切削复合循环（G87）

G87指令同G86，只是G87中的K值的意义是牙数/英寸（1英寸＝25.4mm）。其他参数完全一致。

2.2.18 刀尖半径补偿（G40，G41，G42）

有关刀尖半径补偿的说明见第六章。

2.2.19 坐标系设定（G50）

指令格式：G50 X*** Z ***

此指令建立一个坐标系，使刀具上的某一点，例如刀尖在此坐标系中的坐标为（***,***）。此坐标称为工件坐标系。工件坐标系一旦建立后，后面指令中绝对值指令或相对值指令的位置都是依此坐标系坐标原点的位置来表示的。

46

DF-200T/DF-300T 用户使用手册 南京达风数控技术

注：当为直径编程模式时，X值表示的是直径值；当为半径编程模式时，X值表示的是半径值。

工件Za起刀点=基准点Xb

图2－15

如图2－15，直径编程时，可由G50 X 2b Z a

指令建立坐标系

b Z a

指令建立坐标系

半径编程时，可由G50 X

2.2.20 每分进给（G98）

指令格式：G98

G98为每分进给模式，在G98模式下，刀具进给速度由F后续的数值指定。

G98是模态的，一旦指定了G98模式，在G99（每转进给）指令之前，一直有效。

系统上电后默认是G98模式。

2.2.21 每转进给（G99）

G99为每转进给模式，在G99模式下，主轴每转刀具的进给量由F后续的数值指定。

G99是模态的，一旦指定了G99状态，在G98（每分进给）指令之前，一直有效。

表2-2

每分进给和每转进给

指定地址

指定代码

指定范围

每分进给

每转进给

F F

G98 G99

1～60000mm/min

(F1～F60000)

0.01～500.00mm/re

(F1～F50000)

注1：当位置编码器的转速在1转/分以下时，速度会出现不均匀地加工。转速越慢，越47