The NIST RS274NGC Interpreter - Version 3

Thomas R. Kramer

Frederick M. Proctor

Elena Messina

Intelligent Systems Division

National Institute of Standards and Technology

Technology Administration

U.S. Department of Commerce

Gaithersburg, Maryland 20899

NISTIR 6556

August 17, 2000
RS274/NGC Interpreter - Version 3

ii

Disclaimer

Commercial equipment and materials are identified in order to specify certain

procedures adequately. In no case does such identification imply recommendation or

endorsement by the National Institute of Standards and Technology, not does it imply

that the materials or equipment identified are necessarily the best available for the

purpose.

Acknowledgements

Partial funding for the work described in this paper was provided to Catholic University

by the National Institute of Standards and Technology under cooperative agreement

Number 70NANB7H0016.

Abstract

This report describes an interpreter which reads numerical control code and produces

calls to a set of canonical machining functions. The interpreter is a software system

written in the C++ programming language. The output of the interpreter may be used

to drive 3-axis to 6-axis machining centers. Input to the interpreter is RS274 code in the

dialect defined by the Next Generation Controller (NGC) project, with modifications.

The interpreter may be compiled as a stand-alone computer program or may be

integrated with the NIST Enhanced Machine Controller (EMC) control system. Input

can come from a file or from a user typing on a computer keyboard. Output commands

can either be printed for future use or be executed directly on a machining center. The

report includes a full description of the RS274/NGC input language and the canonical

machining functions called by the interpreter. It is a complete users manual.

Keywords

controller, interpreter, machining, NC code, numerical control, NIST, rs274
iii

NIST RS274/NGC Interpreter - Version 3

CONTENTS

1.0 Introduction............................................................................................. 1

1.1 Audience ............................................................................................................1

1.2 Background........................................................................................................1

1.2.1 Enhanced Machine Controller Project...................................................1

1.2.2 Numerical Control Programming Language RS274..............................1

1.2.3 The RS274/NGC Language ...................................................................2

1.2.4 Previous Work at NIST..........................................................................2

1.2.5 Current Work at NIST ...........................................................................3

1.3 Major Characteristics of the Interpreter.............................................................3

1.3.1 How it Runs ...........................................................................................3

1.3.2 Modes of Use .........................................................................................3

2.0 Machining Center Overview.................................................................. 4

2.1 Machining Centers.............................................................................................4

2.1.1 Mechanical Components........................................................................4

2.1.2 Control and Data Components...............................................................6

2.2 Interpreter Interaction with Switches.................................................................9

2.2.1 Feed and Speed Override Switches........................................................9

2.2.2 Block Delete Switch ..............................................................................9

2.2.3 Optional Program Stop Switch ..............................................................9

2.3 Tool File.............................................................................................................9

3.0 Input: the RS274/NGC Language ....................................................... 12

3.1 Overview..........................................................................................................12

3.2 RS274/NGC Language View of a Machining Center......................................12

3.2.1 Parameters............................................................................................12

3.2.2 Coordinate Systems .............................................................................14

3.3 Format of a Line...............................................................................................14

3.3.1 Line Number ........................................................................................15

3.3.2 Word ....................................................................................................15

3.3.3 Parameter Setting.................................................................................18

3.3.4 Comments and Messages.....................................................................18

3.3.5 Item Repeats.........................................................................................19

3.3.6 Item order.............................................................................................19

3.3.7 Commands and Machine Modes..........................................................19

3.4 Modal Groups ..................................................................................................20
NIST RS274/NGC Interpreter - Version 3

iv

3.5 G Codes............................................................................................................21

3.5.1 Rapid Linear Motion — G0.................................................................23

3.5.2 Linear Motion at Feed Rate — G1 ......................................................23

3.5.3 Arc at Feed Rate — G2 and G3...........................................................23

3.5.4 Dwell — G4.........................................................................................25

3.5.5 Set Coordinate System Data — G10 ...................................................25

3.5.6 Plane Selection — G17, G18, and G19 ...............................................25

3.5.7 Length Units — G20 and G21.............................................................26

3.5.8 Return to Home — G28 and G30 ........................................................26

3.5.9 Straight Probe — G38.2.......................................................................26

3.5.10 Cutter Radius Compensation — G40, G41, and G42..........................28

3.5.11 Tool Length Offsets — G43 and G49..................................................29

3.5.12 Move in Absolute Coordinates — G53 ...............................................29

3.5.13 Select Coordinate System — G54 to G59.3 ........................................29

3.5.14 Set Path Control Mode — G61, G61.1, and G64 ................................30

3.5.15 Cancel Modal Motion — G80 .............................................................30

3.5.16 Canned Cycles — G81 to G89.............................................................30

3.5.17 Set Distance Mode — G90 and G91....................................................36

3.5.18 Coordinate System Offsets — G92, G92.1, G92.2, G92.3..................36

3.5.19 Set Feed Rate Mode — G93 and G94 .................................................37

3.5.20 Set Canned Cycle Return Level — G98 and G99 ...............................37

3.6 Input M Codes..................................................................................................38

3.6.1 Program Stopping and Ending — M0, M1, M2, M30, M60 ...............38

3.6.2 Spindle Control — M3, M4, M5 .........................................................39

3.6.3 Tool Change — M6 .............................................................................39

3.6.4 Coolant Control — M7, M8, M9.........................................................39

3.6.5 Override Control — M48 and M49 .....................................................39

3.7 Other Input Codes............................................................................................40

3.7.1 Set Feed Rate — F ...............................................................................40

3.7.2 Set Spindle Speed — S ........................................................................40

3.7.3 Select Tool — T...................................................................................40

3.8 Order of Execution...........................................................................................41

4.0 Output: the Canonical Machining Functions..................................... 42

4.1 Introduction......................................................................................................42

4.1.1 Objectives of Canonical Machining Functions....................................42

4.1.2 Implementing Canonical Machining Functions...................................42

4.2 Canonical Machining Function View of a Machining Center.........................45

4.2.1 Mechanical Components......................................................................45

4.2.2 Control Components ............................................................................45

4.2.3 Error Conditions...................................................................................46

4.3 The Canonical Machining Functions Defined .................................................46
NIST RS274/NGC Interpreter - Version 3

v

4.3.1 Preliminaries ........................................................................................46

4.3.2 Initialization and Termination..............................................................47

4.3.3 Representation......................................................................................47

4.3.4 Free Space Motion ...............................................................................48

4.3.5 Machining Attributes ...........................................................................48

4.3.6 Machining Functions ...........................................................................51

4.3.7 Spindle Functions ................................................................................55

4.3.8 Tool Functions .....................................................................................57

4.3.9 Miscellaneous Functions......................................................................58

4.3.10 Program Functions...............................................................................61

4.3.11 Cutter Radius Compensation ...............................................................61

5.0 Stand-Alone Interpreter....................................................................... 62

5.1 Running the SAI ..............................................................................................62

5.1.1 Starting the SAI....................................................................................62

5.1.2 Running with Keyboard Input .............................................................63

5.1.3 Running with RS274/NGC File Input .................................................65

5.2 Building an SAI Executable.............................................................................65

5.3 Interpreter Speed..............................................................................................68

Appendix A Error Handling ...................................................................... 70

A.1 Basic Approach............................................................................................... 70

A.2 Handling Calculated Values ........................................................................... 71

A.3 Compiler Macros ............................................................................................ 71

A.4 Automatic Generation of Software ................................................................. 71

A.5 Interpreter Bugs .............................................................................................. 72

A.6 Stand-Alone Interpreter Driver Error Messages............................................. 72

Appendix B Cutter Radius Compensation ............................................... 73

B.1 Introduction..................................................................................................... 73

B.1.1 Data for Cutter Radius Compensation .................................................74

B.2 Programming Instructions............................................................................... 75

B.2.1 Turning Cutter Radius Compensation On............................................75

B.2.2 Turning Cutter Radius Compensation Off...........................................75

B.2.3 Sequencing...........................................................................................75

B.2.4 Use of D Number.................................................................................75

B.3 Material Edge Contour.................................................................................... 75

B.3.1 Programming Entry Moves..................................................................76
NIST RS274/NGC Interpreter - Version 3

vi

B.4 Nominal Path Contour .................................................................................... 78

B.5 Programming Errors and Limitations ............................................................. 80

B.5.1 Concave Corner and Tool Radius Too Big (10 and 16) ......................81

B.5.2 Cannot Turn Cutter Radius Comp on When On (5) ............................81

B.5.3 Cutter Gouging (11).............................................................................82

B.5.4 Tool Radius Index Too Big (15)..........................................................82

B.5.5 Two G Codes Used from Same Modal Group (17) .............................82

B.6 First Move into Cutter Compensation ............................................................ 82

Appendix C Sample Programs................................................................... 84

C.1 Sample Simple Program ................................................................................. 84

C.2 Sample Program to Test Expressions ............................................................. 85

C.3 Sample Program to Test Canned Cycles......................................................... 86

Appendix D Interpreter Software.............................................................. 88

D.1 Interpreter Interfaces....................................................................................... 88

D.2 Software Files and Organization..................................................................... 89

D.3 Cyclic Operation ............................................................................................. 91

D.3.1 Read, Store, and Check........................................................................91

D.3.2 Execute.................................................................................................91

D.4 Interpreter-do-it Functions.............................................................................. 91

D.5 Interpreter-give-information Functions .......................................................... 92

D.6 World-give-information Functions ................................................................. 93

D.7 Interpreter Function Call Hierarchies ............................................................. 95

D.8 Special Topics............................................................................................... 101

D.8.1 Interpreter World Model....................................................................101

D.8.2 Block Model.......................................................................................102

D.8.3 Expression Evaluation .......................................................................103

D.8.4 Parameter Buffering...........................................................................103

Appendix E Production Rules for theRS274/NGC Language .............. 105

E.1 Production Language .................................................................................... 105

E.2 Productions ................................................................................................... 105

E.3 Production Tokens in Terms of Characters .................................................. 107
vii

NIST RS274/NGC Interpreter - Version 3

FIGURES

Figure 1. G87 Cycle .........................................................................................35

Figure 2. Two Cutter Radius Compensation Methods ................................74

Figure 3. Cutter Radius Compensation Entry Moves .................................76

Figure 4. Simpler Cutter Radius Compensation Entry Move ....................78

Figure 5. Cutter Radius Compensation Entry Moves .................................80

Figure 6. Two Cutter Radius Compensation Errors ...................................81

Figure 7. First Cutter Radius Compensation Move - Straight ...................82

Figure 8. First Cutter Radius Compensation Move - Arc ...........................83

Figure 9. Interpreter Interfaces .....................................................................88

Figure 10. Software .........................................................................................90

Figure 11. Interpreter-do-it Function Call Hierarchy .................................96

Figure 12. Interpreter Function Call Hierarchy

(from rs274_ngc read) ...............................................................................97

Figure 13. Interpreter Function Call Hierarchy

(from read_real_value) .............................................................................98

Figure 14. Interpreter Function Call Hierarchy

(from rs274ngc_execute) ...........................................................................99

Figure 15. Interpreter Function Call Hierarchy

(from convert_motion) ............................................................................100

Figure 16. SAI Driver Function Call Hierarchy .........................................101
viii

NIST RS274/NGC Interpreter - Version 3

TABLES

Table 1. Sample Tool File ............................................................................... 11

Table 2. Default Parameter File..................................................................... 13

Table 3. Word-starting Letters ...................................................................... 16

Table 4. Modal Groups ................................................................................... 20

Table 5. G Codes.............................................................................................. 22

Table 6. Code to Probe Hole.......................................................................... 28

Table 7. M Codes............................................................................................. 38

Table 8. Order of Execution ........................................................................... 41

Table 9. Canonical Machining Functions Called By Interpreter ............... 44

Table 10. Transcript of an SAI Session Using Keyboard Input.................. 64

Table 11. Makefile for Interpreter................................................................. 67

Table 12. NC Program for Figure 3............................................................... 77

Table 13. NC Program for Figure 5............................................................... 79

Table 14. Block Attributes............................................................................ 103
 RS274/NGC Interpreter - Version 3

1

1 Introduction

The RS274/NGC Interpreter (the Interpreter) is a software system that reads numerical control

code in the “NGC” dialect of the RS274 numerical control language and produces calls to a set of

canonical machining functions. The output of the Interpreter can be used to drive machining

centers with three to six axes. Two earlier versions of the RS274/NGC Interpreter were built. This

report describes a new version, version 3.

The Interpreter may be used either (1) in a stand-alone system, the “Stand-Alone Interpreter”

(SAI) that reads RS274/NGC control code and writes canonical machining function calls but does

not control physical equipment, or (2) integrated with an Enhanced Machine Controller (EMC)

system, as described below, to control a machining center.

This report is self-contained in regard to the RS274/NGC language, the canonical machining

functions, and the operation of the SAI; no other documents should be required to understand

them fully. The report is not self-contained with regard to EMC systems. The reader operating an

EMC system will need additional documentation.

The report does not deal with unimplemented alternatives or research issues.

1.1 Audience

This report is intended to be useful to:

• programmers writing RS274/NGC programs that will be run on an EMC controller or

tested on the SAI,

• machine operators running machining centers with EMC controllers,

• people installing the SAI software,

• software developers building controllers for machining centers,

• manufacturing researchers.

The beginning of each major section and appendix of the report describes the audience for the

section.

1.2 Background

1.2.1 Enhanced Machine Controller Project

The Intelligent Systems Division of the National Institute of Standards and Technology (NIST) is

carrying out an Enhanced Machine Controller project. The primary objective of the project is to

build a testbed for evaluating application programming interface standards for open-architecture

machine controllers. A secondary objective is to demonstrate implementations of the Next

Generation Controller (NGC) architecture.

1.2.2 Numerical Control Programming Language RS274

RS274 is a programming language for numerically controlled (NC) machine tools, which has

been used for many years. The most recent standard version of RS274 is RS274-D, which was

completed in 1979. It is described in the document “EIA Standard EIA-274-D” by the Electronic

Industries Association [EIA]. Most NC machine tools can be run using programs written in
 RS274/NGC Interpreter - Version 3

2

RS274. Implementations of the language differ from machine to machine, however, and a

program that runs on one machine probably will not run on one from a different maker.

1.2.3 The RS274/NGC Language

The NGC architecture has many independent parts, one of which is a specification for the RS274/

NGC language, a numerical control code language for machining and turning centers. The

specification was originally given in an August 24, 1992 report “RS274/NGC for the LOW END

CONTROLLER - First Draft” [Allen-Bradley] prepared by the Allen-Bradley company. A second

draft of that document was released in August 1994 by the National Center for Manufacturing

Sciences under the name “The Next Generation Controller Part Programming Functional

Specification (RS-274/NGC)” [NCMS]. All references in this report are to the second draft. The

RS274/NGC language has many capabilities beyond those of RS274-D.

In the remainder of this report, “the RS274/NGC language” means that portion of the

specification implemented in the EMC project (with modifications and additions). The report does

not provide specific references to parts of [NCMS] or discuss how the implementation differs

from it. The in-line documentation of the source code for the Interpreter, however, has many

references and discusses differences.

1.2.4 Previous Work at NIST

As part of its assistance to the program that developed the NGC architecture, the Intelligent

Systems Division prepared a report “NIST Support to the Next Generation Controller Program:

1991 Final Technical Report,” [Albus] containing a variety of suggestions. Appendix C to that

report proposed three sets of commands for 3-axis machining, one set for each of three proposed

hierarchical control levels. The suite proposed for the lowest (primitive) control level was

implemented in 1993 by the EMC project as a set of functions in the C programming language.

This suite, known in the EMC project and in this report as the “canonical machining functions,”

was upgraded in 1994 for 4-axis machining, and in 1995 for 5-axis machining. For the Interpreter,

the suite has been revised to be suitable for 3-axis to 6-axis machining.

Also in 1993, the authors developed a software system in the C language for reading machining

commands in the RS274/NGC language and outputting canonical machining functions. This was

called “the RS274/NGC Interpreter.” A report, “The NIST RS274/NGC Interpreter, Version 1”

[Kramer1] was published in April 1994 describing that interpreter.

In 1994, the EMC project, in collaboration with the General Motors Company (GM), undertook to

retrofit a 4-axis Kearney and Trecker 800 machining center with an EMC controller. The retrofit

was successfully completed in 1995. For this project, NIST built both Version 2 of the RS274/

NGC Interpreter and an RS274KT Interpreter, which interprets programs written in the K&T

dialect of RS274 [K&T]. These two interpreters were written in the C++ programming language.

Reports were written describing the RS274KT Interpreter [Kramer2] and version 2 of the RS274/

NGC Interpreter [Kramer3]. In addition, a report about the canonical machining functions was

written [Proctor] which extended them to six axes.

In 1995 the EMC project collaborated with several industrial partners in an open-architecture

machine tool controller project known as VGER (a name, not an acronym). This project retrofitted

an SNK 5-axis machining center with an open architecture controller. NIST provided the RS274

interpreter for this project [Kramer4]. It was intended to be able to interpret some existing

programs for the SNK machine which were written for its former Fanuc controller [Fanuc]. Thus,

the RS274/VGER Interpreter took Fanuc flavored RS274/NGC code as input.
 RS274/NGC Interpreter - Version 3

3

1.2.5 Current Work at NIST

The EMC project has provided the EMC controller to several small machine shops. Version 2 of

the RS274/NGC Interpreter, with numerous upgrades, has been used as the interpreter. In order to

be able to provide EMC controllers for 3-axis to 6-axis machining centers without having many

sets of source code to maintain, it was decided to build a single set of interpreter source code that

would serve for all. The Interpreter reported here is that one.

1.3 Major Characteristics of the Interpreter

1.3.1 How it Runs

When the Interpreter starts up, before accepting any input, it sets up a world model that includes

data about itself, parameter data, and data about the machining center being controlled (including

data about the tools in the tool carousel of the machine).

Once initialized, the Interpreter runs using a two-step process:

1. Get a line of RS274/NGC code and read it into memory, building an internal representation

of the meaning of the entire line. We will call this stage “reading.”

2. Change internal state and/or call one or more canonical machining functions (see Section

4) in order to do what the line says to do. We will call this “executing” the line.

The Interpreter runs integrated with the EMC system or in the SAI system. The Interpreter

software is the same in both cases. We will refer to the software that tells the Interpreter what to

do and asks it for data as the “driver,” regardless of whether it runs in the EMC system or in the

SAI.

If an error occurs, the Interpreter returns an error code to the driver. It is always possible to

recover from an error that occurs during reading. If an error occurs while executing the line,

recoverability is situation dependent.

1.3.2 Modes of Use

1.3.2.1 Integrated with EMC System

In the EMC system, the Interpreter is used both to interpret NC programs from files and to

interpret individual commands entered using the manual data input (MDI) capability of the

control system. When running an NC program from a file, the driver tells the Interpreter when to

read another line of code from the program file. When using MDI input, the driver sends the

Interpreter a line of code to read that the controller has received from its user interface. Either

way, the Interpreter reads the line and tells the driver if the line was readable. If so, the driver tells

the Interpreter to execute the line.

The Interpreter does not control machine action directly. Rather, the Interpreter calls canonical

machining functions that generate messages, which are passed back to the control system. The

control system queues up and executes the messages.

1.3.2.2 Stand-Alone Interpreter (SAI)

The SAI runs in a command window on any computer for which it is compiled. It also reads either

from a file or by MDI (from the keyboard of the computer). The SAI is intended to allow the pretesting of NC programs. It can also be used in MDI mode to experiment with the RS274/NGC

language and the Interpreter.
 RS274/NGC Interpreter - Version 3

4

2 Machining Center Overview

This section gives a brief description of how a machining center is viewed from the input and

output ends of the Interpreter. It is assumed the reader is already familiar with machining centers.

This section is intended to be useful to NC programmers, machine operators, developers, and

researchers. SAI installers will probably not find it useful.

The section describes the format of tool files, which are required for using the Interpreter but are

not known to either the RS274/NGC language or the canonical machining functions. Parameter

files, also required by the Interpreter, are described in Section 3.2.1.

2.1 Machining Centers

Both the RS274/NGC input language and the output canonical machining functions have a view

of (1) mechanical components of a machining center being controlled and (2) what activities of

the machining center may be controlled, and what data is used in control. The two views of the

mechanical components are very similar, the canonical machining function view including a few

more components. The two views of control and data differ significantly, with the canonical

machining function view being much simpler in most cases; the Interpreter deals with many

complexities of the RS274/NGC language so that lower levels of control do not have to. For

example, the RS274/NGC language includes a single command to perform a peck drilling cycle.

The Interpreter decomposes this complex single command into many simple straight_feed and

straight_traverse canonical function calls.

This section, Section 2, presents the elements that are shared between the two views. Unshared

elements of the two views are described in Section 3.2 (RS274/NGC language) and Section 4.2

(canonical machining functions).

The view here includes some items that a given machining center may not have, such as a pallet

shuttle. The RS274/NGC language and canonical machining functions may be used with such a

machine provided that no NC program used with the controller includes commands intended to

activate physical capabilities the machine does not have. For such a machine, it would be useful to

modify the Interpreter so it will reject input commands and will not produce output canonical

function calls addressed to non-existent equipment. For each of the A, B, and C axes, the

Interpreter source code already handles the case of the missing axis, as described in Section 5.2.

2.1.1 Mechanical Components

A machining center has many mechanical components that may be controlled or may affect the

way in which control is exercised. This section describes the subset of those components that

interact with the Interpreter. Mechanical components that do not interact directly with the

Interpreter, such as the jog buttons, are not described here, even if they affect control.

2.1.1.1 Linear Axes

A machining center has independent mechanisms1 for producing relative linear motion of the tool

1. If the motion of mechanical components is not independent, as with hexapod machines, the RS274/NGC

language and the canonical machining functions will still be usable, as long as the lower levels of control

know how to control the actual mechanisms to produce the same relative motion of tool and workpiece as

would be produced by independent axes.
 RS274/NGC Interpreter - Version 3

5

and workpiece in three mutually orthogonal directions. These are the X, Y and Z axes.

2.1.1.2 Rotational axes

Three additional independent mechanisms produce relative rotation of the workpiece and the tool

around an axis. These mechanisms (often a rotary table on which the workpiece is mounted or a

drum on which the spindle is mounted) are called rotational axes and labelled A, B, and C. The Aaxis is parallel to the X-axis. B is parallel to the Y-axis, and C parallel to the Z-axis1. Each

rotational mechanism may or may not have a mechanical limit on how far it can rotate.

2.1.1.3 Spindle

A machining center has a spindle which holds one cutting tool, probe, or other item. The spindle

can rotate in either direction, and it can be made to rotate at a constant rate, which may be

changed. Except on machines where the spindle may be moved by moving a rotational axis, the

axis of the spindle is kept parallel to the Z-axis and is coincident with the Z-axis when X and Y

are zero. The spindle can be stopped in a fixed orientation or stopped without specifying

orientation.

2.1.1.4 Coolant

A machining center has components to provide mist coolant and/or flood coolant. The canonical

machining functions view also has through-tool coolant; see Section 4.2.2.1.

2.1.1.5 Pallet Shuttle

A machining center has a pallet shuttle system. The system has two movable pallets on which

workpieces can be fixtured. Only one pallet at a time is in position for machining.

2.1.1.6 Tool Carousel

A machining center has a tool carousel with slots for tools fixed in tool holders.

2.1.1.7 Tool Changer

A machining center has a mechanism for changing tools (fixed in tool holders) between the

spindle and the tool carousel.

2.1.1.8 Message Display

A machining center has a device that can display messages.

2.1.1.9 Feed and Speed Override Switches

A machining center has separate feed and speed override switches, which let the operator specify

that the actual feed rate or spindle speed used in machining should be some percentage of the

programmed rate. See Section 2.1.2.15 and Section 2.2.1.

2.1.1.10 Block Delete Switch

A machining center has a block delete switch. See Section 2.2.2.

2.1.1.11 Optional Program Stop Switch

A machining center has an optional program stop switch. See Section 2.2.3.

1. The requirement of parallelism is not used by either language, so both languages are usable if any

rotational axis is not parallel to any linear axis. Rotational axis commands flow through both languages to

lower levels of control without significant change in nature.
 RS274/NGC Interpreter - Version 3

6

2.1.2 Control and Data Components

2.1.2.1 Linear Axes

The X, Y, and Z axes form a standard right-handed coordinate system of orthogonal linear axes.

Positions of the three linear motion mechanisms are expressed using coordinates on these axes.

2.1.2.2 Rotational Axes

The rotational axes are measured in degrees as wrapped linear axes in which the direction of

positive rotation is counterclockwise when viewed from the positive end of the corresponding X,

Y, or Z-axis. By “wrapped linear axis,” we mean one on which the angular position increases

without limit (goes towards plus infinity) as the axis turns counterclockwise and deceases without

limit (goes towards minus infinity) as the axis turns clockwise. Wrapped linear axes are used

regardless of whether or not there is a mechanical limit on rotation.

Clockwise or counterclockwise is from the point of view of the workpiece. If the workpiece is

fastened to a turntable which turns on a rotational axis, a counterclockwise turn from the point of

view of the workpiece is accomplished by turning the turntable in a direction that (for most

common machine configurations) looks clockwise from the point of view of someone standing

next to the machine.1

2.1.2.3 Controlled Point

The controlled point is the point whose position and rate of motion are controlled. When the tool

length offset is zero (the default value), this is a point on the spindle axis (often called the gauge

point) that is some fixed distance beyond the end of the spindle, usually near the end of a tool

holder that fits into the spindle. The location of the controlled point can be moved out along the

spindle axis by specifying some positive amount for the tool length offset. This amount is

normally the length of the cutting tool in use, so that the controlled point is at the end of the

cutting tool.

2.1.2.4 Coordinated Linear Motion

To drive a tool along a specified path, a machining center must often coordinate the motion of

several axes. We use the term “coordinated linear motion” to describe the situation in which,

nominally, each axis moves at constant speed and all axes move from their starting positions to

their end positions at the same time. If only the X, Y, and Z axes (or any one or two of them)

move, this produces motion in a straight line, hence the word “linear” in the term. In actual

motions, it is often not possible to maintain constant speed because acceleration or deceleration is

required at the beginning and/or end of the motion. It is feasible, however, to control the axes so

that, at all times, each axis has completed the same fraction of its required motion as the other

axes. This moves the tool along same path, and we also call this kind of motion coordinated linear

motion.

Coordinated linear motion can be performed either at the prevailing feed rate, or at traverse rate. If

physical limits on axis speed make the desired rate unobtainable, all axes are slowed to maintain

the desired path.

1. If the parallelism requirement is violated, the system builder will have to say how to distinguish clockwise

from counterclockwise.
 RS274/NGC Interpreter - Version 3

7

2.1.2.5 Feed Rate

The rate at which the controlled point or the axes move is nominally a steady rate which may be

set by the user. In the Interpreter, the interpretation of the feed rate is as follows unless inverse

time feed rate mode is being used in the RS274/NGC view (see Section 3.5.19). The canonical

machining functions view of feed rate, as described in Section 4.3.5.1, has conditions under which

the set feed rate is applied differently, but none of these is used in the Interpreter.

A. For motion involving one or more of the X, Y, and Z axes (with or without simultaneous

rotational axis motion), the feed rate means length units per minute along the

programmed XYZ path, as if the rotational axes were not moving.

B. For motion of one rotational axis with X, Y, and Z axes not moving, the feed rate means

degrees per minute rotation of the rotational axis.

C. For motion of two or three rotational axes with X, Y, and Z axes not moving, the rate is

applied as follows. Let dA, dB, and dC be the angles in degrees through which the A, B,

and C axes, respectively, must move. Let D = . Conceptually, D is a

measure of total angular motion, using the usual Euclidean metric. Let T be the amount

of time required to move through D degrees at the current feed rate in degrees per

minute. The rotational axes should be moved in coordinated linear motion so that the

elapsed time from the start to the end of the motion is T plus any time required for

acceleration or deceleration.

2.1.2.6 Arc Motion

Any pair of the linear axes (XY, YZ, XZ) can be controlled to move in a circular arc in the plane

of that pair of axes. While this is occurring, the third linear axis and the rotational axes can be

controlled to move simultaneously at effectively a constant rate. As in coordinated linear motion,

the motions can be coordinated so that acceleration and deceleration do not affect the path.

If the rotational axes do not move, but the third linear axis does move, the trajectory of the

controlled point is a helix.

The feed rate during arc motion is as described in item A of Section 2.1.2.5, immediately above.

In the case of helical motion, the rate is applied along the helix. In some other versions of RS274,

the rate is applied to the circular arc which is the projection of the helix on the selected plane.

2.1.2.7 Coolant

Flood coolant and mist coolant may each be turned on independently. The RS274/NGC language

turns them off together (see Section 3.6.4) while the canonical machining functions turn them off

independently (see Section 4.3.9).

2.1.2.8 Dwell

A machining center may be commanded to dwell (i.e., keep all axes unmoving) for a specific

amount of time. The most common use of dwell is to break and clear chips, so the spindle is

usually turning during a dwell.

2.1.2.9 Units

Units used for distances along the X, Y, and Z axes may be measured in millimeters or inches.

Units for all other quantities involved in machine control cannot be changed. Different quantities

( ) dA 2 ( ) dB 2 ( ) dC 2 + +
 RS274/NGC Interpreter - Version 3

8

use different specific units. Spindle speed is measured in revolutions per minute. The positions of

rotational axes are measured in degrees. Feed rates are expressed in current length units per

minute or in degrees per minute, as described in Section 2.1.2.5.

2.1.2.10 Current Position

The controlled point is always at some location called the “current position,” and the controller

always knows where that is. The numbers representing the current position must be adjusted in

the absence of any axis motion if any of several events take place:

1. Length units are changed.

2. Tool length offset is changed.

3. Coordinate system offsets are changed.

2.1.2.11 Selected Plane

There is always a “selected plane”, which must be the XY-plane, the YZ-plane, or the XZ-plane of

the machining center. The Z-axis is, of course, perpendicular to the XY-plane, the X-axis to the

YZ-plane, and the Y-axis to the XZ-plane.

2.1.2.12 Tool Carousel

Zero or one tool is assigned to each slot in the tool carousel.

2.1.2.13 Tool Change

A machining center may be commanded to change tools.

2.1.2.14 Pallet Shuttle

The two pallets may be exchanged by command.

2.1.2.15 Feed and Speed Override Switches

The feed and speed override switches may be enabled (so they work as expected) or disabled (so

they have no effect on the feed rate or spindle speed). The RS274/NGC language has one

command that enables both switches and one command that disables both (see Section 3.6.5). The

canonical machining functions have separate commands for the two switches (see Section 4.3.9).

See Section 2.2.1 for further details.

2.1.2.16 Path Control Mode

The machining center may be put into any one of three path control modes: (1) exact stop mode,

(2) exact path mode, or (3) continuous mode. In exact stop mode, the machine stops briefly at the

end of each programmed move. In exact path mode, the machine follows the programmed path as

exactly as possible, slowing or stopping if necessary at sharp corners of the path. In continuous

mode, sharp corners of the path may be rounded slightly so that the feed rate may be kept up. See

Section 3.5.14 and Section 4.3.5.3

The canonical machining functions share with the RS274 language the simplifying assumption

that machine dynamics can be almost ignored. That is, in this model, acceleration and

deceleration do not occur. Components of the machining center can be told to move at a specific

rate, and that rate is imagined as being achieved instantaneously. Stopping is also imagined as

instantaneous. This model obviously does not correspond with reality. The control modes

provided here provide some compensation for this lack of consideration of dynamics.
 RS274/NGC Interpreter - Version 3

9

2.2 Interpreter Interaction with Switches

As noted in Section 2.1.2, the Interpreter interacts with three switches. This section describes the

interactions in more detail. In no case does the Interpreter know what the setting of any of these

switches is.

2.2.1 Feed and Speed Override Switches

The Interpreter will interpret RS274/NGC commands which enable (M48) or disable (M49) the

feed and speed override switches and will make canonical machining function calls to enable or

disable them (Section 4.3.9). It is useful to be able to override these switches for some machining

operations. The idea is that optimal settings have been included in the program, and the operator

should not change them.

The EMC control system reacts to the setting of the speed or feed override switches on the control

panel, when these switches are enabled.

The SAI does not emulate these switches.

2.2.2 Block Delete Switch

If the block delete switch is on, lines of RS274/NGC code which start with a slash (the block

delete character) are not interpreted. If the switch is off, such lines are interpreted.

As outlined in Section 1.3.1, the Interpreter runs in two stages (read and execute). The driver tells

the Interpreter when to perform each stage. When the Interpreter reads a line starting with a slash,

it informs the driver, “I just read a line starting with a slash.” The driver checks the setting of the

block delete switch. If the switch is off, it tells the Interpreter, “Execute that line.” If the switch is

on, the driver does not tell the Interpreter to execute the line. Instead, it tells the Interpreter to read

another line, with the result that the line starting with the slash is not executed.

In the SAI, the block delete switch may be set, and its default setting is off.

2.2.3 Optional Program Stop Switch

The optional program stop switch works as follows. If this switch is on and an input RS274/NGC

code line contains an M1 code, program execution is supposed to stop until the cycle start button

is pushed. The Interpreter interprets an M1 on an input line into an

OPTIONAL_PROGRAM_STOP canonical function call in the output (see Section 4.3.10).

When the Interpreter is integrated with the EMC system, the controller checks the optional stop

switch when the OPTIONAL_PROGRAM_STOP canonical function call is executed and either

stops (if the switch is on) or not (if the switch is off).

The SAI does not emulate the optional program stop switch.

2.3 Tool File

A tool file is required to use the Interpreter. The file tells which tools are in which carousel slots

and what the length and diameter of each tool are.

The Interpreter does not deal directly with tool files. A tool file is read either by the EMC system

or the SAI, as the case may be, and the Interpreter gets the tool information by making calls to

canonical functions that obtain it from the EMC system or SAI.
 RS274/NGC Interpreter - Version 3

10

The format of a tool file is exemplified in Table 1.

The file consists of any number of header lines, followed by one blank line, followed by any

number of lines of data. The header lines are ignored. It is important that there be exactly one

blank line (with no spaces or tabs, even) before the data. The header line shown in Table 1

describes the data columns, so it is suggested (but not required) that such a line always be

included in the header.

Each data line of the file contains the data for one tool. Each line has five entries. The first four

entries are required. The last entry (a comment) is optional. It makes reading easier if the entries

are arranged in columns, as shown in the table, but the only format requirement is that there be at

least one space or tab after each of the first three entries on a line and a space, tab, or newline at

the end of the fourth entry. The meanings of the columns and the type of data to be put in each are

as follows.

The “POCKET” column contains an unsigned integer which represents the pocket number (slot

number) of the tool carousel slot in which the tool is placed. The entries in this column must all be

different.

The “FMS” column contains an unsigned integer which represents a code number for the tool.

The user may use any code for any tool, as long as the codes are unsigned integers.

The “TLO” column contains a real number which represents the tool length offset. This number

will be used if tool length offsets are being used and this pocket is selected. This is normally a

positive real number, but it may be zero or any other number if it is never to be used.

The “DIAM” column contains a real number. This number is used only if tool radius

compensation is turned on using this pocket. If the programmed path during compensation is the

edge of the material being cut, this should be a positive real number representing the measured

diameter of the tool. If the programmed path during compensation is the path of a tool whose

diameter is nominal, this should be a small number (positive, negative, or zero) representing the

difference between the measured diameter of the tool and the nominal diameter. If cutter radius

compensation is not used with a tool, it does not matter what number is in this column.

The “Comment” column may optionally be used to describe the tool. Any type of description is

OK. This column is for the benefit of human readers only.

The SAI only reads data from the first four columns of each line. The rest of the line is read but

ignored.

The units used for the length and diameter of the tool may be in either millimeters or inches, but if

the data is used by an NC program, the user must be sure the units used for a tool in the file are the

same as the units in effect when NC code that uses the tool data is interpreted. The table shows a

mixture of types of units.

The lines do not have to be in any particular order. Switching the order of lines has no effect on

the SAI (unless the same slot number is used on two or more lines, which should not normally be

done, in which case the data for only the last such line will persist).
 RS274/NGC Interpreter - Version 3

11

POCKET FMS TLO DIAMETER COMMENT

1 1 2.0 1.0

2 2 1.0 0.2

5 5 1.5 0.25 endmill

10 10 2.4 -0.3 for testing

21 21 173.740 0 1/2” spot drill

32 32 247.615 0 8.5 mm drill

41 41 228.360 0 10 mm tap

60 60 0 0 large chuck

Table 1. Sample Tool File
 RS274/NGC Interpreter - Version 3

12

3 Input: the RS274/NGC Language

This section describes the input language, RS274/NGC. This section is intended for NC

programmers, machine operators, developers and researchers. SAI installers can skip it.

3.1 Overview

The RS274/NGC language is based on lines of code. Each line (also called a “block”) may

include commands to a machining center to do several different things. Lines of code may be

collected in a file to make a program.

A typical line of code consists of an optional line number at the beginning followed by one or

more “words.” A word consists of a letter followed by a number (or something that evaluates to a

number). A word may either give a command or provide an argument to a command. For

example, “G1 X3” is a valid line of code with two words. “G1” is a command meaning “move in

a straight line at the programmed feed rate,” and “X3” provides an argument value (the value of X

should be 3 at the end of the move). Most RS274/NGC commands start with either G or M (for

miscellaneous). The words for these commands are called “G codes” and “M codes.”

The RS274/NGC language has no indicator for the start of a program. The Interpreter, however,

deals with files. A single program may be in a single file, or a program may be spread across

several files. A file may demarcated with percents in the following way. The first non-blank line of

a file may contain nothing but a percent sign, “%”, possibly surrounded by white space, and later

in the file (normally at the end of the file) there may be a similar line. Demarcating a file with

percents is optional if the file has an M2 or M30 in it, but is required if not. An error will be

signalled if a file has a percent line at the beginning but not at the end. The useful contents of a file

demarcated by percents stop after the second percent line. Anything after that is ignored.

The RS274/NGC language has two commands (M2 or M30), either of which ends a program. A

program may end before the end of a file. Lines of a file that occur after the end of a program are

not to be executed. The SAI does not even read them.

3.2 RS274/NGC Language View of a Machining Center

The RS274/NGC language is based on a particular view of what a machining center to be

controlled is like. The view is as described in Section 2.1, with the changes described below. The

RS274/NGC language view includes one mechanical component not known to the canonical

machining functions: a cycle start button. The use of the button is described in Section 3.6.1.

The RS274/NGC language contains commands that change the way subsequent commands are to

be interpreted, but do not tell the machining center to do anything. These are not covered in this

section, but are dealt with as they arise in Section 3.5.17, Section 3.5.19, and Section 3.5.20.

3.2.1 Parameters

In the RS274/NGC language view, a machining center maintains an array of 5400 numerical

parameters. Many of them have specific uses. The parameter array should persist over time, even

if the machining center is powered down. The RS274/NGC language makes no provision

regarding how to ensure persistence. The EMC project uses a parameter file to ensure persistence

and gives the Interpreter the responsibility for maintaining the file. The Interpreter reads the file

when it starts up, and writes the file when it exits.
 RS274/NGC Interpreter - Version 3

13

Parameter

number

Parameter

value Comment Parameter

number

Parameter

value Comment

5161

5162

5163

5164

5165

5166

5181

5182

5183

5184

5185

5186

5211

5212

5213

5214

5215

5216

5220

5221

5222

5223

5224

5225

5226

5241

5242

5243

5244

5245

5246

5261

5262

5263

5264

5265

5266

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

1.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

G28 home X

G28 home Y

G28 home Z

G28 home A

G28 home B

G28 home C

G30 home X

G30 home Y

G30 home Z

G30 home A

G30 home B

G30 home C

G92 offset X

G92 offset Y

G92 offset Z

G92 offset A

G92 offset B

G92 offset C

coord. system number

coord. system 1 X

coord. system 1 Y

coord. system 1 Z

coord. system 1 A

coord. system 1 B

coord. system 1 C

coord. system 2 X

coord. system 2 Y

coord. system 2 Z

coord. system 2 A

coord. system 2 B

coord. system 2 C

coord. system 3 X

coord. system 3 Y

coord. system 3 Z

coord. system 3 A

coord. system 3 B

coord. system 3 C

5281

5282

5283

5284

5285

5286

5301

5302

5303

5304

5305

5306

5321

5322

5323

5324

5325

5326

5341

5342

5343

5344

5345

5346

5361

5362

5363

5364

5365

5366

5381

5382

5383

5384

5385

5386

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

0.0

coord. system 4 X

coord. system 4 Y

coord. system 4 Z

coord. system 4 A

coord. system 4 B

coord. system 4 C

coord. system 5 X

coord. system 5 Y

coord. system 5 Z

coord. system 5 A

coord. system 5 B

coord. system 5 C

coord. system 6 X

coord. system 6 Y

coord. system 6 Z

coord. system 6 A

coord. system 6 B

coord. system 6 C

coord. system 7 X

coord. system 7 Y

coord. system 7 Z

coord. system 7 A

coord. system 7 B

coord. system 7 C

coord. system 8 X

coord. system 8 Y

coord. system 8 Z

coord. system 8 A

coord. system 8 B

coord. system 8 C

coord. system 9 X

coord. system 9 Y

coord. system 9 Z

coord. system 9 A

coord. system 9 B

coord. system 9 C

Table 2. Default Parameter File

Actual file is in 3 columns, not 6. A, B, and C values are conditional. Comments are optional. All

the parameters in this file are required. All values are set to 0.0, except 5220 is 1.0.
 RS274/NGC Interpreter - Version 3

14

The format of a parameter file is shown in Table 2. The file consists of any number of header lines,

followed by one blank line, followed by any number of lines of data. The Interpreter skips over

the header lines. It is important that there be exactly one blank line (with no spaces or tabs, even)

before the data. The header line shown in Table 2 describes the data columns, so it is suggested

(but not required) that that line always be included in the header.

The Interpreter reads only the first two columns of the table. The third column, “Comment,” is not

read by the Interpreter.

Each line of the file contains the index number of a parameter in the first column and the value to

which that parameter should be set in the second column. The value is represented as a doubleprecision floating point number inside the Interpreter, but a decimal point is not required in the

file. All of the parameters shown in Table 2 are required parameters and must be included in any

parameter file, except that any parameter representing a rotational axis value for an unused axis

may be omitted. An error will be signalled if any required parameter is missing. A parameter file

may include any other parameter, as long as its number is in the range 1 to 5400. The parameter

numbers must be arranged in ascending order. An error will be signalled if not. Any parameter

included in the file read by the Interpreter will be included in the file it writes as it exits. The

original file is saved as a backup file when the new file is written.

3.2.2 Coordinate Systems

In the RS274/NGC language view, a machining center has an absolute coordinate system and nine

program coordinate systems.

You can set the offsets of the nine program coordinate systems using G10 L2 Pn (n is the number

of the coordinate system) with values for the axes in terms of the absolute coordinate system. See

Section 3.5.5.

You can select one of the nine systems by using G54, G55, G56, G57, G58, G59, G59.1, G59.2, or

G59.3 (see Section 3.5.13). It is not possible to select the absolute coordinate system directly.

You can offset the current coordinate system using G92 or G92.3. This offset will then apply to all

nine program coordinate systems. This offset may be cancelled with G92.1 or G92.2. See Section

3.5.18.

You can make straight moves in the absolute machine coordinate system by using G53 with either

G0 or G1. See Section 3.5.12.

Data for coordinate systems is stored in parameters.

During initialization, the coordinate system is selected that is specified by parameter 5220. A

value of 1 means the first coordinate system (the one G54 activates), a value of 2 means the

second coordinate system (the one G55 activates), and so on. It is an error for the value of

parameter 5220 to be anything but a whole number between one and nine.

3.3 Format of a Line

A permissible line of input RS274/NGC code consists of the following, in order, with the

restriction that there is a maximum (currently 256) to the number of characters allowed on a line.

1. an optional block delete character, which is a slash “/” .

2. an optional line number.
 RS274/NGC Interpreter - Version 3

15

3. any number of words, parameter settings, and comments.

4. an end of line marker (carriage return or line feed or both).

Any input not explicitly allowed is illegal and will cause the Interpreter to signal an error.

To make the specification of an allowable line of code precise, we have defined it in a production

language (Wirth Syntax Notation) in Appendix E.

Spaces and tabs are allowed anywhere on a line of code and do not change the meaning of the

line, except inside comments. This makes some strange-looking input legal. The line “g0x +0. 12

34y 7” is equivalent to “g0 x+0.1234 y7”, for example.

Blank lines are allowed in the input. They are to be ignored.

Input is case insensitive, except in comments, i.e., any letter outside a comment may be in upper

or lower case without changing the meaning of a line.

3.3.1 Line Number

A line number is the letter N followed by an integer (with no sign) between 0 and 99999 written

with no more than five digits (000009 is not OK, for example). Line numbers may be repeated or

used out of order, although normal practice is to avoid such usage. Line numbers may also be

skipped, and that is normal practice. A line number is not required to be used, but must be in the

proper place if used.

3.3.2 Word

A word is a letter other than N followed by a real value.

Words may begin with any of the letters shown in Table 3. The table includes N for completeness,

even though, as defined above, line numbers are not words. Several letters (I, J, K, L, P, R) may

have different meanings in different contexts.
 RS274/NGC Interpreter - Version 3

16

Letter Meaning

A A-axis of machine

B B-axis of machine

C C-axis of machine

D tool radius compensation number

F feedrate

G general function (see Table 5)

H tool length offset index

I X-axis offset for arcs

X offset in G87 canned cycle

J Y-axis offset for arcs

Y offset in G87 canned cycle

K Z-axis offset for arcs

Z offset in G87 canned cycle

L number of repetitions in canned cycles

key used with G10

M miscellaneous function (see Table 7)

N line number

P dwell time in canned cycles

dwell time with G4

key used with G10

Q feed increment in G83 canned cycle

R arc radius

canned cycle plane

S spindle speed

T tool selection

X X-axis of machine

Y Y-axis of machine

Z Z-axis of machine

Table 3. Word-starting Letters
 RS274/NGC Interpreter - Version 3

17

A real value is some collection of characters that can be processed to come up with a number. A

real value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression,

or a unary operation value. Definitions of these follow immediately. Processing characters to

come up with a number is called “evaluating”. An explicit number evaluates to itself.

3.3.2.1 Number

The following rules are used for (explicit) numbers. In these rules a digit is a single character

between 0 and 9.

• A number consists of (1) an optional plus or minus sign, followed by (2) zero to many

digits, followed, possibly, by (3) one decimal point, followed by (4) zero to many

digits — provided that there is at least one digit somewhere in the number.

• There are two kinds of numbers: integers and decimals. An integer does not have a

decimal point in it; a decimal does.

• Numbers may have any number of digits, subject to the limitation on line length. Only

about seventeen significant figures will be retained, however (enough for all known

applications).

• A non-zero number with no sign as the first character is assumed to be positive.

Notice that initial (before the decimal point and the first non-zero digit) and trailing (after the

decimal point and the last non-zero digit) zeros are allowed but not required. A number written

with initial or trailing zeros will have the same value when it is read as if the extra zeros were not

there.

Numbers used for specific purposes in RS274/NGC are often restricted to some finite set of values

or some to some range of values. In many uses, decimal numbers must be close to integers; this

includes the values of indexes (for parameters and carousel slot numbers, for example), M codes,

and G codes multiplied by ten. A decimal number which is supposed be close to an integer is

considered close enough if it is within 0.0001 of an integer.

3.3.2.2 Parameter Value

A parameter value is the pound character # followed by a real value. The real value must evaluate

to an integer between 1 and 5399. The integer is a parameter number, and the value of the

parameter value is whatever number is stored in the numbered parameter.

The # character takes precedence over other operations, so that, for example, “#1+2” means the

number found by adding 2 to the value of parameter 1, not the value found in parameter 3. Of

course, #[1+2] does mean the value found in parameter 3. The # character may be repeated; for

example ##2 means the value of the parameter whose index is the (integer) value of parameter 2.

3.3.2.3 Expressions and Binary Operations

An expression is a set of characters starting with a left bracket [ and ending with a balancing right

bracket ]. In between the brackets are numbers, parameter values, mathematical operations, and

other expressions. An expression may be evaluated to produce a number. The expressions on a

line are evaluated when the line is read, before anything on the line is executed. An example of an

expression is [ 1 + acos[0] - [#3 ** [4.0/2]]].

Binary operations appear only inside expressions. Nine binary operations are defined. There are
 RS274/NGC Interpreter - Version 3

18

four basic mathematical operations: addition (+), subtraction (-), multiplication (*), and division (/

). There are three logical operations: non-exclusive or (OR), exclusive or (XOR), and logical and

(AND). The eighth operation is the modulus operation (MOD). The ninth operation is the

“power” operation (**) of raising the number on the left of the operation to the power on the right.

The binary operations are divided into three groups. The first group is: power. The second group

is: multiplication, division, and modulus. The third group is: addition, subtraction, logical nonexclusive or, logical exclusive or, and logical and. If operations are strung together (for example

in the expression [2.0 / 3 * 1.5 - 5.5 / 11.0]), operations in the first group are to be performed

before operations in the second group and operations in the second group before operations in the

third group. If an expression contains more than one operation from the same group (such as the

first / and * in the example), the operation on the left is performed first. Thus, the example is

equivalent to: [((2.0 / 3) * 1.5) - (5.5 / 11.0)] , which simplifies to [1.0 - 0.5] , which is 0.5.

The logical operations and modulus are to be performed on any real numbers, not just on integers.

The number zero is equivalent to logical false, and any non-zero number is equivalent to logical

true.

3.3.2.4 Unary Operation Value

A unary operation value is either “ATAN” followed by one expression divided by another

expression (for example “ATAN[2]/[1+3]”) or any other unary operation name followed by an

expression (for example “SIN[90]”). The unary operations are: ABS (absolute value), ACOS (arc

cosine), ASIN (arc sine), ATAN (arc tangent), COS (cosine), EXP (e raised to the given power),

FIX (round down), FUP (round up), LN (natural logarithm), ROUND (round to the nearest whole

number), SIN (sine), SQRT (square root), and TAN (tangent). Arguments to unary operations

which take angle measures (COS, SIN, and TAN) are in degrees. Values returned by unary

operations which return angle measures (ACOS, ASIN, and ATAN) are also in degrees.

The FIX operation rounds towards the left (less positive or more negative) on a number line, so

that FIX[2.8] =2 and FIX[-2.8] = -3, for example. The FUP operation rounds towards the right

(more positive or less negative) on a number line; FUP[2.8] = 3 and FUP[-2.8] = -2, for example.

3.3.3 Parameter Setting

A parameter setting is the following four items one after the other: (1) a pound character # , (2) a

real value which evaluates to an integer between 1 and 5399, (3) an equal sign = , and (4) a real

value. For example “#3 = 15” is a parameter setting meaning “set parameter 3 to 15.”

A parameter setting does not take effect until after all parameter values on the same line have been

found. For example, if parameter 3 has been previously set to 15 and the line “#3=6 G1 x#3” is

interpreted, a straight move to a point where x equals 15 will occur and the value of parameter 3

will be 6.

3.3.4 Comments and Messages

Printable characters and white space inside parentheses is a comment. A left parenthesis always

starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left

parenthesis is placed on a line, a matching right parenthesis must appear before the end of the line.

Comments may not be nested; it is an error if a left parenthesis is found after the start of a

comment and before the end of the comment. Here is an example of a line containing a comment:

“G80 M5 (stop motion)”. Comments do not cause a machining center to do anything.
 RS274/NGC Interpreter - Version 3

19

A comment contains a message if “MSG,” appears after the left parenthesis and before any other

printing characters. Variants of “MSG,” which include white space and lower case characters are

allowed. The rest of the characters before the right parenthesis are considered to be a message.

Messages should be displayed on the message display device. Comments not containing messages

need not be displayed there.

3.3.5 Item Repeats

A line may have any number of G words, but two G words from the same modal group (see

Section 3.4) may not appear on the same line.

A line may have zero to four M words. Two M words from the same modal group may not appear

on the same line.

For all other legal letters, a line may have only one word beginning with that letter.

If a parameter setting of the same parameter is repeated on a line, “#3=15 #3=6”, for example,

only the last setting will take effect. It is silly, but not illegal, to set the same parameter twice on

the same line.

If more than one comment appears on a line, only the last one will be used; each of the other

comments will be read and its format will be checked, but it will be ignored thereafter. It is

expected that putting more than one comment on a line will be very rare.

3.3.6 Item order

The three types of item whose order may vary on a line (as given at the beginning of this section)

are word, parameter setting, and comment. Imagine that these three types of item are divided into

three groups by type.

The first group (the words) may be reordered in any way without changing the meaning of the

line.

If the second group (the parameter settings) is reordered, there will be no change in the meaning

of the line unless the same parameter is set more than once. In this case, only the last setting of the

parameter will take effect. For example, after the line “#3=15 #3=6” has been interpreted, the

value of parameter 3 will be 6. If the order is reversed to “#3=6 #3=15” and the line is interpreted,

the value of parameter 3 will be 15.

If the third group (the comments) contains more than one comment and is reordered, only the last

comment will be used.

If each group is kept in order or reordered without changing the meaning of the line, then the three

groups may be interleaved in any way without changing the meaning of the line. For example, the

line “g40 g1 #3=15 (foo) #4=-7.0” has five items and means exactly the same thing in any of the

120 possible orders (such as “#4=-7.0 g1 #3=15 g40 (foo)”) for the five items.

3.3.7 Commands and Machine Modes

In RS274/NGC, many commands cause a machining center to change from one mode to another,

and the mode stays active until some other command changes it implicitly or explicitly. Such

commands are called “modal”. For example, if coolant is turned on, it stays on until it is explicitly

turned off. The G codes for motion are also modal. If a G1 (straight move) command is given on

one line, for example, it will be executed again on the next line if one or more axis words is
 RS274/NGC Interpreter - Version 3

20

available on the line, unless an explicit command is given on that next line using the axis words or

cancelling motion.

“Non-modal” codes have effect only on the lines on which they occur. For example, G4 (dwell) is

non-modal.

3.4 Modal Groups

Modal commands are arranged in sets called “modal groups”, and only one member of a modal

group may be in force at any given time. In general, a modal group contains commands for which

it is logically impossible for two members to be in effect at the same time — like measure in

inches vs. measure in millimeters. A machining center may be in many modes at the same time,

with one mode from each modal group being in effect. The modal groups are shown in Table 4.

For several modal groups, when a machining center is ready to accept commands, one member of

the group must be in effect. There are default settings for these modal groups. When the

machining center is turned on or otherwise re-initialized, the default values are automatically in

effect.

Group 1, the first group on the table, is a group of G codes for motion. One of these is always in

effect. That one is called the current motion mode.

It is an error to put a G-code from group 1 and a G-code from group 0 on the same line if both of

them use axis words. If an axis word-using G-code from group 1 is implicitly in effect on a line

The modal groups for G codes are:

group 1 = {G0, G1, G2, G3, G38.2, G80, G81, G82, G83, G84, G85, G86, G87, G88, G89} motion

group 2 = {G17, G18, G19} plane selection

group 3 = {G90, G91} distance mode

group 5 = {G93, G94} feed rate mode

group 6 = {G20, G21} units

group 7 = {G40, G41, G42} cutter radius compensation

group 8 = {G43, G49} tool length offset

group 10 = {G98, G99} return mode in canned cycles

group 12 = {G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3} coordinate system selection

group 13 = {G61, G61.1, G64} path control mode

The modal groups for M codes are:

group 4 = {M0, M1, M2, M30, M60} stopping

group 6 = {M6} tool change

group 7 = {M3, M4, M5} spindle turning

group 8 = {M7, M8, M9} coolant (special case: M7 and M8 may be active at the same time)

group 9 = {M48, M49} enable/disable feed and speed override switches

In addition to the above modal groups, there is a group for non-modal G codes:

group 0 = {G4, G10, G28, G30, G53, G92, G92.1, G92.2, G92.3}

Table 4. Modal Groups
 RS274/NGC Interpreter - Version 3

21

(by having been activated on an earlier line), and a group 0 G-code that uses axis words appears

on the line, the activity of the group 1 G-code is suspended for that line. The axis word-using Gcodes from group 0 are G10, G28, G30, and G92.

3.5 G Codes

G codes of the RS274/NGC language are shown in Table 5 and described following that.

The descriptions contain command prototypes, set in helvetica type.

In the command prototypes, three dots (...) stand for a real value. As described earlier, a real

value may be (1) an explicit number, 4, for example, (2) an expression, [2+2], for example, (3) a

parameter value, #88, for example, or (4) a unary function value, acos[0], for example.

In most cases, if axis words (any or all of X..., Y..., Z..., A..., B..., C...) are given, they specify

a destination point. Axis numbers are in the currently active coordinate system, unless explicitly

described as being in the absolute coordinate system. Where axis words are optional, any omitted

axes will have their current value. Any items in the command prototypes not explicitly described

as optional are required. It is an error if a required item is omitted.

In the prototypes, the values following letters are often given as explicit numbers. Unless stated

otherwise, the explicit numbers can be real values. For example, G10 L2 could equally well be

written G[2*5] L[1+1]. If the value of parameter 100 were 2, G10 L#100 would also mean the

same. Using real values which are not explicit numbers as just shown in the examples is rarely

useful.

If L... is written in a prototype the “...” will often be referred to as the “L number”. Similarly the

“...” in H... may be called the “H number”, and so on for any other letter.
 RS274/NGC Interpreter - Version 3

22

G Code Meaning

G0 rapid positioning

G1 linear interpolation

G2 circular/helical interpolation (clockwise)

G3 circular/helical interpolation (counterclockwise)

G4 dwell

G10 coordinate system origin setting

G17 XY-plane selection

G18 XZ-plane selection

G19 YZ-plane selection

G20 inch system selection

G21 millimeter system selection

G28 return to home

G30 return to secondary home

G38.2 straight probe

G40 cancel cutter radius compensation

G41 start cutter radius compensation left

G42 start cutter radius compensation right

G43 tool length offset (plus)

G49 cancel tool length offset

G53 motion in machine coordinate system

G54 use preset work coordinate system 1

G55 use preset work coordinate system 2

G56 use preset work coordinate system 3

G57 use preset work coordinate system 4

G58 use preset work coordinate system 5

G59 use preset work coordinate system 6

G59.1 use preset work coordinate system 7

G59.2 use preset work coordinate system 8

G59.3 use preset work coordinate system 9

G61 set path control mode: exact path

G61.1 set path control mode: exact stop

G64 set path control mode: continuous

G80 cancel motion mode (including any canned cycle)

G81 canned cycle: drilling

G82 canned cycle: drilling with dwell

G83 canned cycle: peck drilling

G84 canned cycle: right hand tapping

G85 canned cycle: boring, no dwell, feed out

G86 canned cycle: boring, spindle stop, rapid out

G87 canned cycle: back boring

G88 canned cycle: boring, spindle stop, manual out

G89 canned cycle: boring, dwell, feed out

G90 absolute distance mode

G91 incremental distance mode

G92 offset coordinate systems and set parameters

G92.1 cancel offset coordinate systems and set parameters to zero

G92.2 cancel offset coordinate systems but do not reset parameters

G92.3 apply parameters to offset coordinate systems

G93 inverse time feed rate mode

G94 units per minute feed rate mode

G98 initial level return in canned cycles

G99 R-point level return in canned cycles

Table 5. G Codes
 RS274/NGC Interpreter - Version 3

23

3.5.1 Rapid Linear Motion — G0

For rapid linear motion, program G0 X... Y... Z... A... B... C..., where all the axis words are

optional, except that at least one must be used. The G0 is optional if the current motion mode is

G0. This will produce coordinated linear motion to the destination point at the current traverse

rate (or slower if the machine will not go that fast). It is expected that cutting will not take place

when a G0 command is executing.

It is an error if:

• all axis words are omitted.

If cutter radius compensation is active, the motion will differ from the above; see Appendix B. If

G53 is programmed on the same line, the motion will also differ; see Section 3.5.12.

3.5.2 Linear Motion at Feed Rate — G1

For linear motion at feed rate (for cutting or not), program G1 X... Y... Z... A... B... C...,

where all the axis words are optional, except that at least one must be used. The G1 is optional if

the current motion mode is G1. This will produce coordinated linear motion to the destination

point at the current feed rate (or slower if the machine will not go that fast).

It is an error if:

• all axis words are omitted.

If cutter radius compensation is active, the motion will differ from the above; see Appendix B. If

G53 is programmed on the same line, the motion will also differ; see Section 3.5.12.

3.5.3 Arc at Feed Rate — G2 and G3

A circular or helical arc is specified using either G2 (clockwise arc) or G3 (counterclockwise arc).

The axis of the circle or helix must be parallel to the X, Y, or Z-axis of the machine coordinate

system. The axis (or, equivalently, the plane perpendicular to the axis) is selected with G17 (Zaxis, XY-plane), G18 (Y-axis, XZ-plane), or G19 (X-axis, YZ-plane). If the arc is circular, it lies

in a plane parallel to the selected plane.

If a line of RS274/NGC code makes an arc and includes rotational axis motion, the rotational axes

turn at a constant rate so that the rotational motion starts and finishes when the XYZ motion starts

and finishes. Lines of this sort are hardly ever programmed.

If cutter radius compensation is active, the motion will differ from what is described here. See

Appendix B.

Two formats are allowed for specifying an arc. We will call these the center format and the radius

format. In both formats the G2 or G3 is optional if it is the current motion mode.

3.5.3.1 Radius Format Arc

In the radius format, the coordinates of the end point of the arc in the selected plane are specified

along with the radius of the arc. Program G2 X... Y... Z... A... B... C... R... (or use G3 instead

of G2). R is the radius. The axis words are all optional except that at least one of the two words for

the axes in the selected plane must be used. The R number is the radius. A positive radius

indicates that the arc turns through 180 degrees or less, while a negative radius indicates a turn of

180 degrees to 359.999 degrees. If the arc is helical, the value of the end point of the arc on the
 RS274/NGC Interpreter - Version 3

24

coordinate axis parallel to the axis of the helix is also specified.

It is an error if:

• both of the axis words for the axes of the selected plane are omitted,

• the end point of the arc is the same as the current point.

It is not good practice to program radius format arcs that are nearly full circles or are semicircles

(or nearly semicircles) because a small change in the location of the end point will produce a

much larger change in the location of the center of the circle (and, hence, the middle of the arc).

The magnification effect is large enough that rounding error in a number can produce out-oftolerance cuts. Nearly full circles are outrageously bad, semicircles (and nearly so) are only very

bad. Other size arcs (in the range tiny to 165 degrees or 195 to 345 degrees) are OK.

Here is an example of a radius format command to mill an arc: G17 G2 x 10 y 15 r 20 z 5.

That means to make a clockwise (as viewed from the positive Z-axis) circular or helical arc whose

axis is parallel to the Z-axis, ending where X=10, Y=15, and Z=5, with a radius of 20. If the

starting value of Z is 5, this is an arc of a circle parallel to the XY-plane; otherwise it is a helical

arc.

3.5.3.2 Center Format Arc

In the center format, the coordinates of the end point of the arc in the selected plane are specified

along with the offsets of the center of the arc from the current location. In this format, it is OK if

the end point of the arc is the same as the current point. It is an error if:

• when the arc is projected on the selected plane, the distance from the current point to

the center differs from the distance from the end point to the center by more than

0.0002 inch (if inches are being used) or 0.002 millimeter (if millimeters are being

used).

When the XY-plane is selected, program G2 X... Y... Z... A... B... C... I... J... (or use G3

instead of G2). The axis words are all optional except that at least one of X and Y must be used. I

and J are the offsets from the current location (in the X and Y directions, respectively) of the

center of the circle. I and J are optional except that at least one of the two must be used. It is an

error if:

• X and Y are both omitted,

• I and J are both omitted.

When the XZ-plane is selected, program G2 X... Y... Z... A... B... C... I... K... (or use G3

instead of G2). The axis words are all optional except that at least one of X and Z must be used. I

and K are the offsets from the current location (in the X and Z directions, respectively) of the

center of the circle. I and K are optional except that at least one of the two must be used. It is an

error if:

• X and Z are both omitted,

• I and K are both omitted.

When the YZ-plane is selected, program G2 X... Y... Z... A... B... C... J... K... (or use G3

instead of G2). The axis words are all optional except that at least one of Y and Z must be used. J
 RS274/NGC Interpreter - Version 3

25

and K are the offsets from the current location (in the Y and Z directions, respectively) of the

center of the circle. J and K are optional except that at least one of the two must be used. It is an

error if:

• Y and Z are both omitted,

• J and K are both omitted.

Here is an example of a center format command to mill an arc: G17 G2 x 10 y 16 i 3 j 4 z 9.

That means to make a clockwise (as viewed from the positive z-axis) circular or helical arc whose

axis is parallel to the Z-axis, ending where X=10, Y=16, and Z=9, with its center offset in the X

direction by 3 units from the current X location and offset in the Y direction by 4 units from the

current Y location. If the current location has X=7, Y=7 at the outset, the center will be at X=10,

Y=11. If the starting value of Z is 9, this is a circular arc; otherwise it is a helical arc. The radius

of this arc would be 5.

In the center format, the radius of the arc is not specified, but it may be found easily as the

distance from the center of the circle to either the current point or the end point of the arc.

3.5.4 Dwell — G4

For a dwell, program G4 P... . This will keep the axes unmoving for the period of time in seconds

specified by the P number. It is an error if:

• the P number is negative.

3.5.5 Set Coordinate System Data — G10

The RS274/NGC language view of coordinate systems is described in Section 3.2.2.

To set the coordinate values for the origin of a coordinate system, program

G10 L2 P ... X... Y... Z... A... B... C..., where the P number must evaluate to an integer in the

range 1 to 9 (corresponding to G54 to G59.3) and all axis words are optional. The coordinates of

the origin of the coordinate system specified by the P number are reset to the coordinate values

given (in terms of the absolute coordinate system). Only those coordinates for which an axis word

is included on the line will be reset.

It is an error if:

• the P number does not evaluate to an integer in the range 1 to 9.

If origin offsets (made by G92 or G92.3) were in effect before G10 is used, they will continue to

be in effect afterwards.

The coordinate system whose origin is set by a G10 command may be active or inactive at the

time the G10 is executed.

Example: G10 L2 P1 x 3.5 y 17.2 sets the origin of the first coordinate system (the one selected

by G54) to a point where X is 3.5 and Y is 17.2 (in absolute coordinates). The Z coordinate of the

origin (and the coordinates for any rotational axes) are whatever those coordinates of the origin

were before the line was executed.

3.5.6 Plane Selection — G17, G18, and G19

Program G17 to select the XY-plane, G18 to select the XZ-plane, or G19 to select the YZ-plane.
 RS274/NGC Interpreter - Version 3

26

The effects of having a plane selected are discussed in Section 3.5.3 and Section 3.5.16.

3.5.7 Length Units — G20 and G21

Program G20 to use inches for length units. Program G21 to use millimeters.

It is usually a good idea to program either G20 or G21 near the beginning of a program before any

motion occurs, and not to use either one anywhere else in the program. It is the responsibility of

the user to be sure all numbers are appropriate for use with the current length units.

3.5.8 Return to Home — G28 and G30

Two home positions are defined (by parameters 5161-5166 for G28 and parameters 5181-5186 for

G30). The parameter values are in terms of the absolute coordinate system, but are in unspecified

length units.

To return to home position by way of the programmed position, program G28 X... Y... Z... A...

B... C... (or use G30). All axis words are optional. The path is made by a traverse move from the

current position to the programmed position, followed by a traverse move to the home position. If

no axis words are programmed, the intermediate point is the current point, so only one move is

made.

3.5.9 Straight Probe — G38.2

3.5.9.1 The Straight Probe Command

Program G38.2 X... Y... Z... A... B... C... to perform a straight probe operation. The rotational

axis words are allowed, but it is better to omit them. If rotational axis words are used, the numbers

must be the same as the current position numbers so that the rotational axes do not move. The

linear axis words are optional, except that at least one of them must be used. The tool in the

spindle must be a probe.

It is an error if:

• the current point is less than 0.254 millimeter or 0.01 inch from the programmed point.

• G38.2 is used in inverse time feed rate mode,

• any rotational axis is commanded to move,

• no X, Y, or Z-axis word is used.

In response to this command, the machine moves the controlled point (which should be at the end

of the probe tip) in a straight line at the current feed rate toward the programmed point. If the

probe trips, the probe is retracted slightly from the trip point at the end of command execution. If

the probe does not trip even after overshooting the programmed point slightly, an error is

signalled.

After successful probing, parameters 5061 to 5066 will be set to the coordinates of the location of

the controlled point at the time the probe tripped.

3.5.9.2 Using the Straight Probe Command

Using the straight probe command, if the probe shank is kept nominally parallel to the Z-axis (i.e.,

any rotational axes are at zero) and the tool length offset for the probe is used, so that the

controlled point is at the end of the tip of the probe:
 RS274/NGC Interpreter - Version 3

27

• without additional knowledge about the probe, the parallelism of a face of a part to the

XY-plane may, for example, be found.

• if the probe tip radius is known approximately, the parallelism of a face of a part to the

YZ or XZ-plane may, for example, be found.

• if the shank of the probe is known to be well-aligned with the Z-axis and the probe tip

radius is known approximately, the center of a circular hole, may, for example, be

found.

• if the shank of the probe is known to be well-aligned with the Z-axis and the probe tip

radius is known precisely, more uses may be made of the straight probe command,

such as finding the diameter of a circular hole.

If the straightness of the probe shank cannot be adjusted to high accuracy, it is desirable to know

the effective radii of the probe tip in at least the +X, -X, +Y, and -Y directions. These quantities

can be stored in parameters either by being included in the parameter file or by being set in an

RS274/NGC program.

Using the probe with rotational axes not set to zero is also feasible. Doing so is more complex

than when rotational axes are at zero, and we do not deal with it here.

3.5.9.3 Example Code

As a usable example, the code for finding the center and diameter of a circular hole is shown in

Table 6. For this code to yield accurate results, the probe shank must be well-aligned with the Zaxis, the cross section of the probe tip at its widest point must be very circular, and the probe tip

radius (i.e., the radius of the circular cross section) must be known precisely. If the probe tip

radius is known only approximately (but the other conditions hold), the location of the hole center

will still be accurate, but the hole diameter will not.

In Table 6, an entry of the form <description of number> is meant to be replaced by an actual

number that matches the description of number. After this section of code has executed, the Xvalue of the center will be in parameter 1041, the Y-value of the center in parameter 1022, and the

diameter in parameter 1034. In addition, the diameter parallel to the X-axis will be in parameter

1024, the diameter parallel to the Y-axis in parameter 1014, and the difference (an indicator of

circularity) in parameter 1035. The probe tip will be in the hole at the XY center of the hole.

The example does not include a tool change to put a probe in the spindle. Add the tool change

code at the beginning, if needed.
 RS274/NGC Interpreter - Version 3

28

3.5.10 Cutter Radius Compensation — G40, G41, and G42

To turn cutter radius compensation off, program G40. It is OK to turn compensation off when it is

already off.

Cutter radius compensation may be performed only if the XY-plane is active.

To turn cutter radius compensation on left (i.e., the cutter stays to the left of the programmed path

N010 (probe to find center and diameter of circular hole)

N020 (This program will not run as given here. You have to)

N030 (insert numbers in place of <description of number>.)

N040 (Delete lines N020, N030, and N040 when you do that.)

N050 G0 Z <Z-value of retracted position> F <feed rate>

N060 #1001=<nominal X-value of hole center>

N070 #1002=<nominal Y-value of hole center>

N080 #1003=<some Z-value inside the hole>

N090 #1004=<probe tip radius>

N100 #1005=[<nominal hole diameter>/2.0 - #1004]

N110 G0 X#1001 Y#1002 (move above nominal hole center)

N120 G0 Z#1003 (move into hole - to be cautious, substitute G1 for G0 here)

N130 G38.2 X[#1001 + #1005] (probe +X side of hole)

N140 #1011=#5061 (save results)

N150 G0 X#1001 Y#1002 (back to center of hole)

N160 G38.2 X[#1001 - #1005] (probe -X side of hole)

N170 #1021=[[#1011 + #5061] / 2.0] (find pretty good X-value of hole center)

N180 G0 X#1021 Y#1002 (back to center of hole)

N190 G38.2 Y[#1002 + #1005] (probe +Y side of hole)

N200 #1012=#5062 (save results)

N210 G0 X#1021 Y#1002 (back to center of hole)

N220 G38.2 Y[#1002 - #1005] (probe -Y side of hole)

N230 #1022=[[#1012 + #5062] / 2.0] (find very good Y-value of hole center)

N240 #1014=[#1012 - #5062 + [2 * #1004]] (find hole diameter in Y-direction)

N250 G0 X#1021 Y#1022 (back to center of hole)

N260 G38.2 X[#1021 + #1005] (probe +X side of hole)

N270 #1031=#5061 (save results)

N280 G0 X#1021 Y#1022 (back to center of hole)

N290 G38.2 X[#1021 - #1005] (probe -X side of hole)

N300 #1041=[[#1031 + #5061] / 2.0] (find very good X-value of hole center)

N310 #1024=[#1031 - #5061 + [2 * #1004]] (find hole diameter in X-direction)

N320 #1034=[[#1014 + #1024] / 2.0] (find average hole diameter)

N330 #1035=[#1024 - #1014] (find difference in hole diameters)

N340 G0 X#1041 Y#1022 (back to center of hole)

N350 M2 (that’s all, folks)

Table 6. Code to Probe Hole
 RS274/NGC Interpreter - Version 3

29

when the tool radius is positive), program G41 D... . To turn cutter radius compensation on right

(i.e., the cutter stays to the right of the programmed path when the tool radius is positive),

program G42 D... . The D word is optional; if there is no D word, the radius of the tool currently

in the spindle will be used. If used, the D number should normally be the slot number of the tool

in the spindle, although this is not required. It is OK for the D number to be zero; a radius value of

zero will be used.

It is an error if:

• the D number is not an integer, is negative or is larger than the number of carousel slots,

• the XY-plane is not active,

• cutter radius compensation is commanded to turn on when it is already on.

The behavior of the machining center when cutter radius compensation is on is described in

Appendix B.

3.5.11 Tool Length Offsets — G43 and G49

To use a tool length offset, program G43 H..., where the H number is the desired index in the tool

table. It is expected that all entries in this table will be positive. The H number should be, but does

not have to be, the same as the slot number of the tool currently in the spindle. It is OK for the H

number to be zero; an offset value of zero will be used.

It is an error if:

• the H number is not an integer, is negative, or is larger than the number of carousel

slots.

To use no tool length offset, program G49.

It is OK to program using the same offset already in use. It is also OK to program using no tool

length offset if none is currently being used.

3.5.12 Move in Absolute Coordinates — G53

For linear motion to a point expressed in absolute coordinates, program G1 G53 X... Y... Z...

A... B... C... (or use G0 instead of G1), where all the axis words are optional, except that at least

one must be used. The G0 or G1 is optional if it is the current motion mode. G53 is not modal and

must be programmed on each line on which it is intended to be active. This will produce

coordinated linear motion to the programmed point. If G1 is active, the speed of motion is the

current feed rate (or slower if the machine will not go that fast). If G0 is active, the speed of

motion is the current traverse rate (or slower if the machine will not go that fast).

It is an error if:

• G53 is used without G0 or G1 being active,

• G53 is used while cutter radius compensation is on.

See Section 3.2.2 for an overview of coordinate systems.

3.5.13 Select Coordinate System — G54 to G59.3

To select coordinate system 1, program G54, and similarly for other coordinate systems. The

system-number—G-code pairs are: (1—G54), (2—G55), (3—G56), (4—G57), (5—G58), (6—
 RS274/NGC Interpreter - Version 3

30

G59), (7—G59.1), (8—G59.2), and (9—G59.3).

It is an error if:

• one of these G-codes is used while cutter radius compensation is on.

See Section 3.2.2 for an overview of coordinate systems.

3.5.14 Set Path Control Mode — G61, G61.1, and G64

Program G61 to put the machining center into exact path mode, G61.1 for exact stop mode, or

G64 for continuous mode. It is OK to program for the mode that is already active. See Section

2.1.2.16 for a discussion of these modes.

3.5.15 Cancel Modal Motion — G80

Program G80 to ensure no axis motion will occur. It is an error if:

• Axis words are programmed when G80 is active, unless a modal group 0 G code is

programmed which uses axis words.

3.5.16 Canned Cycles — G81 to G89

The canned cycles G81 through G89 have been implemented as described in this section. Two

examples are given with the description of G81 below.

All canned cycles are performed with respect to the currently selected plane. Any of the three

planes (XY, YZ, ZX) may be selected. Throughout this section, most of the descriptions assume

the XY-plane has been selected. The behavior is always analogous if the YZ or XZ-plane is

selected.

Rotational axis words are allowed in canned cycles, but it is better to omit them. If rotational axis

words are used, the numbers must be the same as the current position numbers so that the

rotational axes do not move.

All canned cycles use X, Y, R, and Z numbers in the NC code. These numbers are used to

determine X, Y, R, and Z positions. The R (usually meaning retract) position is along the axis

perpendicular to the currently selected plane (Z-axis for XY-plane, X-axis for YZ-plane, Y-axis

for XZ-plane). Some canned cycles use additional arguments.

For canned cycles, we will call a number “sticky” if, when the same cycle is used on several lines

of code in a row, the number must be used the first time, but is optional on the rest of the lines.

Sticky numbers keep their value on the rest of the lines if they are not explicitly programmed to be

different. The R number is always sticky.

In incremental distance mode: when the XY-plane is selected, X, Y, and R numbers are treated as

increments to the current position and Z as an increment from the Z-axis position before the move

involving Z takes place; when the YZ or XZ-plane is selected, treatment of the axis words is

analogous. In absolute distance mode, the X, Y, R, and Z numbers are absolute positions in the

current coordinate system.

The L number is optional and represents the number of repeats. L=0 is not allowed. If the repeat

feature is used, it is normally used in incremental distance mode, so that the same sequence of

motions is repeated in several equally spaced places along a straight line. In absolute distance

mode, L > 1 means “do the same cycle in the same place several times,” Omitting the L word is
 RS274/NGC Interpreter - Version 3

31

equivalent to specifying L=1. The L number is not sticky.

When L>1 in incremental mode with the XY-plane selected, the X and Y positions are determined

by adding the given X and Y numbers either to the current X and Y positions (on the first goaround) or to the X and Y positions at the end of the previous go-around (on the repetitions). The

R and Z positions do not change during the repeats.

The height of the retract move at the end of each repeat (called “clear Z” in the descriptions

below) is determined by the setting of the retract mode: either to the original Z position (if that is

above the R position and the retract mode is G98, OLD_Z), or otherwise to the R position. See

Section 3.5.20

It is an error if:

• X, Y, and Z words are all missing during a canned cycle,

• a P number is required and a negative P number is used,

• an L number is used that does not evaluate to a positive integer,

• rotational axis motion is used during a canned cycle,

• inverse time feed rate is active during a canned cycle,

• cutter radius compensation is active during a canned cycle.

When the XY plane is active, the Z number is sticky, and it is an error if:

• the Z number is missing and the same canned cycle was not already active,

• the R number is less than the Z number.

When the XZ plane is active, the Y number is sticky, and it is an error if:

• the Y number is missing and the same canned cycle was not already active,

• the R number is less than the Y number.

When the YZ plane is active, the X number is sticky, and it is an error if:

• the X number is missing and the same canned cycle was not already active,

• the R number is less than the X number.

3.5.16.1 Preliminary and In-Between Motion

At the very beginning of the execution of any of the canned cycles, with the XY-plane selected, if

the current Z position is below the R position, the Z-axis is traversed to the R position. This

happens only once, regardless of the value of L.

In addition, at the beginning of the first cycle and each repeat, the following one or two moves are

made:

1. a straight traverse parallel to the XY-plane to the given XY-position,

2. a straight traverse of the Z-axis only to the R position, if it is not already at the R position.

If the XZ or YZ plane is active, the preliminary and in-between motions are analogous.
 RS274/NGC Interpreter - Version 3

32

3.5.16.2 G81 Cycle

The G81 cycle is intended for drilling. Program G81 X... Y... Z... A... B... C... R... L...

0. Preliminary motion, as described above.

1. Move the Z-axis only at the current feed rate to the Z position.

2. Retract the Z-axis at traverse rate to clear Z.

Example 1. Suppose the current position is (1, 2, 3) and the XY-plane has been selected, and the

following line of NC code is interpreted.

G90 G81 G98 X4 Y5 Z1.5 R2.8

This calls for absolute distance mode (G90) and OLD_Z retract mode (G98) and calls for the G81

drilling cycle to be performed once. The X number and X position are 4. The Y number and Y

position are 5. The Z number and Z position are 1.5. The R number and clear Z are 2.8. Old Z is 3.

The following moves take place.

1. a traverse parallel to the XY-plane to (4,5,3)

2. a traverse parallel to the Z-axis to (4,5,2.8)

3. a feed parallel to the Z-axis to (4,5,1.5)

4. a traverse parallel to the Z-axis to (4,5,3)

Example 2. Suppose the current position is (1, 2, 3) and the XY-plane has been selected, and the

following line of NC code is interpreted.

G91 G81 G98 X4 Y5 Z-0.6 R1.8 L3

This calls for incremental distance mode (G91) and OLD_Z retract mode (G98) and calls for the

G81 drilling cycle to be repeated three times. The X number is 4, the Y number is 5, the Z number

is -0.6 and the R number is 1.8. The initial X position is 5 (=1+4), the initial Y position is 7

(=2+5), the clear Z position is 4.8 (=1.8+3), and the Z position is 4.2 (=4.8-0.6). Old Z is 3.

The first move is a traverse along the Z-axis to (1,2,4.8), since old Z < clear Z.

The first repeat consists of 3 moves.

1. a traverse parallel to the XY-plane to (5,7,4.8)

2. a feed parallel to the Z-axis to (5,7, 4.2)

3. a traverse parallel to the Z-axis to (5,7,4.8)

The second repeat consists of 3 moves. The X position is reset to 9 (=5+4) and the Y position to

12 (=7+5).

1. a traverse parallel to the XY-plane to (9,12,4.8)

2. a feed parallel to the Z-axis to (9,12, 4.2)

3. a traverse parallel to the Z-axis to (9,12,4.8)

The third repeat consists of 3 moves. The X position is reset to 13 (=9+4) and the Y position to 17

(=12+5).

1. a traverse parallel to the XY-plane to (13,17,4.8)

2. a feed parallel to the Z-axis to (13,17, 4.2)

3. a traverse parallel to the Z-axis to (13,17,4.8)
 RS274/NGC Interpreter - Version 3

33

3.5.16.3 G82 Cycle

The G82 cycle is intended for drilling. Program G82 X... Y... Z... A... B... C... R... L... P...

0. Preliminary motion, as described above.

1. Move the Z-axis only at the current feed rate to the Z position.

2. Dwell for the P number of seconds.

3. Retract the Z-axis at traverse rate to clear Z.

3.5.16.4 G83 Cycle

The G83 cycle (often called peck drilling) is intended for deep drilling or milling with chip

breaking. The retracts in this cycle clear the hole of chips and cut off any long stringers (which are

common when drilling in aluminum). This cycle takes a Q number which represents a “delta”

increment along the Z-axis. Program G83 X... Y... Z... A... B... C... R... L... Q...

0. Preliminary motion, as described above.

1. Move the Z-axis only at the current feed rate downward by delta or to the Z position,

whichever is less deep.

2. Rapid back out to the clear_z.

3. Rapid back down to the current hole bottom, backed off a bit.

4. Repeat steps 1, 2, and 3 until the Z position is reached at step 1.

5. Retract the Z-axis at traverse rate to clear Z.

It is an error if:

• the Q number is negative or zero.

3.5.16.5 G84 Cycle

The G84 cycle is intended for right-hand tapping with a tap tool.

Program G84 X... Y... Z... A... B... C... R... L...

0. Preliminary motion, as described above.

1. Start speed-feed synchronization.

2. Move the Z-axis only at the current feed rate to the Z position.

3. Stop the spindle.

4. Start the spindle counterclockwise.

5. Retract the Z-axis at the current feed rate to clear Z.

6. If speed-feed synch was not on before the cycle started, stop it.

7. Stop the spindle.

8. Start the spindle clockwise.

The spindle must be turning clockwise before this cycle is used. It is an error if:

• the spindle is not turning clockwise before this cycle is executed.

With this cycle, the programmer must be sure to program the speed and feed in the correct

proportion to match the pitch of threads being made. The relationship is that the spindle speed

equals the feed rate times the pitch (in threads per length unit). For example, if the pitch is 2

threads per millimeter, the active length units are millimeters, and the feed rate has been set with

the command F150, then the speed should be set with the command S300, since 150 x 2 = 300.

If the feed and speed override switches are enabled and not set at 100%, the one set at the lower
 RS274/NGC Interpreter - Version 3

34

setting will take effect. The speed and feed rates will still be synchronized.

3.5.16.6 G85 Cycle

The G85 cycle is intended for boring or reaming, but could be used for drilling or milling.

Program G85 X... Y... Z... A... B... C... R... L...

0. Preliminary motion, as described above.

1. Move the Z-axis only at the current feed rate to the Z position.

2. Retract the Z-axis at the current feed rate to clear Z.

3.5.16.7 G86 Cycle

The G86 cycle is intended for boring. This cycle uses a P number for the number of seconds to

dwell. Program G86 X... Y... Z... A... B... C... R... L... P...

0. Preliminary motion, as described above.

1. Move the Z-axis only at the current feed rate to the Z position.

2. Dwell for the P number of seconds.

3. Stop the spindle turning.

4. Retract the Z-axis at traverse rate to clear Z.

5. Restart the spindle in the direction it was going.

The spindle must be turning before this cycle is used. It is an error if:

• the spindle is not turning before this cycle is executed.

3.5.16.8 G87 Cycle

The G87 cycle is intended for back boring.

Program G87 X... Y... Z... A... B... C... R... L... I... J... K...

The situation, as shown in Figure 1, is that you have a through hole and you want to counterbore

the bottom of hole. To do this you put an L-shaped tool in the spindle with a cutting surface on the

UPPER side of its base. You stick it carefully through the hole when it is not spinning and is

oriented so it fits through the hole, then you move it so the stem of the L is on the axis of the hole,

start the spindle, and feed the tool upward to make the counterbore. Then you stop the tool, get it

out of the hole, and restart it.

This cycle uses I and J numbers to indicate the position for inserting and removing the tool. I and

J will always be increments from the X position and the Y position, regardless of the distance

mode setting. This cycle also uses a K number to specify the position along the Z-axis of the

controlled point top of the counterbore. The K number is a Z-value in the current coordinate

system in absolute distance mode, and an increment (from the Z position) in incremental distance

mode.

0. Preliminary motion, as described above.

1. Move at traverse rate parallel to the XY-plane to the point indicated by I and J.

2. Stop the spindle in a specific orientation.

3. Move the Z-axis only at traverse rate downward to the Z position.

4. Move at traverse rate parallel to the XY-plane to the X,Y location.

5. Start the spindle in the direction it was going before.

6. Move the Z-axis only at the given feed rate upward to the position indicated by K.
 RS274/NGC Interpreter - Version 3

35

7. Move the Z-axis only at the given feed rate back down to the Z position.

8. Stop the spindle in the same orientation as before.

9. Move at traverse rate parallel to the XY-plane to the point indicated by I and J.

10. Move the Z-axis only at traverse rate to the clear Z.

11. Move at traverse rate parallel to the XY-plane to the specified X,Y location.

12. Restart the spindle in the direction it was going before.

When programming this cycle, the I and J numbers must be chosen so that when the tool is

stopped in an oriented position, it will fit through the hole. Because different cutters are made

differently, it may take some analysis and/or experimentation to determine appropriate values for

I and J.

3.5.16.9 G88 Cycle

The G88 cycle is intended for boring. This cycle uses a P word, where P specifies the number of

seconds to dwell. Program G88 X... Y... Z... A... B... C... R... L... P...

0. Preliminary motion, as described above.

1. Move the Z-axis only at the current feed rate to the Z position.

2. Dwell for the P number of seconds.

3. Stop the spindle turning.

Figure 1. G87 Cycle

The eight subfigures are labelled with the steps from the description above.

1,2 3 4 5

6 7,8 9 10

tool

hole

counterbore
 RS274/NGC Interpreter - Version 3

36

4. Stop the program so the operator can retract the spindle manually.

5. Restart the spindle in the direction it was going.

3.5.16.10 G89 Cycle

The G89 cycle is intended for boring. This cycle uses a P number, where P specifies the number of

seconds to dwell. program G89 X... Y... Z... A... B... C... R... L... P...

0. Preliminary motion, as described above.

1. Move the Z-axis only at the current feed rate to the Z position.

2. Dwell for the P number of seconds.

3. Retract the Z-axis at the current feed rate to clear Z.

3.5.17 Set Distance Mode — G90 and G91

Interpretation of RS274/NGC code can be in one of two distance modes: absolute or incremental.

To go into absolute distance mode, program G90. In absolute distance mode, axis numbers (X, Y,

Z, A, B, C) usually represent positions in terms of the currently active coordinate system. Any

exceptions to that rule are described explicitly in this Section 3.5.

To go into incremental distance mode, program G91. In incremental distance mode, axis numbers

(X, Y, Z, A, B, C) usually represent increments from the current values of the numbers.

I and J numbers always represent increments, regardless of the distance mode setting. K numbers

represent increments in all but one usage (see Section 3.5.16.8), where the meaning changes with

distance mode.

3.5.18 Coordinate System Offsets — G92, G92.1, G92.2, G92.3

See Section 3.2.2 for an overview of coordinate systems.

To make the current point have the coordinates you want (without motion), program G92 X...

Y... Z... A... B... C... , where the axis words contain the axis numbers you want. All axis words

are optional, except that at least one must be used. If an axis word is not used for a given axis, the

coordinate on that axis of the current point is not changed. It is an error if:

• all axis words are omitted.

When G92 is executed, the origin of the currently active coordinate system moves. To do this,

origin offsets are calculated so that the coordinates of the current point with respect to the moved

origin are as specified on the line containing the G92. In addition, parameters 5211 to 5216 are set

to the X, Y, Z, A, B, and C-axis offsets. The offset for an axis is the amount the origin must be

moved so that the coordinate of the controlled point on the axis has the specified value.

Here is an example. Suppose the current point is at X=4 in the currently specified coordinate

system and the current X-axis offset is zero, then G92 x7 sets the X-axis offset to -3, sets

parameter 5211 to -3, and causes the X-coordinate of the current point to be 7.

The axis offsets are always used when motion is specified in absolute distance mode using any of

the nine coordinate systems (those designated by G54 - G59.3). Thus all nine coordinate systems

are affected by G92.

Being in incremental distance mode has no effect on the action of G92.

Non-zero offsets may be already be in effect when the G92 is called. If this is the case, the new
 RS274/NGC Interpreter - Version 3

37

value of each offset is A+B, where A is what the offset would be if the old offset were zero, and B

is the old offset. For example, after the previous example, the X-value of the current point is 7. If

G92 x9 is then programmed, the new X-axis offset is -5, which is calculated by [[7-9] + -3].

To reset axis offsets to zero, program G92.1 or G92.2. G92.1 sets parameters 5211 to 5216 to

zero, whereas G92.2 leaves their current values alone.

To set the axis offset values to the values given in parameters 5211 to 5216, program G92.3.

You can set axis offsets in one program and use the same offsets in another program. Program

G92 in the first program. This will set parameters 5211 to 5216. Do not use G92.1 in the

remainder of the first program. The parameter values will be saved when the first program exits

and restored when the second one starts up. Use G92.3 near the beginning of the second program.

That will restore the offsets saved in the first program. If other programs are to run between the

the program that sets the offsets and the one that restores them, make a copy of the parameter file

written by the first program and use it as the parameter file for the second program.

3.5.19 Set Feed Rate Mode — G93 and G94

Two feed rate modes are recognized: units per minute and inverse time. Program G94 to start the

units per minute mode. Program G93 to start the inverse time mode.

In units per minute feed rate mode, an F word (no, not that F word; we mean feedrate) is

interpreted to mean the controlled point should move at a certain number of inches per minute,

millimeters per minute, or degrees per minute, depending upon what length units are being used

and which axis or axes are moving.

In inverse time feed rate mode, an F word means the move should be completed in [one divided

by the F number] minutes. For example, if the F number is 2.0, the move should be completed in

half a minute.

When the inverse time feed rate mode is active, an F word must appear on every line which has a

G1, G2, or G3 motion, and an F word on a line that does not have G1, G2, or G3 is ignored. Being

in inverse time feed rate mode does not affect G0 (rapid traverse) motions. It is an error if:

• inverse time feed rate mode is active and a line with G1, G2, or G3 (explicitly or

implicitly) does not have an F word.

3.5.20 Set Canned Cycle Return Level — G98 and G99

When the spindle retracts during canned cycles, there is a choice of how far it retracts: (1) retract

perpendicular to the selected plane to the position indicated by the R word, or (2) retract

perpendicular to the selected plane to the position that axis was in just before the canned cycle

started (unless that position is lower than the position indicated by the R word, in which case use

the R word position).

To use option (1), program G99. To use option (2), program G98. Remember that the R word has

different meanings in absolute distance mode and incremental distance mode.
 RS274/NGC Interpreter - Version 3

38

3.6 Input M Codes

M codes of the RS274/NGC language are shown in Table 7.

3.6.1 Program Stopping and Ending — M0, M1, M2, M30, M60

To stop a running program temporarily (regardless of the setting of the optional stop switch),

program M0.

To stop a running program temporarily (but only if the optional stop switch is on), program M1.

It is OK to program M0 and M1 in MDI mode, but the effect will probably not be noticeable,

because normal behavior in MDI mode is to stop after each line of input, anyway.

To exchange pallet shuttles and then stop a running program temporarily (regardless of the setting

of the optional stop switch), program M60.

If a program is stopped by an M0, M1, or M60, pressing the cycle start button will restart the

program at the following line.

To end a program, program M2. To exchange pallet shuttles and then end a program, program

M30. Both of these commands have the following effects.

1. Axis offsets are set to zero (like G92.2) and origin offsets are set to the default (like G54).

2. Selected plane is set to CANON_PLANE_XY (like G17).

3. Distance mode is set to MODE_ABSOLUTE (like G90).

4. Feed rate mode is set to UNITS_PER_MINUTE (like G94).

5. Feed and speed overrides are set to ON (like M48).

6. Cutter compensation is turned off (like G40).

7. The spindle is stopped (like M5).

8. The current motion mode is set to G_1 (like G1).

9. Coolant is turned off (like M9).

M Code Meaning

M0 program stop

M1 optional program stop

M2 program end

M3 turn spindle clockwise

M4 turn spindle counterclockwise

M5 stop spindle turning

M6 tool change

M7 mist coolant on

M8 flood coolant on

M9 mist and flood coolant off

M30 program end, pallet shuttle, and reset

M48 enable speed and feed overrides

M49 disable speed and feed overrides

M60 pallet shuttle and program stop

Table 7. M Codes
 RS274/NGC Interpreter - Version 3

39

No more lines of code in an RS274/NGC file will be executed after the M2 or M30 command is

executed. Pressing cycle start will start the program back at the beginning of the file.

3.6.2 Spindle Control — M3, M4, M5

To start the spindle turning clockwise at the currently programmed speed, program M3.

To start the spindle turning counterclockwise at the currently programmed speed, program M4.

To stop the spindle from turning, program M5.

It is OK to use M3 or M4 if the spindle speed is set to zero. If this is done (or if the speed override

switch is enabled and set to zero), the spindle will not start turning. If, later, the spindle speed is

set above zero (or the override switch is turned up), the spindle will start turning. It is OK to use

M3 or M4 when the spindle is already turning or to use M5 when the spindle is already stopped.

3.6.3 Tool Change — M6

To change a tool in the spindle from the tool currently in the spindle to the tool most recently

selected (using a T word — see Section 3.7.3), program M6. When the tool change is complete:

• The spindle will be stopped.

• The tool that was selected (by a T word on the same line or on any line after the

previous tool change) will be in the spindle. The T number is an integer giving the

changer slot of the tool (not its id).

• If the selected tool was not in the spindle before the tool change, the tool that was in the

spindle (if there was one) will be in its changer slot.

• The coordinate axes will be stopped in the same absolute position they were in before

the tool change (but the spindle may be re-oriented).

• No other changes will be made. For example, coolant will continue to flow during the

tool change unless it has been turned off by an M9.

The tool change may include axis motion while it is in progress. It is OK (but not useful) to

program a change to the tool already in the spindle. It is OK if there is no tool in the selected slot;

in that case, the spindle will be empty after the tool change. If slot zero was last selected, there

will definitely be no tool in the spindle after a tool change.

3.6.4 Coolant Control — M7, M8, M9

To turn mist coolant on, program M7.

To turn flood coolant on, program M8.

To turn all coolant off, program M9.

It is always OK to use any of these commands, regardless of what coolant is on or off.

3.6.5 Override Control — M48 and M49

To enable the speed and feed override switches, program M48. To disable both switches, program

M49. See Section 2.2.1 for more details. It is OK to enable or disable the switches when they are

already enabled or disabled.
 RS274/NGC Interpreter - Version 3

40

3.7 Other Input Codes

3.7.1 Set Feed Rate — F

To set the feed rate, program F... . The application of the feed rate is as described in Section

2.1.2.5, unless inverse time feed rate mode is in effect, in which case the feed rate is as described

in Section 3.5.19.

3.7.2 Set Spindle Speed — S

To set the speed in revolutions per minute (rpm) of the spindle, program S... . The spindle will

turn at that speed when it has been programmed to start turning. It is OK to program an S word

whether the spindle is turning or not. If the speed override switch is enabled and not set at 100%,

the speed will be different from what is programmed. It is OK to program S0; the spindle will not

turn if that is done. It is an error if:

• the S number is negative.

As described in Section 3.5.16.5, if a G84 (tapping) canned cycle is active and the feed and speed

override switches are enabled, the one set at the lower setting will take effect. The speed and feed

rates will still be synchronized. In this case, the speed may differ from what is programmed, even

if the speed override switch is set at 100%.

3.7.3 Select Tool — T

To select a tool, program T..., where the T number is the carousel slot for the tool. The tool is not

changed until an M6 is programmed (see Section 3.6.3). The T word may appear on the same line

as the M6 or on a previous line. It is OK, but not normally useful, if T words appear on two or

more lines with no tool change. The carousel may move a lot, but only the most recent T word

will take effect at the next tool change. It is OK to program T0; no tool will be selected. This is

useful if you want the spindle to be empty after a tool change. It is an error if:

• a negative T number is used,

• a T number larger than the number of slots in the carousel is used.

On some machines, the carousel will move when a T word is programmed, at the same time

machining is occurring. On such machines, programming the T word several lines before a tool

change will save time. A common programming practice for such machines is to put the T word

for the next tool to be used on the line after a tool change. This maximizes the time available for

the carousel to move.
 RS274/NGC Interpreter - Version 3

41

3.8 Order of Execution

The order of execution of items on a line is critical to safe and effective machine operation. Items

are executed in the order shown in Table 8 if they occur on the same line.

1. comment (includes message).

2. set feed rate mode (G93, G94 — inverse time or per minute).

3. set feed rate (F).

4. set spindle speed (S).

5. select tool (T).

6. change tool (M6).

7. spindle on or off (M3, M4, M5).

8. coolant on or off (M7, M8, M9).

9. enable or disable overrides (M48, M49).

10. dwell (G4).

11. set active plane (G17, G18, G19).

12. set length units (G20, G21).

13. cutter radius compensation on or off (G40, G41, G42)

14. cutter length compensation on or off (G43, G49)

15. coordinate system selection (G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3).

16. set path control mode (G61, G61.1, G64)

17. set distance mode (G90, G91).

18. set retract mode (G98, G99).

19. home (G28, G30) or

change coordinate system data (G10) or

set axis offsets (G92, G92.1, G92.2, G94).

20. perform motion (G0 to G3, G80 to G89), as modified (possibly) by G53.

21. stop (M0, M1, M2, M30, M60).

Table 8. Order of Execution
 RS274/NGC Interpreter - Version 3

42

4 Output: the Canonical Machining Functions

4.1 Introduction

This section describes the canonical machining functions. This section is intended to be useful to

developers, researchers, and NC programmers using the SAI. Others should not need to read it.

Earlier, but nearly identical, versions of these functions were described in a separate report,

“Canonical Machining Commands” [Proctor].

The context for canonical machining functions is in a hierarchical control system. These functions

are intended to tell a controller what to do at the control level below the level in which the

Interpreter is running.

4.1.1 Objectives of Canonical Machining Functions

The canonical machining functions were devised with three objectives in mind.

First, all the functionality of common 3-axis to 6-axis machining centers (not turning centers) had

to be covered by the functions; for any function a machining center can perform, there has to be a

way to tell it to do that function.

Second, it was desired that it be possible to use readily available commercial motion control

boards from various vendors to carry out those canonical functions which call for motion, with

roughly a one-to-one correspondence between a canonical motion function and a command a

commercial board recognizes.

Third, it must be possible to interpret RS274 commands into canonical machining function calls.

The first and third objectives still apply completely. The second objective, compatibility with

motion control boards, has become less important as computer speed and power has increased to

the point that motion control boards are not essential.

The canonical machining functions are atomic commands. Each function produces a single tool

motion or a single logical action. Keeping the functions atomic was a side condition we imposed,

both for clarity and to make mappings to commercial control boards straightforward. RS274

commands, on the other hand, include two types: those for which a single RS274 command

corresponds exactly to a canonical function call, and those for which a single RS274 command

will be decomposed into several canonical function calls (possibly dozens). Things like “move in

a straight line” or “turn flood coolant on” are of the first type. Things like “turn all coolant off” or

“run a peck drilling cycle” are of the second type.

4.1.2 Implementing Canonical Machining Functions

The name of each canonical machining function indicates roughly what it does. This report gives

the syntax of the functions and gives function prototypes in the C or C++ programming language.

The report also gives the semantics of the functions — what should happen when each function is

executed. To aid in expressing functions, a number of types are defined (CANON_PLANE, for

example). Each such type can have only a few symbolic values. CANON_PLANE must be one of

CANON_PLANE_XY, CANON_PLANE_YZ, or CANON_PLANE_XZ, for example. All of

these types are defined in Section 4.3.

This report does not provide definitions of the functions in any programming language. Sets of
 RS274/NGC Interpreter - Version 3

43

definitions for the canonical machining functions have been written in C++ for the controllers we

have built which use them. Executing a function from any of these sets of definitions causes a

machining center to do something.

We have used two other types of sets of definitions. The first alternate type simply has the

function call print itself. Executing a function call causes a line of text containing the function call

to be written to standard output or to a file. This type of set of definitions is used in the SAI. The

second alternate type is also used for testing and debugging. In this type, executing a canonical

function call generates a set of graphics calls for displaying a computer picture of the tool path

made by executing the function call. A system has been built using this set with the Interpreter

and the SAI driver to provide a graphical simulation of executing an RS274 program.

The Interpreter uses most but not all of the canonical machining functions. Those that are used are

listed in Table 9.
 RS274/NGC Interpreter - Version 3

44

Functionality Functions

Representation SET_ORIGIN_OFFSETS(double x, double y, double z, double a, double b, double c)

USE_LENGTH_UNITS(CANON_UNITS units)

Free Space

Motion

STRAIGHT_TRAVERSE(double x, double y, double z, double a, double b, double c)

Machining

Attributes

SELECT_PLANE(CANON_PLANE plane)

SET_FEED_RATE(double rate)

SET_FEED_REFERENCE(CANON_FEED_REFERENCE reference)

SET_MOTION_CONTROL_MODE(CANON_MOTION_MODE mode)

START_SPEED_FEED_SYNCH()

STOP_SPEED_FEED_SYNCH()

Machining

Functions

ARC_FEED(double first_end, double second_end, double first_axis, double

second_axis, int rotation, double axis_end_point, double a, double b, double c)

DWELL(double seconds)

STRAIGHT_FEED(double x, double y, double z, double a, double b, double c)

Probe

Functions

STRAIGHT_PROBE(double x, double y, double z, double a, double b, double c)

Spindle

Functions

ORIENT_SPINDLE(double orientation, CANON_DIRECTION direction)

SET_SPINDLE_SPEED(double r)

START_SPINDLE_CLOCKWISE()

START_SPINDLE_COUNTERCLOCKWISE()

STOP_SPINDLE_TURNING()

Tool

Functions

CHANGE_TOOL(int slot)

SELECT_TOOL(int i)

USE_TOOL_LENGTH_OFFSET(double offset)

Miscellaneous

Functions

COMMENT(char * s)

DISABLE_FEED_OVERRIDE()

DISABLE_SPEED_OVERRIDE()

ENABLE_FEED_OVERRIDE()

ENABLE_SPEED_OVERRIDE()

FLOOD_OFF()

FLOOD_ON()

INIT_CANON()

MESSAGE(char * s)

MIST_OFF()

MIST_ON()

PALLET_SHUTTLE()

Program

Functions

OPTIONAL_PROGRAM_STOP()

PROGRAM_END()

PROGRAM_STOP()

Table 9. Canonical Machining Functions Called By Interpreter

Function arguments are written in ANSI C style. All functions return nothing
 RS274/NGC Interpreter - Version 3

45

4.2 Canonical Machining Function View of a Machining Center

The canonical machining functions are based on a particular view of what a machining center to

be controlled is like. The view is as described in Section 2.1, with the changes described below.

Some differences between the canonical machining function view and the RS274/NGC language

view are given here.

4.2.1 Mechanical Components

4.2.1.1 Coolant

In addition to mist coolant and flood coolant, a machining center may have through-tool coolant.

In the RS274/NGC language view, there is no through-tool coolant.

4.2.1.2 Axis Clamps

Each axis may have a physical device which, when activated, clamps the axis so it does not move.

In the RS274/NGC language view, there are no axis clamps.

4.2.2 Control Components

The following control components are included in the canonical machining function view of a

how a machining center may be controlled, but are not included in the RS274/NGC view. These

control components cannot be used by a direct command from an RS274/NGC program, since

they are not included in the language. Only coordination of axis and spindle motion is used

indirectly by the Interpreter. That is used for implementing the G84 tapping canned cycle.

4.2.2.1 Coolant

Each type of coolant can be turned off independently. In the RS274/NGC view, although the

different types of coolant may be turned on independently, all coolant is turned off by a single

command.

4.2.2.2 Axis Clamps

Each axis may be commanded to clamp so it does not move, and commanded to unclamp. If the

axis has a physical clamp, that clamp should be used. A software clamp may be used. Clamping

any one axis or set of axes does not affect motion along the unclamped axes.

4.2.2.3 Elliptical Arc Motion

Any pair of the linear axes (XY, YZ, XZ) can be controlled to move in an elliptical arc in the plane

of that pair of axes. While this is occurring, the third linear axis and the rotational axes can be

controlled to move simultaneously at effectively a constant rate. As above, the motions can be

coordinated so that acceleration and deceleration do not affect the path.

4.2.2.4 Coordinated Motion of Axes and Spindle

The rotation of the spindle can be coordinated with axis motion or de-coupled from it. In the

RS274/NGC view, this is not programmable, but coordination occurs during tapping; see Section

3.5.16.5.

4.2.2.5 Feed Reference

The current feed rate may be referenced either to XYZ axis motion or to motion of the controlled

point with respect to the workpiece. Only the XYZ feed reference is used in the Interpreter. In the
 RS274/NGC Interpreter - Version 3

46

RS274/NGC view, the XYZ feed reference is always used, so there is no command to change the

feed reference.

4.2.2.6 Feed and Speed Overrides

These two switches may be enabled or disabled independently; in the RS274/NGC view, one

single command enables both, and another single command disables both.

4.2.2.7 Units

Units used for distances along the X, Y, and Z axes may be measured centimeters, in addition to

millimeters or inches. The RS274/NGC view does not include using centimeters. Centimeters are

not used in the Interpreter.

4.2.2.8 Coordinate Systems

There are two coordinate systems: the absolute coordinate system of a machining center and a

“program” coordinate system in which all axes may be offset from their absolute position. The

offsets may be changed. All axis values given in all function calls (other than a function call

setting the offsets) are expressed in terms of the program coordinate system.

4.2.3 Error Conditions

The controller which executes the canonical machining function calls should have at least two

conditions: OK and error. If the controller is in the OK condition, it should perform as described

here. If the controller is in the error condition, its behavior is up to the implementation. An

implementation should document what its behavior is for all errors. A generic error behavior

which we believe is reasonable is to stop execution of the current function call as soon as an error

is detected and to be unwilling to execute any other canonical function calls until the error

condition is corrected.

Many situations should put the controller into the error condition, as described later in this report.

Wherever the phrase “it is an error” (or the equivalent) is used to describe a situation that may

occur in the execution of a function call, the controller should always check for that situation

during execution of the function call and should go into the error condition as soon as the situation

is detected if the situation occurs.

In this report, error detection is described as being performed only by the controller receiving the

canonical machining function calls. In an implementation, error detection might also be

performed by the controller sending the function calls.

4.3 The Canonical Machining Functions Defined

4.3.1 Preliminaries

4.3.1.1 Syntax

The canonical machining functions are defined here using C++ syntax in courier type font.

The same syntax is usable in ANSI C. Syntaxes for other computer languages may be derived

readily without changing the semantics of the functions. All the canonical functions return void,

so that bit of syntax is suppressed here.

Where an attribute may take on discrete values from a fixed set of values, the set is given here.

The values in such sets are represented here as symbols beginning with “CANON_”. In our
 RS274/NGC Interpreter - Version 3

47

implementations we have used both #define’s and enum’s for these symbols.

As given here, the functions include the A, B, and C rotational axes. If any of the rotational axis is

not to be used, just omit the argument for that axis.

4.3.1.2 Function Call Errors

It is an error to call any function incorrectly. The arguments to a function must be as described

here. This applies to the number and type of the arguments and also to the stated constraints on the

arguments (such as being non-negative or being positive).

4.3.1.3 Groups of Functions

The canonical machining functions are grouped here into related sets. The grouping is for

convenience only, and is not part of the definition. Within each group, the functions are listed

alphabetically.

4.3.1.4 Rotational Motion Required

In the descriptions of the functions, the phrase “if there is rotational motion” is often used. In all

cases, there is rotational motion if any of the rotational axis values in the function call differs from

the current value of that axis.

4.3.2 Initialization and Termination

4.3.2.1 Init_canon

INIT_CANON ()

Do whatever initialization is required to be ready to execute other canonical machining functions.

A call to this function should always be made before calling any other canonical machining

function. Of course, the controller must already have been brought up to the state where it can

read and execute this function call before the function call is received. That phase of initialization

is outside the scope of this report.

4.3.2.2 End_canon

END_CANON ()

Do whatever is required to shut down in an orderly fashion. After a call to this function has been

executed, if it is desired to begin executing function calls again, the first function call must be an

INIT_CANON function call.

4.3.3 Representation

4.3.3.1 Select_plane

SELECT_PLANE (CANON_PLANE plane)

Use the plane designated by plane as the selected plane. The type CANON_PLANE may have

the value CANON_PLANE_XY, CANON_PLANE_YZ, or CANON_PLANE_XZ. Any of these

is an acceptable values for plane.
 RS274/NGC Interpreter - Version 3

48

4.3.3.2 Set_origin_offsets

SET_ORIGIN_OFFSETS (double x, double y, double z,

double a, double b, double c)

Set the program origin at the point with absolute coordinates x, y, z, a, b, and c. The units for x,

y, and z are whatever length units are being used at the time a call to this function is made. The

units for a, b, and c are degrees. The effective location of the program origin should not change

when units change. It is expected that controllers dealing with the program origin will ensure this.

In a typical implementation, the numbers representing the coordinates will be changed when units

change.

4.3.3.3 Use_length_units

USE_LENGTH_UNITS (CANON_UNITS units)

Use the specified units for length. The type CANON_UNITS is defined which may have the

value CANON_UNITS_INCHES, CANON_UNITS_MM (millimeters), or

CANON_UNITS_CM (centimeters). Any of these is an acceptable values of units. Changing

units changes the effective numerical value of the current position. All other stored values which

involve length units are not changed, including: coordinate system offsets, tool length offsets, tool

diameters, feed rate, and traverse rate.

The Interpreter does not use CANON_UNITS_CM because there is no code for it in the RS274/

NGC language.

4.3.4 Free Space Motion

4.3.4.1 Set_traverse_rate

SET_TRAVERSE_RATE (double rate)

Set the upper limit on the rate that will be used during rapid axis motion, motion during which

cutting does not normally take place. During moves conducted at traverse rate, coordinated linear

motion should take place as fast as possible or at this rate, whichever is less. The rate must be

positive. The application of the rate is as described in Section 2.1.2.5.

4.3.4.2 Straight_traverse

STRAIGHT_TRAVERSE (double x, double y, double z,

double a, double b, double c)

Make a coordinated linear motion at traverse rate from the current position to the point given by

x, y, z, a, b, and c. The application of the rate is as described in Section 4.3.5.1 for when the feed

reference mode is CANON_XYZ, regardless of the setting of feed reference mode.

It is expected that no cutting will occur while a traverse move is being made.

4.3.5 Machining Attributes

4.3.5.1 Set_feed_rate

SET_FEED_RATE (double rate)

Set to rate the feed rate that will be used when the controlled point is told to move at the

currently set feed rate. The rate must be non-negative.
 RS274/NGC Interpreter - Version 3

49

1. If the feed reference mode is CANON_WORKPIECE:

the rate means length units per minute of the controlled point along the programmed

path as seen by the workpiece.

2. If the feed reference mode is CANON_XYZ the interpretation of feed rate is as described

in Section 2.1.2.5.

The canonical machining functions (unlike the RS274/NGC language) do not include the notion

of inverse time feed rate, so the question of behavior under inverse time feed rate does not arise.

The feed rate may also be affected by the feed override switch, if that switch is enabled.

If the USE_SPINDLE_FORCE or USE_SPINDLE_TORQUE mode is in effect, the set feed rate

is an upper limit for the feed rate determined from the force or torque. While either of these

modes is in effect, if the feed override switch is enabled and is set to change the feed rate, the feed

rate determined from the force or torque and the upper limit are both changed proportionally. For

example, if the feed rate is set to 600 millimeters per minute and the feed override switch is

enabled and set to 80%, and the torque on the spindle is such that the machine would feed at 500

millimeters per minute if the override switch were disabled, then the actual feed rate should be

400 millimeters per minute (80% of 500), and the upper limit should be 480 millimeters per

minute (80% of 600).

4.3.5.2 Set_feed_reference

SET_FEED_REFERENCE (CANON_FEED_REFERENCE reference)

This sets the feed reference mode. The type CANON_FEED_REFERENCE is defined. It may

have the value CANON_WORKPIECE (feed rate is from the point of view of the workpiece) or

CANON_XYZ (feedrate is in terms of axis motion). Either is an acceptable value of

reference.

The meaning of feed rate changes depending on the feed reference mode. See the discussion

immediately above.

The CANON_WORKPIECE feed reference mode is more natural and general, since the rate at

which the tool passes through the material must be controlled for safe and effective machining.

This mode does introduce complications, however.

First, some rule is required to define what the path should be. We have adopted the rule that the

path should be the same as it is in the CANON_XYZ mode.

Second, computing the feed rate for each axis may be time-consuming because the trajectories

that result from motion in four or more axes may be complex. Computation of axis feed rates

when only XYZ motion is considered is relatively simple for two of the standard motion types

(straight lines and helical or circular arcs).

Third, in CANON_WORKPIECE mode, some motions cannot be carried out as fast as the

programmed feed rate would require because axis motions may tend to cancel each other. For

example, an arc in the XZ-plane can exactly cancel a rotation around the B-axis, so that the

location of the controlled point with respect to the workpiece does not change at all during the

motion; in this case, the motion should take no time, which is impossible at any finite rate of axis

motion. In such cases, the axes should be moved as fast as possible consistent with accurate

machining.
 RS274/NGC Interpreter - Version 3

50

Some (perhaps most or all) existing dialects of RS274 use only the CANON_XYZ mode [K&T,

page 3.9]. The specification of RS274/NGC is not clear [NCMS, page 22], but appears to intend

CANON_XYZ mode. Some dialects avoid the problem of dealing with how to interpret a perminute feed rate when rotational axis motion occurs simultaneously with XYZ motion by

suggesting [K&T, page 3.9] or requiring [Monarch, page 17-3] that the programmer use inversetime feed rate mode. It may be that the calculations required in CANON_WORKPIECE mode

were too extensive to be carried out sufficiently fast by real-time processors that existed at the

time these languages were defined. Current real-time processors should be sufficiently fast to

handle the calculations.

4.3.5.3 Set_motion_control_mode

SET_MOTION_CONTROL_MODE (CANON_MOTION_MODE mode)

Set the path control mode. The type CANON_MOTION_MODE is defined. It may have the value

CANON_EXACT_STOP, CANON_EXACT_PATH, or CANON_CONTINUOUS. Any of these

is an acceptable value of mode.

In CANON_EXACT_STOP mode, the control stops motion at the end of each move exactly

(within the tolerance the control system can achieve) at the programmed or calculated end point.

The stop is preceded by deceleration at the maximum normal rate, so that motion is kept at the set

feed rate for as long as possible. If there is a subsequent move, the stop is as brief as possible and

is followed by acceleration to the programmed feed rate at the maximum normal rate of

acceleration.

In CANON_EXACT_PATH mode, the control keeps the controlled point on the programmed or

calculated path within the tolerance the control system can achieve at all times. At points which

are the end point of one move and the start point of the next move, the feed rate is kept constant if

possible. It should be possible to avoid changing the rate of motion at such a juncture if the

direction of the path of the controlled point does not change sharply at the juncture, for example if

one straight move is in the same direction as the previous one, or if a straight move is tangent to a

preceding or following arc move.

In CANON_CONTINUOUS mode, the control tries to keep the feed rate constant and does not

try to keep the controlled point exactly on the path at all times. Rather, at junctures between

moves where the direction changes sharply, the corner is rounded. There is a maximum allowable

deviation at such junctures, and the control should never allow that to be exceeded; acceleration

and deceleration may be performed if necessary to do this.

Currently, there is no function to set the maximum deviation allowable in

CANON_CONTINUOUS mode.

4.3.5.4 Start_speed_feed_synch

START_SPEED_FEED_SYNCH ()

Begin exact synchronization of spindle turning with feed motion.

The primary purpose of this synchronization is to provide for effective tapping of holes. In order

to make a clean thread, the axial motion of a tap must be synchronized with its turning motion. In

addition to this synchronization, the feed and speed rates must be set so their ratio is suitable for
 RS274/NGC Interpreter - Version 3

51

the pitch of the thread.

The type CANON_SPEED_FEED_MODE is defined. It may have the value

CANON_SYNCHED (for coupled) or CANON_INDEPENDENT (for uncoupled). The type is

used by the Interpreter to keep track of the current state of synchronization.

4.3.5.5 Stop_speed_feed_synch

STOP_SPEED_FEED_SYNCH ()

Stop forcing synchronization of spindle turning with feed motion. Deal with acceleration and

deceleration of the spindle and the axes independently.

4.3.6 Machining Functions

4.3.6.1 Arc_feed

ARC_FEED (double first_end, double second_end,

double first_axis, double second_axis, int rotation,

double axis_end_point, double a, double b, double c)

Move in a helical arc from the current position at the existing feed rate. The axis of the helix is

parallel to the X, Y, or Z-axis, according to which one is perpendicular to the selected plane. The

helical arc may degenerate to a circular arc if there is no motion parallel to the axis of the helix.

If the selected plane is the XY-plane:

1. first_end is the X coordinate of the end of the arc.

2. second_end is the Y coordinate of the end of the arc.

3. first_axis is the X coordinate of the axis (center) of the arc.

4. second_axis is the Y coordinate of the axis (center) of the arc.

5. axis_end_point is the Z coordinate of the end of the arc.

If the selected plane is the YZ-plane:

1. first_end is the Y coordinate of the end of the arc.

2. second_end is the Z coordinate of the end of the arc.

3. first_axis is the Y coordinate of the axis (center) of the arc.

4. second_axis is the Z coordinate of the axis (center) of the arc.

5. axis_end_point is the X coordinate of the end of the arc.

If the selected plane is the XZ-plane:

1. first_end is the Z coordinate of the end of the arc.

2. second_end is the X coordinate of the end of the arc.

3. first_axis is the Z coordinate of the axis (center) of the arc.

4. second_axis is the X coordinate of the axis (center) of the arc.

5. axis_end_point is the Y coordinate of the end of the arc.

If rotation is positive, the arc is traversed counterclockwise as viewed from the positive end of

the coordinate axis perpendicular to the currently selected plane. If rotation is negative, the

arc is traversed clockwise. If rotation is 0, first_end and second_end must be the same as

the corresponding coordinates of the current position and no arc is made (but there may be

translation parallel to the axis perpendicular to the selected plane and rotational axis motion). If
 RS274/NGC Interpreter - Version 3

52

rotation is 1, more than 0 but not more than 360 degrees of arc should be made. In general, if

rotation is n, n is not 0, and we let N be the absolute value of n, the absolute value of the

amount of rotation in the arc should be more than ([N-1] x 360) but not more than (N x 360).

The radius of the helix is determined by the distance from the current position to the axis of helix

or by the distance from the end location to the axis of the helix. It is an error if the two radii are

not the same (within some tolerance, to be set by the implementation).

The feed rate applies to the distance traveled along the helix. This differs from many existing

systems, which apply the feed rate to the distance traveled by a point on a circle which is the

projection of the helix on a plane perpendicular to the axis of the helix.

Rotational axis motion along with helical XYZ motion has no known applications, but is not

illegal. Rotational axis motion is handled as follows, if there is rotational motion.

1. If the feed reference mode is CANON_XYZ: Perform XYZ motion as if no rotational

motion were specified. While the XYZ motion is going on, move the rotational axes in

coordinated linear motion.

2. If the feed reference mode is CANON_WORKPIECE: the path to follow is the path that

would be followed if the feed reference mode were CANON_XYZ, but the rate along

that path should be kept constant at the programmed feed rate. This will usually cause

variable rates along all moving axes.

4.3.6.2 Dwell

DWELL (double seconds)

Do not move the axes for the time specified by the seconds argument, which must be positive.

4.3.6.3 Ellipse_feed

ELLIPSE_FEED (double major, double minor,

double angle_to_first, double first_end,

double second_end,

double first_axis, double second_axis, int rotation,

double axis_end_point, double a, double b, double c)

Move in an elliptical helical arc from the current position at the existing feed rate. The axis of the

helix is parallel to the X, Y, or Z-axis, according to which one is perpendicular to the selected

plane. The elliptical helical arc may degenerate to an elliptical arc if there is no motion parallel to

the axis of the helix.

The length of the major axis (not the semi-major axis) of the ellipse is given by major, and the

length of the minor axis by minor.

If the selected plane is the XY-plane:

1. angle_to_first is the angle between the major axis of the ellipse and the +X-axis.

2. first_end is the X coordinate of the end of the arc.

3. second_end is the Y coordinate of the end of the arc.

4. first_axis is the X coordinate of the axis (center) of the arc.

5. second_axis is the Y coordinate of the axis (center) of the arc.

6. axis_end_point is the Z coordinate of the end of the arc.
 RS274/NGC Interpreter - Version 3

53

If the selected plane is the YZ-plane:

1. angle_to_first is the angle between the major axis of the ellipse and the +Y-axis.

2. first_end is the Y coordinate of the end of the arc.

3. second_end is the Z coordinate of the end of the arc.

4. first_axis is the Y coordinate of the axis (center) of the arc.

5. second_axis is the Z coordinate of the axis (center) of the arc.

6. axis_end_point is the X coordinate of the end of the arc.

If the selected plane is the XZ-plane:

1. angle_to_first is the angle between the major axis of the ellipse and the +Z-axis.

2. first_end is the Z coordinate of the end of the arc.

3. second_end is the X coordinate of the end of the arc.

4. first_axis is the Z coordinate of the axis (center) of the arc.

5. second_axis is the X coordinate of the axis (center) of the arc.

6. axis_end_point is the Y coordinate of the end of the arc.

If rotation is positive, the arc is traversed counterclockwise as viewed from the positive end of

the coordinate axis perpendicular to the currently selected plane. If rotation is negative, the

arc is traversed clockwise. If rotation is 0, first_end and second_end must be the same as

the corresponding coordinates of the current position and no arc is made (but there may be

translation parallel to the axis perpendicular to the selected plane and rotational axis motion). If

rotation is 1, more than 0 but not more than 360 degrees of arc should be made. In general, if

rotation is n, n is not 0, and we let N be the absolute value of n, the absolute value of the

amount of rotation in the arc should be more than ([N-1] x 360) but not more than (N x 360).

Rotational axis motion along with elliptical helix XYZ motion has no known applications, but is

not illegal. Rotational axis motion is handled as follows, if there is rotational motion.

1. If the feed reference mode is CANON_XYZ: Perform XYZ motion as if no rotational

motion were specified. While the XYZ motion is going on, move the rotational axes in

coordinated linear motion.

2. If the feed reference mode is CANON_WORKPIECE: the path to follow is the path that

would be followed if the feed reference mode were CANON_XYZ, but the rate along

that path should be kept constant at the programmed feed rate. This will usually cause

variable rates along all moving axes.

The ellipse_feed function is much like the arc_feed function, except that the tool path is an

elliptical helix rather than a circular helix. With an elliptical helix, there are at least two choices

for how to coordinate motion parallel to the axis of the helix with motion around the axis. In both

cases, we focus on a point P traveling along the elliptical helix. The “projected ellipse” of the

helix is the projection of the helix on any plane perpendicular to the axis of the helix (which is, by

definition, an ellipse). We define P’ to be the projection of P on the projected ellipse and P” to be

the projection of P on the axis.

1. The slope along the helix is constant. In other words, there is some constant k, such that for

any distance d traveled by P’ around the projected ellipse, the distance traveled along the

axis by P” is kd.

2. The amount of travel along the axis by P” is proportional to the angle swept by a line from

the center of the projected ellipse to P’. This rule produces a variable slope which is
 RS274/NGC Interpreter - Version 3

54

steeper on the pointy ends of the ellipse.

We have implemented the second of these — because that is what the motion control board we

were using would do. It might be useful to add a setting for the machining center or another

argument to the function so that either of the two trajectory types could be selected.

The feed rate applies to the distance travelled along the helix by P. This differs from the one

existing system we have used, which applies the feed rate to the distance traveled by a point on a

circle which is a projection of the projected ellipse.

It is an error if the projections of the current point and the end point of the arc do not lie on the

projected ellipse (within some tolerance, to be set by the implementation).

The functionality of the arc_feed function is the same as what the ellipse_feed function will do if

the major and minor axes of the ellipse are equal. In that case, the value of the angle of the X-axis

with the major axis of the ellipse is irrelevant, and the two trajectory rules give the same

trajectory. It is useful to have both functions, however, because many applications may wish to

implement only arc_feed, and because the arc_feed function is simpler.

4.3.6.4 Stop

STOP ()

Stop axis motion. Regardless of the current path control mode, come briefly to a stop at the end

point of the last programmed move before going on to the next move.

4.3.6.5 Straight_feed

STRAIGHT_FEED (double x, double y, double z,

double a, double b, double c)

If there is no rotational motion, move the controlled point in a straight line at feed rate from the

current position to the point given by the x, y, and z arguments. Do not move the rotational axes.

If there is rotational motion:

1. If the feed reference mode is CANON_XYZ, perform XYZ motion as if there were no

rotational motion. While the XYZ motion is going on, move the rotational axes in

coordinated linear motion.

2. If the feed reference mode is CANON_WORKPIECE, the path to follow is the path that

would be followed if the feed reference mode were CANON_XYZ, but the rate along

that path should be kept constant.

4.3.6.6 Straight_probe

STRAIGHT_PROBE (double x, double y, double z,

double a, double b, double c)

This performs a probing operation. A probe must be in the spindle. The probe may be a touch

probe or a non-contact probe. There must be no rotational motion. The probe must not be already

tripped when execution of a call to this function starts. The spindle must not be turning. The probe

must be turned on. It is an error if any of those “musts” does not hold.

Points to be probed are usually not exactly where expected, so a small overshoot distance is
 RS274/NGC Interpreter - Version 3

55

included in probe motion. An overshoot point is defined by extending the line from the current

point to the programmed point by the overshoot distance.

To execute a call to this function, start by moving the probe in a straight line at the currently

programmed feed rate from the current position toward the overshoot point. The next steps

depend on what type of probe is being used.

For a touch probe, it is expected that the probe will be tripped before the overshoot point is

reached. It is an error for the probe to reach that position without being tripped. If the probe is

tripped before the overshoot point is reached, the control should stop moving the axes as quickly

as possible, move the axes back to where they were when the probe tripped, and stop at that point.

For a non-contact probe, it is expected that the probe will reach the programmed position. It is an

error if not. The probe should either decelerate and stop at that point (gathering data all the way),

or continue at full feed rate through the point (gathering data all the way), stop gathering data and

stop moving as fast as feasible, then move back to the programmed position and stop.

An implementation may put limits on the acceptable range of feed rates for probing, as strict as

requiring a specific value. It is an error to execute a straight_probe function call if the feed rate is

not within the allowed range.

Functions for the Interpreter to call to get data after probing are given in Appendix D.6.

4.3.7 Spindle Functions

4.3.7.1 Orient_spindle

ORIENT_SPINDLE (double orientation, CANON_DIRECTION direction)

Turn the spindle (if it is not already correctly oriented) in the direction specified by direction

to the angle specified by the orientation in degrees. Stop the spindle at that angle. Do not

make a full turn or more. The type CANON_DIRECTION is defined. It may have the value

CANON_STOPPED, CANON_CLOCKWISE, or CANON_COUNTERCLOCKWISE. Of these,

only CANON_CLOCKWISE, or CANON_COUNTERCLOCKWISE is an acceptable value of

direction. Orientation must be between 0 and 359.999.

The rate at which the spindle turns while orienting is up to the implementation.

The zero point of spindle rotation is along the positive X-axis.

The CANON_DIRECTION type is also used in the Interpreter to represent the state of the

spindle. For that use, CANON_STOPPED is needed in addition to CANON_CLOCKWISE and

CANON_COUNTERCLOCKWISE.

4.3.7.2 Set_spindle_speed

SET_SPINDLE_SPEED (double speed)

Set to speed the spindle speed that will be used when the spindle is turning. Speed is given in

revolutions per minute (rpm) and refers to the rate of spindle rotation. Speed must be positive. If

the spindle is already turning and is at a different speed, change to the speed given with this

function. This function does not start the spindle if it is not turning.

An implementation should set an upper limit on spindle speed. It is an error if speed is larger
 RS274/NGC Interpreter - Version 3

56

than that limit.

4.3.7.3 Spindle_retract

SPINDLE_RETRACT ()

Retract the spindle at the current feed rate to the fully retracted position.

4.3.7.4 Spindle_retract_traverse

SPINDLE_RETRACT_TRAVERSE ()

Retract the spindle at traverse rate to the fully retracted position.

4.3.7.5 Start_spindle_clockwise

START_SPINDLE_CLOCKWISE ()

Turn the spindle clockwise at the currently set speed rate. If the spindle is already turning that

way, this function has no effect. If the spindle speed is set outside the allowable range, it is an

error to execute this function.

4.3.7.6 Start_spindle_counterclockwise

START_SPINDLE_COUNTERCLOCKWISE ()

Turn the spindle counterclockwise at the currently set speed rate. If the spindle is already turning

that way, this function has no effect. If the spindle speed is set outside the allowable range, it is an

error to execute this function.

4.3.7.7 Stop_spindle_turning

STOP_SPINDLE_TURNING ()

Stop the spindle from turning. If the spindle is already stopped, this function has no effect.

4.3.7.8 Use_no_spindle_force

USE_NO_SPINDLE_FORCE ()

Do not consider spindle force. Instead, use the feed rate to determine spindle motion. A call to this

function does not reinstate use_spindle_torque (if, for example, using spindle torque was stopped

earlier by a call to use_spindle_force).

4.3.7.9 Use_no_spindle_torque

USE_NO_SPINDLE_TORQUE ()

Do not consider spindle torque. Instead, use the feed rate to determine spindle motion. A call to

this function does not reinstate use_spindle_force (if, for example, using spindle force was

stopped earlier by a call to use_spindle_torque).
 RS274/NGC Interpreter - Version 3

57

4.3.7.10 Use_spindle_force

USE_SPINDLE_FORCE (double force)

If the force on the spindle exceeds force (in newtons), reduce the feed rate until the force on the

spindle drops below that amount. Use the programmed feed rate as an upper limit on the feed rate.

This is intended for adaptive machining. It requires that the machining center have a mechanism

to measure the force. It is an error to execute this function if the machining center does not have

such a mechanism.

A call to use_spindle_force cancels the use of spindle torque to affect feed rate (if it is in effect

before the call).

4.3.7.11 Use_spindle_torque

USE_SPINDLE_TORQUE (double torque)

If the torque on the spindle exceeds torque (in newton-meters), reduce the feed rate until the

torque on the spindle drops below that amount. Use the programmed feed rate as an upper limit on

the feed rate.

This is intended for adaptive machining. It requires that the machining center have a mechanism

to measure the torque. It is an error to execute this function if the machining center does not have

such a mechanism.

A call to use_spindle_torque cancels the use of spindle force to affect feed rate (if it is in effect

before the call).

4.3.8 Tool Functions

CHANGE_TOOL (int slot)

The slots of a tool changer are taken to be numbered consecutively from 1 to however many slots

there are in the changer. The value of slot may be zero. It is an error if slot is not zero or the

number of an actual changer slot.

This function results in the tool currently in the spindle (if any) being returned to its slot, and the

tool from the slot designated by slot (if any) being inserted in the spindle. If slot is zero, no

tool should be inserted in the spindle.

If there is no tool in the slot designated by slot, there will be no tool in the spindle after this

function is executed and no error condition will result in the controller. Similarly, if there is no

tool in the spindle when this function is executed, no tool will be returned to the carousel and no

error condition will result in the controller, whether or not a tool was previously selected in the

program. On the machining centers we have used, these actions do not harm the machine. If the

machine design is such that these actions will harm the machine, we suggest that the superior

controller check for potential harm before calling the CHANGE_TOOL function.

It is expected that when the machining center controller is initialized, the designated slot for a tool

already in the spindle will be established. This may be done in any manner deemed fit, including

(for, example) recording that information in a persistent, crash-proof location so it is always

available from the last time the machining center was run, or having the operator enter it. It is
 RS274/NGC Interpreter - Version 3

58

expected that the machining center controller will remember that information as long as it is not

re-initialized; in particular, it will be remembered between programs.

For the purposes of this function, the tool includes the tool holder.

For machining centers which can carry out a SELECT_TOOL function call separately from a

CHANGE_TOOL function call, the SELECT_TOOL function call must have been executed

before the CHANGE_TOOL function call, and the value of slot in the CHANGE_TOOL

function call must be the slot number of the selected tool.

If the spindle is turning before a tool change, the spindle should be stopped by the

CHANGE_TOOL function call and should not be restarted.

During a tool change, the machining center may move the axes, but when the tool change is

complete, the axes should all be back to where they were before the tool change began. If the new

tool is a different length than the old one, the tool tip will be in a different location.

If the spindle was oriented before a CHANGE_TOOL function call, changing the tool may

disorient it.

A tool change has no effect on coolant use. Coolant must be turned on and off by a coolant

function.

4.3.8.1 Select_tool

SELECT_TOOL (int slot)

Select the tool in the given slot. It is an error if slot is not zero or the number of an actual

changer slot. If it is possible and efficient to do so, move the tool carousel so that the selected slot

is in position for access by the tool changer.

If the changer mechanism can handle only one tool at a time, moving the carousel when a call to

this function is executed is not usually an efficient thing to do, since the tool in the spindle must

usually be removed and put into its slot first when the CHANGE_TOOL function call is executed.

If the changer mechanism can handle two tools simultaneously, moving the carousel is usually an

efficient thing to do.

4.3.8.2 Use_tool_length_offset

USE_TOOL_LENGTH_OFFSET (double length)

Set the tool length offset to the given length (in current length units). The length must be

non-negative. The effective value of a tool length offset changes if length units are changed, as

discussed in Section 4.3.3.3.

4.3.9 Miscellaneous Functions

4.3.9.1 Clamp_axis

CLAMP_AXIS (CANON_AXIS axis)

Clamp the given axis. The type CANON_AXIS is defined. It may have the value

CANON_AXIS_X, CANON_AXIS_Y, CANON_AXIS_Z, CANON_AXIS_A,

CANON_AXIS_B, or CANON_AXIS_C. Any of these is an acceptable value of axis, provided
 RS274/NGC Interpreter - Version 3

59

the machining center has such an axis.

It is an error to execute a function call which would move an axis while the axis is clamped.

4.3.9.2 Comment

COMMENT (char * text)

This function has no physical effect. If function calls are being printed or logged, the comment

function call is printed or logged, including the string which is the value of text.

4.3.9.3 Disable_feed_override

DISABLE_FEED_OVERRIDE ()

Do not pay attention to the setting of the feed override switch. Make the feed rate have its

programmed value immediately.

4.3.9.4 Disable_speed_override

DISABLE_SPEED_OVERRIDE ()

Do not pay attention to the setting of the speed override switch. Make the spindle speed have its

programmed value immediately.

4.3.9.5 Enable_feed_override

ENABLE_FEED_OVERRIDE ()

Pay attention to the setting of the feed override switch. Modify feeds in accordance with the

switch settings.

4.3.9.6 Enable_speed_override

ENABLE_SPEED_OVERRIDE ()

Pay attention to the setting of the speed override switch. Modify spindle speeds in accordance

with the switch settings.

4.3.9.7 Flood_off

FLOOD_OFF ()

Turn flood coolant off. It is an error to execute a call to this function if the machining center does

not have flood coolant.

4.3.9.8 Flood_on

FLOOD_ON ()

Turn flood coolant on. It is an error to execute a call to this function if the machining center does

not have flood coolant.
 RS274/NGC Interpreter - Version 3

60

4.3.9.9 Message

MESSAGE (char * text)

Display the text on the message display device.

4.3.9.10 Mist_off

MIST_OFF ()

Turn mist coolant off. It is an error to execute a call to this function if the machining center does

not have mist coolant.

4.3.9.11 Mist_on

MIST_ON ()

Turn mist coolant on. It is an error to execute a call to this function if the machining center does

not have mist coolant.

4.3.9.12 Pallet_shuttle

PALLET_SHUTTLE ()

If the machining center has a pallet shuttle mechanism (a mechanism which switches the position

of two pallets), a call to this function should cause that switch to be made. If either or both of the

pallets are missing, this will not result in an error condition in the controller.

4.3.9.13 Through_tool_off

THROUGH_TOOL_OFF ()

Turn through-tool coolant off. It is an error to execute a call to this function if the machining

center does not have through-tool coolant.

4.3.9.14 Through_tool_on

THROUGH_TOOL_ON ()

Turn through-tool coolant on. It is an error to execute a call to this function if the machining

center does not have through-tool coolant.

4.3.9.15 Turn_probe_off

TURN_PROBE_OFF ()

Turn the probe off. It is an error to execute a call to this function if the tool in the spindle is not a

probe. It is not an error to call this function when the probe is already off.

4.3.9.16 Turn_probe_on

TURN_PROBE_ON ()

Turn the probe on. It is an error to execute a call to this function if the tool in the spindle is not a

probe. It is not an error to call this function when the probe is already on.
 RS274/NGC Interpreter - Version 3

61

4.3.9.17 Unclamp_axis

UNCLAMP_AXIS (CANON_AXIS axis)

Unclamp the given axis.

4.3.10 Program Functions

OPTIONAL_PROGRAM_STOP();

If the optional stop switch is on when a call to this function is read from a program, stop executing

the program at this point, but be prepared to resume with the next line of the program.

PROGRAM_END();

If a program is being read, stop executing the program and be prepared to accept a new program

or to be shut down.

PROGRAM_STOP();

Stop executing the program at this point, but be prepared to resume with the next line of the

program.

4.3.11 Cutter Radius Compensation

Canonical machining functions for cutter radius compensation are defined as follows. These

functions are not used in the Interpreter, which performs the cutter radius compensation itself,

rather than passing the work on to lower levels of control, so NC programmers and machine

operators should ignore this section. The type CANON_COMP_SIDE is defined which may have

the value CANON_COMP_RIGHT, CANON_COMP_LEFT, or CANON_COMP_OFF.

4.3.11.1 Set_cutter_radius_compensation

SET_CUTTER_RADIUS_COMPENSATION (double radius)

Set to radius the radius to use when performing cutter radius compensation. The radius must

be positive. The effective cutter radius changes if length units are changed.

4.3.11.2 Start_cutter_radius_compensation

START_CUTTER_RADIUS_COMPENSATION (CANON_COMP_SIDE side)

This starts cutter radius compensation. Acceptable values of side are CANON_COMP_LEFT

and CANON_COMP_RIGHT, where left means the cutter stays to the left of the programmed

path (when viewed from the positive end of the axis perpendicular to the currently selected plane)

as the cutter moves forward and right means the cutter stays to the right of the programmed path.

4.3.11.3 Stop_cutter_radius_compensation

STOP_CUTTER_RADIUS_COMPENSATION ()

Do not apply cutter radius compensation when executing spindle translation function calls.
 RS274/NGC Interpreter - Version 3

62

5 Stand-Alone Interpreter

This section describes the Stand-Alone Interpreter (SAI). The section is intended to be useful to

SAI installers, NC programmers, developers, and researchers. Machine operators might find it

useful.

The SAI is valuable because it allows a user to pre-test an NC program without having to run it on

the machine controller itself. Any computer for which the SAI can be compiled can be used to

pre-test NC programs.

The SAI includes the Interpreter, a driver, and a version of the canonical machining functions.

Pre-tests of NC programs on the SAI are strong tests because the Interpreter runs exactly the same

way in the SAI as it does integrated with the EMC control system.

The SAI has two input modes: keyboard (MDI) mode and file (batch) mode. In the MDI mode,

the user types lines of RS274/NGC code at the keyboard. In the batch mode, the Interpreter reads

lines of code from a file.

The set of canonical machining functions which prints text has been linked into the SAI, so the

output is always text. The output is printed either to the computer terminal or to a file. In general,

an output file is useful only if input is taken from a file and errors do not occur during

interpretation.

5.1 Running the SAI

5.1.1 Starting the SAI

The SAI is started by giving a command in a terminal window. After the SAI starts, the user is

presented with a number of options. The user must press the “return” key after each choice; the

return key presses are not printed here. Many different versions of the SAI executable may be

compiled from the same source code. This section uses the name “rs274” for the executable. The

name of your SAI executable may be different; if so, use your name, instead of “rs274.”

The Interpreter requires parameter data (which it reads from a file) and tool data (which it obtains

by calling world-give-information functions — see Appendix D.6). In the SAI, the driver reads a

tool file so it can provide the tool data the Interpreter asks for by function call. There is a default

parameter file, “rs274ngc.var,” and a default tool file, “rs274ngc.tool_default”. The default data

does not represent the actual state of any machining center or set of tools.

In the SAI, the parameter data and tool data files may be designated by the user. The data in the

files may be actual or hypothetical. When the SAI starts up, the user is offered the opportunity to

provide the name of a parameter file and the name of a tool file. In both cases, if a name is

provided, the named file is used. If a name is not provided, the default is used. The default files are

shown in Table 1 and Table 2. If a file is missing or in bad format, the SAI prints a message to that

effect and quits.

Either way the SAI is used, when it starts, the following menu is printed:
 RS274/NGC Interpreter - Version 3

63

enter a number:

1 = start interpreting

2 = choose parameter file ...

3 = read tool file ...

4 = turn block delete switch ON

5 = adjust error handling ...

enter choice =>

When the user selects 1, the menu disappears, and interpretation begins. The user may select any

of 2 through 5 zero, one, or many times; only the last setting of those items is used.

If the user selects 2 or 3, the user is prompted for the name of a file and offered the same menu

again.

If the user selects 4, the user is offered the same menu again, with “turn block delete switch ON”

changed to “turn block delete switch OFF”; the two toggle back and forth when 4 is selected.

If the user selects 5, another menu is offered, as follows, and then the above menu is offered again.

enter a number:

1 = done with error handling

2 = print stack on error

enter choice =>

When the user selects 1, the previous menu comes up again.

If the user selects 2, the user is offered the same menu again, with “print stack on error” changed

to “do not print stack on error”; the two toggle back and forth when 2 is selected. The meaning of

item 2 is that the user has a choice of whether, if there is an error, the system will print the stack of

function calls that was active when the error occurred. The default setting is not to print the stack.

With file input, there is a number 3 choice on the second menu, as described a few paragraphs

hence.

5.1.2 Running with Keyboard Input

The SAI is invoked with keyboard (MDI) input by giving the command:

rs274

The user is presented with the menus shown above. When the user finishes with the menus, the

following two-step cycle repeats until the user exits.

1. The SAI prints the prompt READ =>

2. The user enters a line of RS274/NGC code at the keyboard, hits the carriage return button, and

the line is interpreted.

When using keyboard input, the SAI exits only if it reads a line with the one word “quit”. Most

variations of “quit” are valid, e.g., “Q uI t”.

The user interface provides no capability to edit ahead, undo, or anything else involving more than

the current line.

A transcript of a short session with the SAI using keyboard input is shown in Table 10.
 RS274/NGC Interpreter - Version 3

64

rs274

enter a number:

1 = start interpreting

2 = choose parameter file ...

3 = read tool file ...

4 = turn block delete switch ON

5 = adjust error handling...

enter choice => 3

name of tool file => rs274ngc.tool_default

enter a number:

1 = start interpreting

2 = choose parameter file ...

3 = read tool file ...

4 = turn block delete switch ON

5 = adjust error handling...

enter choice => 1

executing

 1 N..... USE_LENGTH_UNITS(CANON_UNITS_MM)

 2 N..... SET_ORIGIN_OFFSETS(0.0000, 0.0000, 0.0000)

 3 N..... SET_FEED_REFERENCE(CANON_XYZ)

READ => g1 x3 y1 f20.0

 4 N..... SET_FEED_RATE(20.0000)

 5 N..... STRAIGHT_FEED(3.0000, 1.0000, 0.0000)

READ => g2 x[6-[4*3/2]] r 7.01 z0.5

 6 N..... ARC_FEED(0.0000, 1.0000, 1.5000, 7.8476, -1, 0.5000)

READ => (that was a helical arc)

 7 N..... COMMENT("that was a helical arc")

READ => t2

 8 N..... SELECT_TOOL(2)

READ => m6 g43 h2

 9 N..... CHANGE_TOOL(2)

 10 N..... USE_TOOL_LENGTH_OFFSET(1.0000)

READ => m2

 11 N..... SET_ORIGIN_OFFSETS(0.0000, 0.0000, 0.0000)

 12 N..... STOP_SPINDLE_TURNING()

 13 N..... PROGRAM_END()

READ => g1 x asim[0.5]

Unknown word starting with a

g1 x asim[0.5]

READ => g1 x asin[0.5]

 14 N..... STRAIGHT_FEED(30.0000, 1.0000, -0.5000)

READ => g91 g81 x3 y2 z-0.8 r1.5 l2

 15 N..... COMMENT("interpreter: distance mode changed to incremental")

 16 N..... STRAIGHT_TRAVERSE(30.0000, 1.0000, 1.0000)

 17 N..... SET_MOTION_CONTROL_MODE(CANON_EXACT_PATH)

 18 N..... STRAIGHT_TRAVERSE(33.0000, 3.0000, 1.0000)

 19 N..... STRAIGHT_FEED(33.0000, 3.0000, 0.2000)

 20 N..... STRAIGHT_TRAVERSE(33.0000, 3.0000, 1.0000)

 21 N..... STRAIGHT_TRAVERSE(36.0000, 5.0000, 1.0000)

 22 N..... STRAIGHT_FEED(36.0000, 5.0000, 0.2000)

 23 N..... STRAIGHT_TRAVERSE(36.0000, 5.0000, 1.0000)

 24 N..... SET_MOTION_CONTROL_MODE(CANON_CONTINUOUS)

READ => quit

Table 10. Transcript of an SAI Session Using Keyboard Input
 RS274/NGC Interpreter - Version 3

65

5.1.3 Running with RS274/NGC File Input

There are two ways to use the SAI with file input: with terminal output or with file output. In both

cases the output is printed canonical machining function calls. Also in both cases, a third option

for error handling is given.

If file output is used, the third option is to choose between “continue on error” and “stop on error”.

The menu item for the option toggles between the two. The default is stop.

If file output is not being used, the third option is to choose among “continue on error”, “stop on

error”, and “MDI on error”. The menu item for the option cycles among the three. The default is

stop. If the SAI gets into the MDI mode this way, the user must enter “quit” to get out of MDI,

and after quitting MDI, must decide whether or not to continue interpreting. If the user decides to

continue, interpretation starts at the line of the file following the line where the error occurred that

put the SAI into MDI mode.

For terminal output, give a command of the form:

rs274 input_filename

where input_filename is the name of an RS274/NGC input file. With this invocation, normal

printed output from the SAI (everything but error messages) appears on stdout, which is normally

the terminal on which the command was invoked. Printed output may be redirected from the

terminal to an output file, but it is usually simpler to call the SAI as shown below to get output in

a file.

For file output, give a command of the form:

rs274 input_filename output_filename

where output_filename is the name the output file should have. This file will be created if it does

not exist; if it does exist, it will be overwritten.

If there are errors during interpretation and “continue on error” has been selected, any input line

which causes an error will not be interpreted, and the output file may be incorrect on any line after

the last line which was output before the first error occurred.

When running with file input, the SAI exits if any of the following happens:

1. the SAI executes a line with an M2 or M30 command on it. In this case, the rest of the line is

executed before the SAI exits. If there are more lines in the file following the line with the M2 or

M30, they are ignored.

2. the “stop on error” option is in effect, and an error occurs.

3. the “MDI on error” option is in effect, the user has quit MDI, and the user decides to not to

continue, when prompted to decide.

4. the file ended at the previous line, that line did not include M2 or M30, and the “MDI on error”

option is not in effect.

5.2 Building an SAI Executable

On a SUN SPARCstation 20, an executable file for the SAI may be built from source code in

about half a minute, as described below. The same procedure should work on any computer
 RS274/NGC Interpreter - Version 3

66

running a Unix operating system and having the standard C++ libraries. On computers running

other operating systems, compilation should be similarly easy, provided the standard C++

libraries are available.

To make an executable, seven source code files must be placed in the same directory along with

the Makefile shown in Table 11. The source code files are:

canon.hh

canon_pre.cc

driver.cc

rs274ngc.hh

rs274ngc_errors.cc

rs274ngc_pre.cc

rs274ngc_return.hh

The first two files are the header file and function definitions for the canonical machining

functions and the world-give-information functions described in Appendix D.6, which the

Interpreter calls to get information about the world outside itself.

The version of canon.cc which prints function calls is used with the SAI. This file also contains a

minimal model of the world outside the Interpreter. The canonical machining functions defined in

this file update the model when they are called, as well as printing themselves. The world-giveinformation functions take information from the outside world model and give it to the Interpreter.

The third file, driver.cc, contains the SAI driver. The driver handles interaction between the user

and the Interpreter. It also helps maintain the model of the world outside the Interpreter.

The fourth file, rs274ngc.hh is the header file for the Interpreter.

The rs274ngc_errors.cc file defines an array containing all the Interpreter error messages. It works

with the last file, rs274ngc_return.hh, which has symbolic values for the indexes of the array.

These two files were prepared automatically from the source file rs274ngc.cc.

The sixth file, rs274ngc_pre.cc, contains the function definitions for the Interpreter. It is a prepreprocessed version of rs274ngc.cc, also prepared automatically from rs274ngc.cc. The source

file rs274ngc.cc is not needed to compile the SAI but is available on request.

An executable SAI for 3-axis machining named “rs274” is built in the same directory by giving

the command:

make rs274.

In the Makefile, we are using the Gnu C++ compiler, “g++.” Any other C++ compiler may be

substituted for g++.

There are three types of compiler options: (1) axis existence options -DAA, -DBB, and -DCC, (2)

-DALL_AXES, and (3) -DAXIS_ERROR.

The axis existence options are for compiling for machining centers with different sets of rotational

axes. Eight combinations of rotational axes are possible: none, all, any one of three, and missing

one of three. Only two of the eight are shown in the Makefile below. The rules for rs274ac.o and

rs274ac may be copied and easily modified for the other six combinations of axes. -DAA means

include an A-axis. -DBB means include a B-axis. -DCC means include a C-axis.
 RS274/NGC Interpreter - Version 3

67

The -DALL_AXES option is used if you want the Interpreter to include all three rotational axes in

the canonical machining function calls it makes, even though the Interpreter is compiled with two

or fewer rotational axes. When this option is used, the value zero is used in the canonical

machining function calls for the otherwise missing axes.

The -DAXIS_ERROR option is used if you want the Interpreter to signal an error if an input

RS274/NGC program uses a rotational axis the Interpreter was not compiled with. If this option is

not used, the Interpreter will read and ignore axis values for rotational axes with which it was not

compiled.

The Makefile gives an example of each option. The options may be combined to make a total of

29 different executables (1 with all three rotational axes, 4 with each of the 7 combinations of

fewer than three rotational axes).

COMPILE = g++ -c -v -g

LINK = g++ -v

canon.o: canon_pre.cc canon.hh

 $(COMPILE) -o canon.o canon_pre.cc

canon_abc.o: canon_pre.cc canon.hh

 $(COMPILE) -DAA -DBB -DCC -o canon_abc.o canon_pre.cc

canon_ac.o: canon_pre.cc canon.hh

 $(COMPILE) -DAA -DCC -o canon_ac.o canon_pre.cc

driver.o: driver.cc canon.hh rs274ngc.hh rs274ngc_return.hh

 $(COMPILE) -o driver.o driver.cc

rs274: rs274.o canon.o driver.o

 $(LINK) -o rs274 rs274.o canon.o driver.o -lm

rs274.o: rs274ngc_pre.cc canon.hh rs274ngc.hh rs274ngc_errors.cc rs274ngc_return.hh

 $(COMPILE) -o rs274.o rs274ngc_pre.cc

rs274ac: rs274ac.o canon_ac.o driver.o

 $(LINK) -o rs274ac rs274ac.o canon_ac.o driver.o -lm

rs274ac.o: rs274ngc_pre.cc canon.hh rs274ngc.hh rs274ngc_errors.cc rs274ngc_return.hh

 $(COMPILE) -DAA -DCC -o rs274ac.o rs274ngc_pre.cc

rs274_all.o: rs274ngc_pre.cc canon.hh rs274ngc.hh rs274ngc_errors.cc rs274ngc_return.hh

 $(COMPILE) -DALL_AXES -o rs274_all.o rs274ngc_pre.cc

rs274_all: rs274_all.o canon_abc.o driver.o

 $(LINK) -o rs274_all rs274_all.o canon_abc.o driver.o -lm

rs274_no.o: rs274ngc_pre.cc canon.hh rs274ngc.hh rs274ngc_errors.cc rs274ngc_return.hh

 $(COMPILE) -DAXIS_ERROR -o rs274_no.o rs274ngc_pre.cc

rs274_no: rs274_no.o canon.o driver.o

 $(LINK) -o rs274_no rs274_no.o canon.o driver.o -lm

Table 11. Makefile for Interpreter
 RS274/NGC Interpreter - Version 3

68

5.3 Interpreter Speed

Using a 2004-line input test file for machining 2000 straight cuts, running on a Sun SPARCstation

20 using the Solaris operating system, the SAI wrote an output file in 1.6 seconds elapsed time, as

measured by the “time” utility. A 3605-line file for machining 3600 arcs took 2.5 seconds. These

tests show a rate of over 1000 lines per second for the SAI on a Sun SPARCstation 20 computer.

Running on a PC using the Red Hat Linux operating system with a 200 megahertz processor, the

(recompiled) SAI handled the same two test files somewhat faster — 0.8 seconds and 1.7 seconds.

The output from the two computers was byte-by-byte identical for the two input programs. A Gnu

C++ compiler was used for both the Sun and the PC.

Tests with other types of programs show similar results. Thus, it is clear that using the SAI system

for pre-testing NC programs takes little time.

When the Interpreter is being used integrated with the EMC control system, there are relatively

few situations in which a modern PC would be challenged, since the tool path prescribed by a line

found in a typical program will rarely take less than a tenth of a second to cut, while interpreting

that line will rarely take more than a hundredth of a second. Thus, for most NC programs, the

Interpreter speed will not be a significant factor.

There is one known class of program for which Interpreter speed may be a significant factor. This

class is those programs which include many consecutive short lines or arcs (say 0.1 millimeter

long each). This type of program is produced by many NC program post-processors for following

complex contours approximately. At 1000 millimeters per minute feed rate (a realistic value), a

2000-line file should run in 12 seconds. The test results above show that the Interpreter runs about

ten times that fast on computers with moderate (in year 2000) speed, so the Interpreter should not

be a bottleneck in dealing with that class of programs.
 RS274/NGC Interpreter - Version 3

69

References

[Albus] Albus, James S; et al; NIST Support to the Next Generation Controller

Program: 1991 Final Technical Report; NISTIR 4888; National Institute of

Standards and Technology, Gaithersburg, MD; July 1992

[Allen-Bradley] Allen-Bradley; RS274/NGC for the Low End Controller; First Draft;

Allen-Bradley; August 1992

[EIA] Electronic Industries Association; EIA Standard EIA-274-D Interchangeable

Variable Block Data Format for Positioning, Contouring, and Contouring/

Positioning Numerically Controlled Machines; Electronic Industries

Association; Washington, DC; February 1979

[Fanuc] Fanuc Ltd.; Fanuc System 9-Model A Operators Manual; Pub B-52364E/03;

Fanuc Ltd; 1981

[Kramer1] Kramer, Thomas R.; Proctor, Frederick M.; Michaloski, John L.; The NIST

RS274/NGC Interpreter, Version 1; NISTIR 5416; National Institute of

Standards and Technology, Gaithersburg, MD; April 1994

[Kramer2] Kramer, Thomas R.; Proctor, Frederick M.; The NIST RS274KT Interpreter;

NISTIR 5738; National Institute of Standards and Technology, Gaithersburg,

MD; October 1995

[Kramer3] Kramer, Thomas R.; Proctor, Frederick M.; The NIST RS274/NGC Interpreter

- Version 2; NISTIR 5739; National Institute of Standards and Technology,

Gaithersburg, MD; October 1995

[Kramer4] Kramer, Thomas R.; Proctor, Frederick M.; The NIST RS274/VGER

Interpreter; NISTIR 5754; National Institute of Standards and Technology,

Gaithersburg, MD; November 1995

[K&T] Kearney and Trecker Co.; Part Programming and Operating Manual, KT/CNC

Control, Type C; Pub 687D; Kearney and Trecker Corp.; 1980

[Martin] Martin Marietta; Controls Standardized Application (CSA); Draft Volume V of

Next Generation Workstation/Machine Controller (NGC) Specification for an

Open System Architecture Standard (SOSAS); Martin Marietta Document No.

NGC-0001-14-000-CSA; March 1992

[Monarch] Monarch Cortland; Programming Manual for Monarch VMC-75 with General

Electric 2000MC Controls; Monarch Cortland Publication Number PRG

GE2000MC-4

[NCMS] National Center for Manufacturing Sciences; The Next Generation Controller

Part Programming Functional Specification (RS-274/NGC); Draft; NCMS;

August 1994

[Proctor] Proctor, Frederick M.; Kramer, Thomas R.; Michaloski, John L.; Canonical

Machining Commands; NISTIR 5970; National Institute of Standards and

Technology, Gaithersburg, MD; January 1997
 RS274/NGC Interpreter - Version 3

70

Appendix A. Error Handling

This appendix describes error handling in the Interpreter and the SAI. Software for error handling

is described here rather than in Appendix D. This appendix is intended to be useful to developers

and researchers. NC programmers, machine operators, and SAI installers are not likely to find it

useful. A complete list of error messages the Interpreter can generate (not including SAI driver

error messages) is in the file rs274ngc_errors.cc, for those who are interested.

The Interpreter detects and flags most kinds of illegal input. Unreadable input, missing words,

extra words, out-of-bounds numbers, and illegal combinations of words, for example, are all

detected. The Interpreter does not check for axis overtravel or excessively high feeds or speeds,

however. The Interpreter also does not detect situations where a legal command does something

unfortunate, such as machining a fixture.

A.1 Basic Approach

The basic approach to error handling is:

1. Check carefully for errors.

2. If an error occurs, identify it specifically so that the user can be informed.

3. If an error occurs, return through the function call hierarchy rather than jumping out of it.

The Interpreter always saves the text of the last line to be interpreted. If there is an error, the

Interpreter also saves the names of the functions in the function call stack. The driver, which has

been given the error code, may then ask the Interpreter for (1) the text of the error, (2) the text of

the line, and/or (3) some or all of the names of the functions in the stack. In the SAI, if an error

occurs, the driver always asks for and prints the error text and line text. If the user has asked for it

(see Section 5.1.1), the SAI also prints the names on the function call stack.

Control flow for error handling, synchronization of the Interpreter with the driver, and exiting are

handled together by having each function that tells the Interpreter to do something return a status

value meaning one of six things:

1. None of the other situations in this list has occurred. The symbolic value for this is

RS274NGC_OK.

2. The Interpreter just executed a line that makes it necessary for the Interpreter to ask for

information. No error has occurred, and it is not time to exit. If there is a queue of things

that canonical machining function calls said to do, empty the queue (by executing

everything in it), so that the state of the world will be up-to-date when the Interpreter asks

for information. The driver should not ask the Interpreter to read again until the queue is

empty. The symbolic value for this is RS274NGC_EXECUTE_FINISH. The main

instance of this situation is in probing. After interpreting a line with a probe command, the

Interpreter is going to ask for the results of probing the next time the driver tells it to read,

but needs to be sure the probing has been carried out before asking for results.

3. The Interpreter just read a line starting with the block_delete character and there were no

errors in reading the line. The symbolic value for this is also

RS274NGC_EXECUTE_FINISH. This use of that value is easily distinguished from its

use in item 2 (immediately above) because this use occurs during reading while the

previous use occurs during execution.

4. Interpretation of a file has begun, and the Interpreter has read a line with nothing on it but a
 RS274/NGC Interpreter - Version 3

71

percent sign, “%”, possibly surrounded by white space. If the first non-blank line of the

file was the same sort of line, this means interpretation of the file should stop, and the

value RS274NGC_ENDFILE is returned. If the first line was not such a line, an error has

occurred.

5. The Interpreter has executed M2 or M30, meaning end of program. This means

interpretation of the file should stop. The symbolic value is RS274NGC_EXIT.

6. An error has occurred. The symbolic value is a specific error code identifying the error.

If an error occurs, control is passed back up through the function call hierarchy to some driver

function. If a subordinate Interpreter function called by a superior Interpreter function returns an

error code, the superior stops where it is and passes the error code up to the function that called it.

When the error code reaches the driver, it may be reported (and is, in the SAI).

A.2 Handling Calculated Values

Since returned values are usually used as just described to handle the possibility of errors, an

alternative method of passing calculated values is required. In general, if Interpreter function A

needs a value for variable V calculated by Interpreter function B, this is handled by passing a

pointer to V from A to B, and B calculates and sets V. A few Interpreter functions in which no

errors can be detected return calculated values rather than error codes.

A.3 Compiler Macros

The Interpreter software for handling errors uses four compiler macros: CHK, CHP, ERM, and

ERP. Macros make the source more compact and easier to understand. Macros are used rather

than functions because a “return” statement needs to be included.

The CHK macro checks if a given condition is true and returns a given error code if so.

The CHP macro calls another Interpreter function. If the called function returns an error code,

CHP returns that code; otherwise, CHP does not cause a return.

ERP returns an error code generated in some other Interpreter function and passed to it.

ERM returns an error code originated in the function in which it resides.

All four macros record the name of the function in which they reside.

A.4 Automatic Generation of Software

The rs274ngc_error.cc and rs274ngc_return.hh files are generated automatically from the source

code file rs274ngc.cc. This is done by a combination of lex programs and shell scripts. The basic

approach is for the programmer (the authors of this report) to use symbolic values

(NCE_G_CODE_OUT_OF_RANGE, for example) while writing rs274ngc.cc. Each symbolic

value is the text of an error message set in all upper case letters, with spaces replaced by

underscores, and the prefix “NCE_” added.

In writing the source code, a new error message is used (as a symbolic value) whenever none of

the old ones is adequate to describe a particular error.

The lex programs and shell script read the source code file, pull out the error symbols (keeping

track of which message comes from which function(s)), remove duplicates, alphabetize the list,

assign an integer value to each symbol in the list, and write the list in the rs274ngc_return.hh file.
 RS274/NGC Interpreter - Version 3

72

A typical line of the file is #define NCE_G_CODE_OUT_OF_RANGE 82, for example.

The lex programs and shell script also convert each symbol back to text by removing the prefix,

changing all letters except the first to lower case, and putting spaces back in where there are

underscores. The text strings are written as a C array in the rs274ngc_error.cc file. That file also

includes the index numbers as comments and the names of the functions which can give the

messages. A typical line of the file is, for example:

/* 82 */ "G code out of range", // read_g

A.5 Interpreter Bugs

The Interpreter has no known bugs.

Error messages in the rs274ngc_error.cc file beginning with the word “Bug” should never appear

but are provided as a check on the internal workings of the Interpreter. The appearance of one of

these means there is a bug in the source code for the Interpreter. If one of these error messages

ever appears, please contact kramer@cme.nist.gov by E-mail; include the message and describe

the circumstances in which it appeared.

A.6 Stand-Alone Interpreter Driver Error Messages

The following error messages may be printed by the SAI. Each message describes an error in the

SAI that is not an Interpreter error. In the list below, each message is followed by the names of the

driver function(s) that can print it. The messages originate in the source code for the SAI driver. A

word in bold italics stands for a number or word that will differ according the exact nature of the

error. The error messages are not kept in an array.

1. Bad input line line text in tool file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . read_tool_file

2. Bad tool file format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . read_tool_file

3. Cannot open file name . . . . . . . . . . . . . . . . . . . . . . . read_tool_file, designate_parameter_file

4. Could not open output file file name . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . main

5. Out of range tool slot number slot number. . . . . . . . . . . . . . . . . . . . . . . . . . . . read_tool_file

6. Unknown error, bad error code. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . report_error
 RS274/NGC Interpreter - Version 3

73

Appendix B. Cutter Radius Compensation

This appendix discusses cutter radius compensation. It is intended for NC programmers and

machine operators. Researchers and developers may find it useful. SAI system installers will

probably not find it useful.

See Section 3.5.10 for additional information on cutter radius compensation.

B.1 Introduction

The cutter radius compensation1capabilities of the Interpreter enable the programmer to specify

that a cutter should travel to the right or left of an open or closed contour in the XY-plane

composed of arcs of circles and straight line segments.

Cutter radius compensation is performed only with the XY-plane active. All the figures in this

appendix, therefore, show projections on the XY-plane.

Where the adjacent sides of remaining material meet at a corner, there are two common ways to

handle the tool path. The tool may pass in an arc around the corner, or the tool path may continue

straight in the direction it was going along the first side until it reaches a point where it changes

direction to go straight along the second side. Figure 2 shows these two types of path. On Figure

2:

• Uncut material is shaded in the figures. Note that the inner triangles have the same

shape with both tool paths.

• The white areas are the areas cleared by the tool.

• The lines in the center of the white areas represent the path of the tip of a cutting tool.

• The tool is the cross-hatched circles.

Both paths will clear away material near the shaded triangle and leave the shaded triangle uncut.

When the Interpreter performs cutter radius compensation, the tool path is rounded at the corners,

as shown on the left in Figure 2. In the method on the right (the one not used), the tool does not

stay in contact with the shaded triangle at sharp corners, and more material than necessary is

removed.

There are also two alternatives for the path that is programmed in NC code during cutter radius

compensation. The programmed path may be either (1) the edge of the material to remain uncut

(for example, the edge of the inner triangle on the left of Figure 2), or (2) the nominal tool path

(for example, the tool path on the left side of Figure 2). The nominal tool path is the path that

would be used if the tool were exactly the intended size. The Interpreter will handle both cases

without being told which one it is. The two cases are very similar, but different enough that they

are described in separate sections of this manual. To use the material edge method, read Appendix

B.3. To use the nominal path method, read Appendix B.4.

1. The term “cutter diameter compensation” is often used to mean the same thing.
 RS274/NGC Interpreter - Version 3

74

Z-axis motion may take place while the contour is being followed in the XY-plane. Portions of the

contour may be skipped by retracting the Z-axis above the part, following the contour to the next

point at which machining should be done, and re-extending the Z-axis. These skip motions may

be performed at feed rate (G1) or at traverse rate (G0). The Z motion will not interfere with the

XY path following. The sample NC code in this appendix does not include moving the Z-axis. In

actual programs, include Z-axis motion wherever you want it.

Rotational axis motions (A, B, and C axes) are allowed with cutter radius compensation, but using

them would be very unusual.

Inverse time feed rate (G93) or units per minute feed rate (G94) may be used with cutter radius

compensation. Under G94, the feed rate will apply to the actual path of the cutter tip, not to the

programmed contour.

B.1.1 Data for Cutter Radius Compensation

The Interpreter world model keeps three data items for cutter radius compensation: the setting

itself (right, left, or off), program_x, and program_y. The last two represent the X and Y positions

which are given in the NC code while compensation is on. When compensation is off, these both

Figure 2. Two Cutter Radius Compensation Methods

NOT This way

Interpreter does

Tool Path

it this way

Cutter
 RS274/NGC Interpreter - Version 3

75

are set to a very small number (10-20) whose symbolic value is “unknown”. The Interpreter world

model uses the data items current_x and current_y to represent the position of the center of the

tool tip (in the currently active coordinate system) at all times.

B.2 Programming Instructions

B.2.1 Turning Cutter Radius Compensation On

To start cutter radius compensation keeping the tool to the left of the contour, program G41 D... .

The D word is optional (see “Use of D Number”, just below).

To start cutter radius compensation keeping the tool to the right of the contour, program G42 D...

In Figure 2, for example, if G41 were programmed, the tool would move clockwise around the

triangle, so that the tool is always to the left of the triangle when facing in the direction of travel.

If G42 were programmed, the tool would stay right of the triangle and move counterclockwise

around the triangle.

B.2.2 Turning Cutter Radius Compensation Off

To stop cutter radius compensation, program G40. It is OK to turn compensation off when it is

already off.

B.2.3 Sequencing

If G40, G41, or G42 is programmed on the same line as tool motion, cutter compensation will be

turned on or off before the motion is made. To make the motion come first, the motion must be

programmed on a separate, previous line of code.

B.2.4 Use of D Number

Programming a D word with G41 or G42, is optional.

If a D number is programmed, it must be a non-negative integer. It represents the slot number of

the tool whose radius (half the diameter given in the tool table) will be used, or it may be zero

(which is not a slot number). If it is zero, the value of the radius will also be zero. Any slot in the

tool table may be selected. The D number does not have to be the same as the slot number of the

tool in the spindle, although it is rarely useful for it not to be.

If a D number is not programmed, the slot number of the tool in the spindle will be used as the D

number.

B.3 Material Edge Contour

When the contour is the edge of the material, the outline of the edge is described in the NC

program.

For a material edge contour, the value for the diameter in the tool table is the actual value of the

diameter of the tool. The value in the table must be positive. The NC code for a material edge

contour is the same regardless of the (actual or intended) diameter of the tool.
 RS274/NGC Interpreter - Version 3

76

B.3.1 Programming Entry Moves

In general, two pre-entry moves and one entry move are needed to begin compensation correctly.

However, if there is a convex corner on the contour, a simpler method is available using zero or

one pre-entry move and one entry move. The general method, which will work in all situations, is

described first. We assume here that the programmer knows what the contour is already and has

the job of adding entry moves.

B.3.1.1 General Method

The general method includes programming two pre-entry moves and one entry move. See Figure

3. The shaded area is the remaining material. It has no corners, so the simple method cannot be

used. The dotted line is the programmed path. The solid line is the actual path of the tool tip. Both

paths go clockwise around the remaining material. A cutter one unit in diameter is shown part

way around the path. The black dots mark points at the beginning or end of programmed or actual

moves. The figure shows the second pre-entry move but not the first, since the beginning point of

the first pre-entry move could be anywhere.

First, pick a point A on the contour where it is convenient to attach an entry arc. Specify an arc

outside the contour which begins at a point B and ends at A tangent to the contour (and going in

Figure 3. Cutter Radius Compensation Entry Moves

for material edge contour

•

•

B (1, 4)

C (1, 5)

A (2, 3)

•

•

•

•

•

•

•

• •

•

•

•

•

• •

•

programmed path

actual path

Cutter
 RS274/NGC Interpreter - Version 3

77

the same direction as it is planned to go around the contour). The radius of the arc should be larger

than half the diameter given in the tool table. Then extend a line tangent to the arc from B to some

point C, located so that the line BC is more than one tool radius long. After the construction is

finished, the code is written in the reverse order from the construction. The NC code is shown in

Table 12; the first three lines are the entry moves just described.

Cutter radius compensation is turned on after the first pre-entry move and before the second preentry move (including G41 on the same line as the second pre-entry move turns compensation on

before the move is made). In the code above, line N0010 is the first pre-entry move, line N0020

turns compensation on and makes the second pre-entry move, and line N0030 makes the entry

move.

B.3.1.2 Simple Method

If there is a convex (sticking out, not in) corner somewhere on the contour, a simpler method of

making an entry is available. See Figure 4.

First, pick a convex corner. There is only one corner in Figure 4. It is at A, and it is convex. Decide

which way you want to go along the contour from A. In our example we are keeping the tool to

the left of the remaining material and going clockwise. Extend the side to be cut (DA in the figure)

to divide the area outside the material near A into two regions; DA extended is the dotted line AC

on the figure. Make a pre-entry move to anywhere in the region on the same side of DC as the

remaining material (point B on the figure) and not so close to the remaining material that the tool

is cutting into it. Anywhere in the diagonally shaded area of the figure (or above or to the left of

that area) is OK. If the tool is already in region, no pre-entry move is needed. Write a line of NC

code to move to B, if necessary. Then write a line of NC code for a straight entry move that turns

compensation on and goes to point A. If B is at (1.5, 4), the two lines of code for the pre-entry and

entry moves would be:

N0010 G1 X1.5 Y4 (move to B)

N0020 G41 G1 X3 Y3 (turn compensation on and make entry move to A)

These two lines would be followed by four lines identical to lines N0050 to N0080 from Table 12,

but the end of the program would be different since the shape of remaining material is different.

N0010 G1 X1 Y5 (make first pre-entry move to C)

N0020 G41 G1 Y4 (turn compensation on and make second pre-entry move to point B)

N0030 G3 X2 Y3 I1 (make entry move to point A)

N0040 G2 X3 Y2 J-1 (cut along arc at top)

N0050 G1 Y-1 (cut along right side)

N0060 G2 X2 Y-2 I-1 (cut along arc at bottom right)

N0070 G1 X-2 (cut along bottom side)

N0080 G2 X-2.6 Y-0.2 J1 (cut along arc at bottom left)

N0090 G1 X1.4 Y2.8 (cut along third side)

N0100 G2 X2 Y3 I0.6 J-0.8 (cut along arc at top of tool path)

N0110 G40 (turn compensation off)

Table 12. NC Program for Figure 3
 RS274/NGC Interpreter - Version 3

78

It would be OK for B to be on line AC. In fact, B could be placed on the extension outside the part

of any straight side of the part. B could be placed on EF extended to the right (but not to the left,

for going clockwise), for example.

If DA were an arc, not a straight line, the two lines of code above would still be suitable. In this

case, the dotted line extending DA should be tangent to DA at A.

B.4 Nominal Path Contour

When the contour is a nominal path contour (the path a tool with exactly the intended diameter

would take), the tool path is described in the NC program. It is expected that (except for during

the entry moves) the path is intended to create some part geometry. The path may be generated

manually or by a post-processor, considering the part geometry which is intended to be made. For

the Interpreter to work, the tool path must be such that the tool stays in contact with the edge of

the part geometry, as shown on the left side of Figure 2. If a path of the sort shown on the right of

Figure 2 is used, in which the tool does not stay in contact with the part geometry all the time, the

Interpreter will not be able to compensate properly when undersized tools are used. A nominal

path contour has no corners, so the simple method just described will not work.

For a nominal path contour, the value for the cutter diameter in the tool table will be a small

positive number if the selected tool is slightly oversized and will be a small negative number if the

Figure 4. Simpler Cutter Radius Compensation Entry Move

for material edge contour

A (3, 3)

•

•

• •

• •

•

•

•

•

•

•

•

programmed path

actual path

D

B

E F

• C

Cutter
 RS274/NGC Interpreter - Version 3

79

tool is slightly undersized. If a cutter diameter value is negative, the Interpreter compensates on

the other side of the contour from the one programmed and uses the absolute value of the given

diameter. If the actual tool is the correct size, the value in the table should be zero. Suppose, for

example, the diameter of the cutter currently in the spindle is 0.97, and the diameter assumed in

generating the tool path was 1.0. Then the value in the tool table for the diameter for this tool

should be -0.03.

The nominal tool path needs to be programmed so that it will work with the largest and smallest

tools expected to be actually used. We will call the difference between the radius of the largest

expected tool and the intended radius of the tool the “maximum radius difference.” This is usually

a small number.

The method includes programming two pre-entry moves and one entry moves. See Figure 5. The

shaded area is the remaining material. The dashed line is the programmed tool path. The solid line

is the actual path of the tool tip. Both paths go clockwise around the remaining material. The

actual path is to the right of the programmed path even though G41 was programmed, because the

diameter value is negative. On the figure, the distance between the two paths is larger than would

normally be expected. The 1-inch diameter tool is shown part way around the path. The black dots

mark points at the beginning or end of programmed moves. The corresponding points on the

actual path have not been marked. The actual path will have a very small additional arc near point

B unless the tool diameter is exactly the size intended. The figure shows the second pre-entry

move but not the first, since the beginning point of the first pre-entry move could be anywhere.

First, pick a point A on the contour where it is convenient to attach an entry arc. Specify an arc

outside the contour which begins at a point B and ends at A tangent to the contour (and going in

the same direction as it is planned to go around the contour). The radius of the arc should be larger

than the maximum radius difference. Then extend a line tangent to the arc from B to some point

C, located so that the length of line BC is more than the maximum radius difference. After the

construction is finished, the code is written in the reverse order from the construction. The NC

code is shown in Table 13; the first three lines are the entry moves just described.

N0010 G1 X1.5 Y5 (make first pre-entry move to C)

N0020 G41 G1 Y4 (turn compensation on and make second pre-entry move to point B)

N0030 G3 X2 Y3.5 I0.5 (make entry move to point A)

N0040 G2 X3.5 Y2 J-1.5 (cut along arc at top)

N0050 G1 Y-1 (cut along right side)

N0060 G2 X2 Y-2.5 I-1.5 (cut along arc at bottom right)

N0070 G1 X-2 (cut along bottom side)

N0080 G2 X-2.9 Y0.2 J1.5 (cut along arc at bottom left)

N0090 G1 X1.1 Y3.2 (cut along third side)

N0100 G2 X2 Y3.5 I0.9 J-1.2 (cut along arc at top of tool path)

N0110 G40 (turn compensation off)

Table 13. NC Program for Figure 5
 RS274/NGC Interpreter - Version 3

80

Cutter radius compensation is turned on after the first pre-entry move and before the second preentry move (including G41 on the same line as the second pre-entry move turns compensation on

before the move is made). In the code above, line N0010 is the first pre-entry move, line N0020

turns compensation on and makes the second pre-entry move, and line N0030 makes the entry

move.

B.5 Programming Errors and Limitations

The Interpreter will issue the following error messages involving cutter radius compensation. In

addition to these, there are several bug messages related to cutter compensation, but they should

never occur.

1. Cannot change axis offsets with cutter radius comp

2. Cannot change units with cutter radius comp

3. Cannot probe with cutter radius comp on

4. Cannot turn cutter radius comp on out of xy-plane

5. Cannot turn cutter radius comp on when on

6. Cannot use g28 or g30 with cutter radius comp

7. Cannot use g53 with cutter radius comp

Figure 5. Cutter Radius Compensation Entry Moves

for nominal path contour

•

•

B (1.5, 4)

C (1.5, 5)

A (2, 3.5)

•

•

•

• •

•

•

programmed path

actual path

Cutter
 RS274/NGC Interpreter - Version 3

81

8. Cannot use xz-plane with cutter radius comp

9. Cannot use yz-plane with cutter radius comp

10. Concave corner with cutter radius comp

11. Cutter gouging with cutter radius comp

12. D word with no g41 or g42

13. Multiple d words on one line

14. Negative d word tool radius index used

15. Tool radius index too big

16. Tool radius not less than arc radius with comp

17. Two g codes used from same modal group.

Most of these are self-explanatory. For those that require explanation, an explanation is given

below.

Changing a tool while cutter radius compensation is on is not treated as an error, although it is

unlikely this would be done intentionally. The radius used when cutter radius compensation was

first turned on will continue to be used until compensation is turned off, even though a new tool is

actually being used.

B.5.1 Concave Corner and Tool Radius Too Big (10 and 16)

When cutter radius compensation is on, it must be physically possible for a circle whose radius is

the half the diameter given in the tool table to be tangent to the contour at all points of the contour.

In particular, the Interpreter treats concave corners and concave arcs into which the circle will not

fit as errors, since the circle cannot be kept tangent to the contour in these situations. See Figure 6.

This error detection does not limit the shapes which can be cut, but it does require that the

programmer specify the actual shape to be cut (or path to be followed), not an approximation. In

this respect, the NIST RS274/NGC Interpreter differs from interpreters used with many other

controllers, which often allow these errors silently and either gouge the part or round the corner.

B.5.2 Cannot Turn Cutter Radius Comp on When On (5)

If cutter radius compensation has already been turned on, it cannot be turned on again. It must be

turned off first; then it can be turned on again. It is not necessary to move the cutter between

turning compensation off and back on, but the move after turning it back on will be treated as a

Figure 6. Two Cutter Radius Compensation Errors

In both examples, the line represents a contour, and the circle represents the cross section of a

tool following the contour using cutter radius compensation (tangent to one side of the path.)

concave corner - tool does not fit concave arc too small - tool does not fit
 RS274/NGC Interpreter - Version 3

82

first move, as described below.

It is not possible to change from one cutter radius index to another while compensation is on

because of the combined effect of rules 5 and 12. It is also not possible to switch compensation

from one side to another while compensation is on.

B.5.3 Cutter Gouging (11)

If the tool is already covering up the next XY destination point when cutter radius compensation

is turned on, the gouging message is given when the line of NC code which gives the point is

reached. In this situation, the tool is already cutting into material it should not cut. More details

are given in Section B.6.

B.5.4 Tool Radius Index Too Big (15)

If a D word is programmed that is larger than the number of tool carousel slots, this error message

is given. In the SAI, the number of slots is 68.

B.5.5 Two G Codes Used from Same Modal Group (17)

This is a generic message used for many sets of G codes. As applied to cutter radius

compensation, it means that more than one of G40, G41, and G42 appears on a line of NC code.

This is not allowed.

B.6 First Move into Cutter Compensation

The algorithm used for the first move after cutter radius compensation is turned on, when the first

move is a straight line, is to draw a straight line from the programmed destination point which is

tangent to a circle whose center is at the current point and whose radius is the radius of the tool.

The destination point of the tool tip is then found as the center of a circle of the same radius

tangent to the tangent line at the destination point. If the programmed point is inside the initial

cross section of the tool (the circle on the left), an error is signalled as described in Section B.5.3.

The concept of the algorithm is shown in Figure 7.

The function that locates the destination point actually takes a computational shortcut based on

the fact that the line (not drawn on the figure) from the current point to the programmed point is

the hypotenuse of a right triangle having the destination point at the corner with the right angle.

Figure 7. First Cutter Radius Compensation Move - Straight

Second, construct this line to

determine the destination point

programmed point

current point

First, construct this line.

destination point of tool tip path of tool tip
 RS274/NGC Interpreter - Version 3

83

If the first move after cutter radius compensation has been turned on is an arc, the arc which is

generated is derived from an auxiliary arc which has its center at the programmed center point,

passes through the programmed end point, and is tangent to the cutter at its current location. If the

auxiliary arc cannot be constructed, an error is signalled. The generated arc moves the tool so that

it stays tangent to the auxiliary arc throughout the move. This is shown in Figure 8.

Figure 8 shows the conceptual approach for finding the arc. The actual computations differ

between the center format arc and the radius format arc (see Section 3.5.3).

After the entry moves of cutter radius compensation, the Interpreter keeps the tool tangent to the

programmed path on the appropriate side. If a convex corner is on the path, an arc is inserted to go

around the corner. The radius of the arc is half the diameter given in the tool table.

When cutter radius compensation is turned off, no special exit move takes place. The next move is

what it would have been if cutter radius compensation had never been turned on and the previous

move had placed the tool at its current position.

The Interpreter signals when cutter radius compensation is turned on or off by calling the

COMMENT canonical function with a message to that effect.

Figure 8. First Cutter Radius Compensation Move - Arc

programmed/computed

center point

current point

First, construct this auxiliary arc.

programmed end point

destination point of tool tip

Second, construct this arc,

which is the path taken.
 RS274/NGC Interpreter - Version 3

84

Appendix C. Sample Programs

This appendix includes three sample programs. This section is intended to be useful to NC

programmers and machine operators. Others will probably not find it useful. Additional sample

programs are given in Table 6 (hole probing), Table 12 and Table 13 (cutter radius compensation).

A transcript of a session using the SAI with keyboard input is shown in Table 10. Table 12 and

Table 13 are only sections of programs and need a line at the beginning (to select tool, change

tool, start spindle, and set feed and speed rates) and a line at the end (an M2 to end the program).

C.1 Sample Simple Program

The classical simple computer program prints “Hello world”. Here it is in RS274/NGC. The

program may be safely run on a machining center.

(this program mills “Hello world” between X=0 and X=81 millimeters)

n0010 g21 g0 x0 y0 z50 (top of part should be on XY plane)

n0020 t1 m6 m3 f20 s4000 (use an engraver or small ball-nose endmill)

n0030 g0 x0 y0 z2

n0040 g1 z-0.5 (start H)

n0050 y10

n0060 g0 z2

n0070 y5

n0080 g1 z-0.5

n0090 x 7

n0100 g0 z2

n0110 y0

n0120 g1 z-0.5

n0130 y10

n0140 g0 z2

n0150 x11 y2.5

n0160 g1 z-0.5 (start e)

n0170 x16

n0190 g3 x13.5 y0 i-2.5

n0200 g1 x16

n0210 g0 z2

n0220 x20 y0

n0230 g1 z-0.5 (start l)

n0240 y9

n0250 g0 z2

n0260 x26

n0270 g1 z-0.5 (start l)

n0280 y0

n0290 g0 z2

n0300 x32.5

n0310 g1 z-0.5 (start o)

n0320 g2 x32.5 j2.5

n0330 g0 z2
 RS274/NGC Interpreter - Version 3

85

n0340 x45 y5

n0350 g1 z-0.5 (start w)

n0360 x47 y0

n0370 x48.5 y3

n0380 x50 y0

n0390 x52 y5

n0400 g0 z2

n0410 x57.5 y0

n0420 g1 z-0.5 (start o)

n0430 g2 x57.5 j2.5

n0440 g0 z2

n0450 x64

n0460 g1 z-0.5 (start r)

n0470 y5

n0480 y4

n0490 g2 x69 r4

n0500 g0 z2

n0510 x73 y0

n0520 g1 z-0.5 (start l)

n0530 y9

n0540 g0 z2

n0550 x81

n0560 g1 z-0.5 (start d)

n0570 y0

n0580 x79.5

n0590 g2 j2.5 y5

n0600 g1 x81

n0610 g0 z50

n0620 m2

C.2 Sample Program to Test Expressions

This file is to test the interpretation of expressions. It tests all unary and binary functions

implemented. It also tests parameter setting and referencing. The last few lines test more

complicated expressions. This program is not intended to be run on a machining center. The tool

path is just random back and forth on the X-axis.

n0010 g21 g1 x3 f20 (expression test)

n0020 x [1 + 2] (x should be 3)

n0030 x [1 - 2] (x should be -1)

n0040 x [1 --3] (x should be 4)

n0050 x [2/5] (x should be 0.40)

n0060 x [3.0 * 5] (x should be 15)

n0070 x [0 OR 0] (x should be 0)

n0080 x [0 OR 1] (x should be 1)

n0090 x [2 or 2] (x should be 1)

n0100 x [0 AND 0] (x should be 0)
 RS274/NGC Interpreter - Version 3

86

n0110 x [0 AND 1] (x should be 0)

n0120 x [2 and 2] (x should be 1)

n0130 x [0 XOR 0] (x should be 0)

n0140 x [0 XOR 1] (x should be 1)

n0150 x [2 xor 2] (x should be 0)

n0160 x [15 MOD 4.0] (x should be 3)

n0170 x [1 + 2 * 3 - 4 / 5] (x should be 6.2)

n0180 x sin[30] (x should be 0.5)

n0190 x cos[0.0] (x should be 1.0)

n0200 x tan[60.0] (x should be 1.7321)

n0210 x sqrt[3] (x should be 1.7321)

n0220 x atan[1.7321]/[1.0] (x should be 60.0)

n0230 x asin[1.0] (x should be 90.0)

n0240 x acos[0.707107] (x should be 45.0000)

n0250 x abs[20.0] (x should be 20)

n0260 x abs[-1.23] (x should be 1.23)

n0270 x round[-0.499] (x should be 0)

n0280 x round[-0.5001] (x should be -1.0)

n0290 x round[2.444] (x should be 2)

n0300 x round[9.975] (x should be 10)

n0310 x fix[-0.499] (x should be -1.0)

n0320 x fix[-0.5001] (x should be -1.0)

n0330 x fix[2.444] (x should be 2)

n0340 x fix[9.975] (x should be 9)

n0350 x fup[-0.499] (x should be 0.0)

n0360 x fup[-0.5001] (x should be 0.0)

n0370 x fup[2.444] (x should be 3)

n0380 x fup[9.975] (x should be 10)

n0390 x exp[2.3026] (x should be 10)

n0400 x ln[10.0] (x should be 2.3026)

n0410 x [2 ** 3.0] #1=2.0 (x should be 8.0)

n0420 ##1 = 0.375 (#1 is 2, so parameter 2 is set to 0.375)

n0430 x #2 (x should be 0.375) #3=7.0

n0440 #3=5.0 x #3 (parameters set in parallel, so x should be 7, not 5)

n0450 x #3 #3=1.1 (parameters set in parallel, so x should be 5, not 1.1)

n0460 x [2 + asin[1/2.1+-0.345] / [atan[fix[4.4] * 2.1 * sqrt[16.8]] /[-18]]**2]

n0470 x sqrt[3**2 + 4**2] (x should be 5.0)

n0480 m2

C.3 Sample Program to Test Canned Cycles

This file tests canned cycles. It is not intended to be run on a machining center.

n0010 g20 (cycle test)

n0020 g17 g43 h1 m3 s1234 f16 (start in XY-plane)

n0030 g81 x3 y4 r0.2 z-1.1

n0040 x1 y0 r0 g91 l3 (three more g81’s an inch apart)
 RS274/NGC Interpreter - Version 3

87

n0050 y-2 r0.1 (one more g81)

n0060 g82 g90 x4 y5 r0.2 z-1.1 p0.6

n0070 x2 z-3.0 (one more G82)

n0080 g91 x-2 y2 r0 l4 (four more g82’s)

n0090 g83 g90 x5 y6 r0.2 z-1.1 q0.21

n0100 g84 x6 y7 r0.2 z-1.1

n0110 g85 x7 y8 r0.2 z-1.1

n0120 g86 x8 y9 r0.2 z-1.1 p902.61

n0130 g87 x9 y10 r0.2 z-1.1 i0.231 j-0 k-3

n0135 g91 x1 r0.2 z-1.1 i0.231 j-0 k-3

n0140 g88 x10 y11 r0.2 z-1.1 p0.3333

n0150 g89 x11 y12 r0.2 z-1.1 p1.272

n0160 m4 (run spindle counterclockwise)

n0170 g86 x8 y9 r0.2 z-1.1 p902.61

n0180 g87 x9 y10 r0.2 z-1.1 i0.231 j-0 k-3

n0190 g88 x10 y11 r0.2 z-1.1 p0.3333

n0220 g18 m3 (now run all cycles in the XZ-plane)

n0230 g81 z3 x4 r0.2 y-1.1

n0240 g91 z1 x0 r0 l3

n0260 g82 g90 z4 x5 r0.2 y-1.1 p0.6

n0280 g91 z-2 x2 r0 l4

n0290 g83 g90 z5 x6 r0.2 y-1.1 q0.21

n0300 g84 z6 x7 r0.2 y-1.1

n0310 g85 z7 x8 r0.2 y-1.1

n0320 g86 z8 x9 r0.2 y-1.1 p902.61

n0330 g87 z9 x10 r0.2 y-1.1 k0.231 i-0 j-3

n0335 g91 z1 r0.2 y-1.1 k0.231 i-0 j-3

n0340 g88 z10 x11 r0.2 y-1.1 p0.3333

n0350 g89 z11 x12 r0.2 y-1.1 p1.272

n0420 g19 (now run all cycles in the YZ-plane)

n0430 g81 y3 z4 r0.2 x-1.1

n0440 g91 y1 z0 r0 l3

n0460 g82 g90 y4 z5 r0.2 x-1.1 p0.6

n0480 g91 y-2 z2 r0 l4

n0490 g83 g90 y5 z6 r0.2 x-1.1 q0.21

n0500 g84 y6 z7 r0.2 x-1.1

n0510 g85 y7 z8 r0.2 x-1.1

n0520 g86 y8 z9 r0.2 x-1.1 p902.61

n0530 g87 y9 z10 r0.2 x-1.1 j0.231 k-0 i-3

n0535 g91 y1 r0.2 x-1.1 j0.231 k-0 i-3

n0540 g88 y10 z11 r0.2 x-1.1 p0.3333

n0550 g89 y11 z12 r0.2 x-1.1 p1.272

n1000 m2 (the end)
 RS274/NGC Interpreter - Version 3

88

Appendix D. Interpreter Software

This section describes the Interpreter software. NC programmers and machine operators should

never need to use this section. SAI installers should not need it but may find it helpful. Developers

and researchers should find the section useful.

D.1 Interpreter Interfaces

The Interpreter has four interfaces, as shown in Figure 9. These are all function call interfaces.

The direction of function calling is indicated by arrows. The flow of information in the reverse

direction from the arrows differs in the different interfaces.

The Interpreter-do-it functions tell the Interpreter to do something, such as read a line of NC code

or execute the line last read. These functions all return an integer status code as described in

Appendix A.1. The functions themselves are described in Appendix D.4. They are declared in

rs274ngc.hh and defined in rs274ngc_pre.cc. The names of these functions all begin with

“rs274ngc_”.

The Interpreter-give-information functions ask the Interpreter to give information. Some of these

functions pass from the driver a pointer to a place to put information. The Interpreter provides the

information either as a returned value, or by putting it into the place pointed at by the pointer. The

functions are described in Appendix D.5. They are declared in rs274ngc.hh and defined in

rs274ngc_pre.cc. The names of these functions all begin with “rs274ngc_”.

The canonical machining functions tell the rest of the system to do something. These functions do

not return anything. They are described in Section 4. They are declared in canon.hh and defined in

canon.cc. The names of these functions do not all have the same prefix.

The world-give-information functions ask the world outside the Interpreter to give the Interpreter

information. Some of these function pass from the Interpreter a pointer to a place to put

information. The world provides the information either as a returned value, or by putting it into

Interpreter

canonical machining

functions

world-give-information

functions

Figure 9. Interpreter Interfaces

Arrows show the direction of function calls.

Interpreter-give-information

functions

Interpreter-do-it

functions
 RS274/NGC Interpreter - Version 3

89

the place pointed at by the pointer. The functions are described in Appendix D.6. They are

declared in canon.hh and defined in canon.cc. The names of these functions all begin with

“GET_EXTERNAL_”.

D.2 Software Files and Organization

The Interpreter software is written in C++.

The files for the Interpreter and the rest of the SAI are:

Interpreter

1. rs274ngc_errors.cc

2. rs274ngc_return.hhs

3. rs274ngc_pre.cc

4. rs274ngc.hh

5. canon.hh

Rest of SAI

1. driver.cc

2. canon_pre.cc

The rs274ngc_pre.cc file is a bit over 12,000 lines. The other files are all in the range of 100 to

1100 lines.

The organization of the software by file is shown in Figure 10. The SAI uses the files shown in the

left and middle columns. The EMC Controller uses the files shown in the right and middle

columns. In the figure, arrows show the direction of function calls.

The rs274ngc_pre.cc file includes interface functions (the Interpreter-do-it and Interpreter-giveinformation functions) and other functions. In the file itself, the interface functions are given after

the other functions. As shown in Figure 10, other functions are called only by interface functions,

while interface functions are called by driver functions (in the SAI or EMC Controller). Both

interface functions and other functions call canonical machining functions and world-giveinformation functions.

Different versions of the canonical machining functions are used in the SAI and the EMC

Controller. The canonical machining functions used with the SAI print themselves and manipulate

an emulated environment, while those used in the EMC controller send messages which

ultimately lead to controlling the machine. The same header file, canon.hh, is used with both

versions of the functions.

As described in Appendix A.4, the rs274ngc_errors.cc and the rs274ngc_return.hh files are

prepared automatically.
 RS274/NGC Interpreter - Version 3

90

The source code is heavily documented. In general, for each function, four fields are given:

1. Returned Value - a description of possible returned values and the circumstances in which

particular values may be returned.

2. Side Effects - a description of the important side effects (things other than the returned value) of

executing a function. Since the returned value of most functions is used to indicate error status,

the side effects of most functions are important.

3. Called By - a list of functions which call the function being documented.

4. Arguments - a one-line description of the meaning of each argument to a function, placed

immediately after the declaration of the argument. This field is omitted if there are no arguments.

canon.hh

canon.cc canon.cc

driver.cc

(SAI driver)

EMC files

(EMC driver)

rs274ngc.hh

rs274ngc_pre.cc

interface functions

(Interpreter-do-it &

Interpreter-give-info

functions)

other

functions

Figure 10. Software

Files are in light grey boxes. Related sets of functions are in white boxes.

Arrows show the direction of function calls.

The four arrows on each side of the rs274ngc_pre.cc box are the four interfaces of Figure 9.

rs274ngc_errors.cc

rs274ngc_return.hh

canonical mach.

functions

(print self)

world-give-info

functions

canonical mach.

functions

(control machine)

world-give-info

functions

ONLY IN EMC

CONTROLLER

INTERPRETER —

IN SAI AND IN

EMC CONTROLLER

ONLY IN

SAI
 RS274/NGC Interpreter - Version 3

91

In addition to these four fields, most functions have a paragraph or two (up to several pages) of

discussion. These discussions include many references to the RS274 manuals [NCMS], [EIA],

[Monarch], and [Fanuc]. Where a function implements an algorithm for geometric or numerical

calculation (as do many of the functions having to do with cutter radius compensation, for

example), the algorithm is described.

D.3 Cyclic Operation

In the EMC Controller, Interpreter input may be taken from a file or via manual data input (MDI)

from the controller console. In the SAI, input may be taken from a file or from the keyboard of the

computer running the Interpreter. Two major phases of interpretation take place. In the first phase,

a call to rs274ngc_read causes the Interpreter to read a line of code, to check it somewhat, and to

store the information from the line in a structure called a “block”. In the second phase, a call to

rs274ngc_execute causes the Interpreter to examine the block, to check it further, and (usually) to

make calls to canonical machining functions.

D.3.1 Read, Store, and Check

The Interpreter reads lines of RS274/NGC code one at a time. First the line is read into a buffer.

Next, any spaces not in comments are removed, and any upper case letters not in comments are

changed to lower case letters.

Then the buffer and a counter holding the index of the next character to be read are handed around

among a lot of functions named read_XXXX. All such functions read characters from the buffer

using the counter. They all reset the counter to point at the character in the buffer following the

last one used by the function. The first character read by most of these functions is expected to be

a member of some set of characters (often a specific single character), and each function checks

the first character.

Each line of code is stored until it has been executed in a reusable “block” structure, which has a

slot for every potential piece of information on the line. Each time a useful piece of information

has been extracted from the line, the information is put into the block.

The read_XXXX functions do a lot of error detection, but they only look for errors which would

cause reading or storing to fail. After reading and storing is complete, more checking functions

(check_g_codes, check_m_codes, and check_other_codes) are run. These functions look for

logical errors, such as all axis words missing with a G code for motion in effect.

D.3.2 Execute

Once a block is built and checked, the block is executed by the execute_block function, which

calls one or more functions named convert_XXXX. In RS274/NGC, as in all dialects of RS274, a

line of code may specify several different things to do, such as moving from one place to another

along a straight line or arc, changing the feed rate, starting the spindle turning, etc. The order of

execution is shown in Table 8.

D.4 Interpreter-do-it Functions

This section describes the Interpreter-do-it functions. They are arranged alphabetically. All

function names start with “rs274ngc_”.
 RS274/NGC Interpreter - Version 3

92

int rs274ngc_close();

Close the currently open NC code file.

int rs274ngc_execute();

Execute the block representing the last line of NC code that was read.

int rs274ngc_exit();

Stop running.

int rs274ngc_init();

Get ready to run.

int rs274ngc_load_tool_table();

Load a tool table.

int rs274ngc_open(const char * filename);

Open the NC code file whose name is filename.

int rs274ngc_read(const char * mdi = 0);

If mdi is not null, read the string mdi points to. If mdi is null, read the next line of the

currently open NC code file.

int rs274ngc_reset();

Reset yourself.

int rs274ngc_restore_parameters(const char * filename);

Restore parameters from the file named filename.

int rs274ngc_save_parameters(const char * filename, const double

parameters[]);

Save the parameters in the file named filename.

int rs274ngc_synch();

synchronize your internal world model with the external world.

D.5 Interpreter-give-information Functions

These are interface functions to call to get information from the Interpreter. If a function has a

return value, the return value contains the information. If a function returns nothing, information

is copied into one of the arguments to the function. These functions do not change the state of the

Interpreter.

void rs274ngc_active_g_codes(int * codes);

Copy active G codes into the codes array [0]..[11].

void rs274ngc_active_m_codes(int * codes);

Copy active M codes into the codes array [0]..[6].

void rs274ngc_active_settings(double * settings);

Copy active F, S settings into the settings array [0]..[2].
 RS274/NGC Interpreter - Version 3

93

void rs274ngc_error_text(int error_code, char * error_text, int

max_size);

Copy the text of the error message whose number is error_code into the error_text

array, but stop at max_size if the text is longer.

void rs274ngc_file_name(char * file_name, int max_size);

Copy the name of the currently open file into the file_name array, but stop at max_size

if the name is longer.

int rs274ngc_line_length();

Return the length of the most recently read line.

void rs274ngc_line_text(char * line_text, int max_size);

Copy the text of the most recently read line into the line_text array, but stop at

max_size if the text is longer.

int rs274ngc_sequence_number();

Return the current sequence number (how many lines read).

void rs274ngc_stack_name(int stack_index, char * function_name,

int max_size);

Copy the function name from the stack_index’th position of the function call stack at the

time of the most recent error into the function_name string, but stop at max_size if the

name is longer.

D.6 World-give-information Functions

This section describes the world-give-information functions. These functions get information for

the Interpreter. They are arranged alphabetically. All function names start with

“GET_EXTERNAL_”.

double GET_EXTERNAL_ANGLE_UNIT_FACTOR();

Return the system angular unit factor, in units / degree. The Interpreter is not currently using

this function.

double GET_EXTERNAL_FEED_RATE();

Return the system feed rate.

int GET_EXTERNAL_FLOOD();

Return the system value for flood coolant, zero = off, non-zero = on.

double GET_EXTERNAL_LENGTH_UNIT_FACTOR();

Return the system length unit factor, in units / mm. The Interpreter is not currently using this

function.

CANON_UNITS GET_EXTERNAL_LENGTH_UNIT_TYPE();

Return the system length unit type.

int GET_EXTERNAL_MIST();

Return the system value for mist coolant, zero = off, non-zero = on.
 RS274/NGC Interpreter - Version 3

94

CANON_MOTION_MODE GET_EXTERNAL_MOTION_CONTROL_MODE();

Return the current path control mode.

double GET_EXTERNAL_ORIGIN_A();

double GET_EXTERNAL_ORIGIN_B();

double GET_EXTERNAL_ORIGIN_C();

double GET_EXTERNAL_ORIGIN_X();

double GET_EXTERNAL_ORIGIN_Y();

double GET_EXTERNAL_ORIGIN_Z();

The Interpreter is not using these six GET_EXTERNAL_ORIGIN functions, each of which

returns the current value of the origin offset for the axis it names.

void GET_EXTERNAL_PARAMETER_FILE_NAME(char * filename, int

max_size);

Return nothing but copy the name of the parameter file into the filename array, stopping at

max_size if the name is longer. An empty string may be placed in filename.

CANON_PLANE GET_EXTERNAL_PLANE();

Return the currently active plane.

double GET_EXTERNAL_POSITION_A();

double GET_EXTERNAL_POSITION_B();

double GET_EXTERNAL_POSITION_C();

double GET_EXTERNAL_POSITION_X();

double GET_EXTERNAL_POSITION_Y();

double GET_EXTERNAL_POSITION_Z();

Each of the six functions above returns the current position for the axis it names.

double GET_EXTERNAL_PROBE_POSITION_A();

double GET_EXTERNAL_PROBE_POSITION_B();

double GET_EXTERNAL_PROBE_POSITION_C();

double GET_EXTERNAL_PROBE_POSITION_X();

double GET_EXTERNAL_PROBE_POSITION_Y();

double GET_EXTERNAL_PROBE_POSITION_Z();

Each of the six functions above returns the position at the last probe trip for the axis it names.

double GET_EXTERNAL_PROBE_VALUE();

Return the value for any analog non-contact probing.

int GET_EXTERNAL_QUEUE_EMPTY();

Return zero if queue is not empty, non-zero if the queue is empty.

double GET_EXTERNAL_SPEED();

Return the system value for the spindle speed setting in revolutions per minute (rpm). The

actual spindle speed may differ from this.

CANON_DIRECTION GET_EXTERNAL_SPINDLE();

Return the system value for direction of spindle turning.
 RS274/NGC Interpreter - Version 3

95

double GET_EXTERNAL_TOOL_LENGTH_OFFSET();

Return the current tool length offset.

int GET_EXTERNAL_TOOL_MAX();

returns number of slots in carousel.

int GET_EXTERNAL_TOOL_SLOT();

Returns the system value for the carousel slot in which the tool currently in the spindle

belongs. Return value zero means there is no tool in the spindle.

CANON_TOOL_TABLE GET_EXTERNAL_TOOL_TABLE(int pocket);

Returns the CANON_TOOL_TABLE structure associated with the tool in the given pocket. A

CANON_TOOL_TABLE structure has three data elements: id (an int), length (a double), and

diameter (a double).

double GET_EXTERNAL_TRAVERSE_RATE();

Returns the system traverse rate.

D.7 Interpreter Function Call Hierarchies

Function call hierarchies are shown in the following six figures. Except in Figure 13, which is

highly recursive, if a function is called by more than one other function, its name may appear

more than once in a figure. The functions called by a function are those listed underneath the

calling function, one level further indented than the calling function. In Figure 13, function calls

are shown with arrows from the caller to the called.

Figure 11 shows the hierarchies of all Interpreter-do-it functions other than rs274ngc_read and

rs274ngc_execute.

Figure 12 and Figure 13 show the hierarchy starting with the Interpreter-do-it function

rs274ngc_read. Figure 12 stops at read_real_value and Figure 13 begins there.

Figure 14 and Figure 15 show the hierarchy starting with the Interpreter-do-it function

rs274_ngc_execute. Figure 14 stops at convert_motion and Figure 15 begins there.

Figure 16 shows the hierarchy of function calls from the driver.

Calls to canonical machining functions are not included in the figures.
 RS274/NGC Interpreter - Version 3

96

rs274ngc_close

rs274ngc_reset

rs274ngc_exit

GET_EXTERNAL_PARAMETER_FILE_NAME

rs274ngc_reset

rs274ngc_save_parameters

rs274ngc_init

GET_EXTERNAL_LENGTH_UNIT_TYPE

GET_EXTERNAL_PARAMETER_FILE_NAME

rs274ngc_restore_parameters

rs274ngc_synch

write_g_codes

write_m_codes

write_settings

rs274ngc_load_tool_table

GET_EXTERNAL_TOOL_TABLE

rs274ngc_open

rs274ngc_reset

rs274ngc_reset

rs274ngc_restore_parameters

rs274ngc_save_parameters

rs274ngc_synch

GET_EXTERNAL_FEED_RATE

GET_EXTERNAL_FLOOD

GET_EXTERNAL_LENGTH_UNIT_TYPE

GET_EXTERNAL_MIST

GET_EXTERNAL_MOTION_CONTROL_MODE

GET_EXTERNAL_PLANE

GET_EXTERNAL_POSITION_A

GET_EXTERNAL_POSITION_B

GET_EXTERNAL_POSITION_C

GET_EXTERNAL_POSITION_X

GET_EXTERNAL_POSITION_Y

GET_EXTERNAL_POSITION_Z

GET_EXTERNAL_SPEED

GET_EXTERNAL_SPINDLE

GET_EXTERNAL_TOOL_MAX

GET_EXTERNAL_TOOL_SLOT

GET_EXTERNAL_TRAVERSE_RATE

rs274ngc_load_tool_table

Figure 11. Interpreter-do-it Function Call Hierarchy

This figure shows the hierarchy of function calls from Interpreter-do-it functions to other

Interpreter functions and to world-give-information functions. This figure does not show the

sub-hierarchies starting at rs274ngc_read. (see Figure 12 and Figure 13) and rs274ngc_execute

(see Figure 14 and Figure 15).

Interpreter-do-it interface functions are shown in boldface, other Interpreter functions are

shown in ordinary typeface, and world-give-information functions are shown in ITALIC.
 RS274/NGC Interpreter - Version 3

97

rs274ngc_read

GET_EXTERNAL_QUEUE_EMPTY

read_text

close_and_downcase

set_probe_data

parse_line

check_items

check_g_codes

check_m_codes

check_other_codes

enhance_block

init_block

read_items

read_line_number

read_integer_unsigned

read_one_item

read_a (read_real_value)

read_b (read_real_value)

read_c (read_real_value)

read_comment

read_d

read_integer_value (read_real_value)

read_f (read_real_value)

read_g (read_real_value)

read_h

read_integer_value (read_real_value)

read_i (read_real_value)

read_j (read_real_value)

read_k (read_real_value)

read_l

read_integer_value (read_real_value)

read_m

read_integer_value (read_real_value)

read_p (read_real_value)

read_parameter_setting (read_real_value)

read_integer_value (read_real_value)

read_q (read_real_value)

read_r (read_real_value)

read_s (read_real_value)

read_t

read_integer_value (read_real_value)

read_x (read_real_value)

read_y (read_real_value)

read_z (read_real_value)

Figure 12. Interpreter Function Call Hierarchy

(from rs274_ngc read)

This figure shows the hierarchy of function calls from the Interpreter function rs274ngc_read to

other Interpreter functions. This figure does not show the sub-hierarchy starting at

read_real_value. That is shown in Figure 13. To save space, calls to read_real_value are shown

in parentheses next to the caller, rather than indented below the caller.

Interpreter-do-it interface functions are shown in boldface, other Interpreter functions are

shown in ordinary typeface, and world-give-information functions are shown in ITALIC.
 RS274/NGC Interpreter - Version 3

98

Figure 13. Interpreter Function Call Hierarchy

(from read_real_value)

This shows the hierarchy of function calls from read_real_value.

Interpreter-do-it interface functions are shown in boldface, other Interpreter functions are

shown in ordinary typeface, and world-give-information functions are shown in ITALIC.

read_unary

read_real_value read_real_expression

precedence

execute_binary

read_integer_value

read_real_number

read_parameter

read_operation

execute_unary

read_operation_unary

read_atan

execute_binary1

execute_binary2
 RS274/NGC Interpreter - Version 3

99

rs274ngc_execute

write_g_codes

write_m_codes

write_settings

execute_block

convert_comment

convert_feed_mode

convert_feed_rate

convert_g

convert_control_mode

convert_coordinate_system

convert_cutter_compensation

convert_cutter_comp_off

convert_cutter_comp_on

convert_distance_mode

convert_dwell

convert_length_units

convert_modal_0

convert_axis_offsets

convert_home

find_ends

find_relative

convert_setup

convert_motion (see Figure 15)

convert_retract_mode

convert_set_plane

convert_tool_length_offset

convert_m

convert_tool_change

convert_speed

convert_stop

convert_tool_select

Figure 14. Interpreter Function Call Hierarchy

(from rs274ngc_execute)

This shows the hierarchy of function calls from rs274ngc_execute to other Interpreter functions.

Interpreter-do-it interface functions are shown in boldface, other Interpreter functions are

shown in ordinary typeface, and world-give-information functions are shown in ITALIC.
 RS274/NGC Interpreter - Version 3

100

convert_motion

convert_arc

convert_arc_comp1

arc_data_comp_ijk

arc_data_comp_r

inverse_time_rate_arc

find_arc_length

convert_arc_comp2

arc_data_ijk

arc_data_r

inverse_time_rate_arc

find_arc_length

inverse_time_rate_arc2

find_arc_length

convert_arc2

arc_data_ijk

arc_data_r

inverse_time_rate_arc

find_arc_length

find_ends

convert_cycle

convert_cycle_xy (also convert_cycle_yz and convert_cycle zx)

GET_EXTERNAL_MOTION_CONTROL_MODE

cycle_traverse

convert_cycle_g81 (cycle_feed)

cycle_traverse

convert_cycle_g82 (cycle_feed)

cycle_traverse

convert_cycle_g83 (cycle_feed)

cycle_traverse

convert_cycle_g84 (cycle_feed)

convert_cycle_g85 (cycle_feed)

convert_cycle_g86 (cycle_feed)

cycle_traverse

convert_cycle_g87 (cycle_feed)

cycle_traverse

convert_cycle_g88 (cycle_feed)

convert_cycle_g89 (cycle_feed)

convert_probe

find_ends

convert_straight

convert_straight_comp1

convert_straight_comp2

find_ends

inverse_time_rate_straight

Figure 15. Interpreter Function Call Hierarchy

(from convert_motion)

This figure shows function calls from convert_motion to other Interpreter functions.

Convert_motion is shown called by convert_g in Figure 14. To save space, calls to cycle_feed

are shown in parentheses next to the caller, rather than indented below the caller.

Interpreter-do-it interface functions are shown in boldface, other Interpreter functions are

shown in ordinary typeface, and world-give-information functions are shown in ITALIC.
 RS274/NGC Interpreter - Version 3

101

D.8 Special Topics

This section focus on parts of the software that may be of particular interest to developers.

D.8.1 Interpreter World Model

The Interpreter maintains a model of its world when it runs. The data type of the model is a struct

named “setup_struct” defined in rs274ngc.hh The working model, a global variable declared in

rs274ngc.cc, is named _setup and is the only instance of a setup_struct. The model includes

around 100 attributes. Most of these are doubles or ints for things like “traverse_rate”, but one,

“parameters” is an array of 5600 doubles, another is the entire tool table, a third is a block (see

main

report_error

rs274ngc_error_text

rs274ngc_line_text

rs274ngc_stack_name

interpret_from_file

interpret_from_keyboard (see below)

report_error (see above)

rs274ngc_execute

rs274ngc_read

interpret_from_keyboard

report_error (see above)

rs274ngc_execute

rs274ngc_read

read_tool_file

designate_parameter_file

adjust_error_handling

rs274ngc_active_g_codes

rs274ngc_active_m_codes

rs274ngc_active_settings

rs274ngc_close

rs274ngc_exit

rs274ngc_file_name

rs274ngc_init

rs274ngc_line_length

rs274ngc_open

rs274ngc_sequence_number

Figure 16. SAI Driver Function Call Hierarchy

This shows the hierarchy of function calls from main in the SAI driver file, driver.cc, to:

1. other functions defined in driver.cc (shown in bold helvetica)

2. Interpreter_do_it functions defined in rs274ngc_pre.cc (shown in boldface).

3. Interpreter_give_information functions defined in rs274ngc_pre.cc

(shown in italic helvetica).

Interpreter-do-it interface functions are shown in boldface, other Interpreter functions are

shown in ordinary typeface, and world-give-information functions are shown in ITALIC.
 RS274/NGC Interpreter - Version 3

102

Appendix D.8.2), and a few others are substantial arrays.

The model is initialized when rs274ngc_init is called. Some of the initial values are hard-coded,

while others are obtained by calls (in rs274ngc_synch) to various world-give-information

functions.

While the Interpreter runs, the model is updated constantly. Most of the updating is done

assuming that canonical machining function calls have had their intended effects. Updating after

probing is done by calls to world-give-information functions.

D.8.2 Block Model

One item in the _setup model is a block struct. The block struct is defined in rs274ngc.hh and has

the attributes listed in Table 14. The rotary axis attributes are conditional; for example, b_number

and b_flag are not part of the struct unless the -DBB flag is used in compiling. Some letters (the

ones for which negative values are OK) have two attributes: a flag and a number. Other letters (the

ones for which negative values are not OK) have only a number.

Information from a line of code is put into the block when the line is read. When an

rs274ngc_execute function call is made, it is the block that is executed. The block is re-initialized

each time a line of code is read. The letters that have flags are initialized by setting the flag to

OFF. The letters that do not have flags are initialized by setting the number to -1.

The g_modes array in the block keeps track of which G modal groups are used on a line of code.

The values in the g_modes array are initialized to -1 before each line of NC code is read. When a

G-code is first read, the G number is multiplied by ten (to make an integer). That number is used

as an index into the _gees array (defined in rs274ngc.cc). The value at that index is the modal

group number for the G code (call it n). The G number is then inserted as the value at the nth

index of the g_modes array. When reading a line is complete, the g_modes array contains a record

of which G codes are to be executed.

The g_modes array also make it easy to check that at most one member of each G modal group is

used on a line of code; when a G code is read, just check that the g_modes value for the modal

group of the G code is -1; if not, another G code from the same group was previously read from

the same line of NC code.

The m_modes array in the block is handled similarly, the main difference being that M codes are

all integers, so they do not need to be multiplied by ten to get an integer. Thus, the _ems array,

which serves the same function with respect to M codes that _gees serves for G codes, is a tenth

the size of the _gees array.
 RS274/NGC Interpreter - Version 3

103

D.8.3 Expression Evaluation

The expression evaluation software is a recursive descent parser that evaluates as it parses. The

function call hierarchy is shown in Figure 13. This software is a coherent package that could be

copied out of the rs274ngc.cc file and used for other purposes. The read_real_expression function

can handle any number of levels of precedence.

D.8.4 Parameter Buffering

As discussed in Section 3.3.3, parameter values on a line of RS274/NGC code are all evaluated

before any parameters are reset. This is often called “parallel” setting. It is implemented by having

a parameter buffer (in the _setup model). When a line of code is read, any parameter values on the

line are taken from the parameters array, and any parameter settings are recorded in the parameter

buffer, not by changing the parameters array. If the line is executed, the parameters in the

attribute name data type attribute name data type

a_flag ON_OFF l_number int

a_number double line_number int

b_flag ON_OFF motion_to_be int

b_number double m_count int

c_flag ON_OFF m_modes array of 10 ints

c_number double p_number double

comment array of 256 chars q_number double

d_number int r_flag ON_OFF

f_number double r_number double

g_modes array of 14 ints s_number double

h_number int t_number int

i_flag ON_OFF x_flag ON_OFF

i_number double x_number double

j_flag ON_OFF y_flag ON_OFF

j_number double y_number double

k_flag ON_OFF z_flag ON_OFF

k_number double z_number double

Table 14. Block Attributes
 RS274/NGC Interpreter - Version 3

104

parameters array are reset according to the settings in the parameter buffer. This has no other

effect on execution because parameters are not used during execution.

A side effect of having the parameter buffer is that it ensures that the parameters in the _setup

model will not change while a line of code is being read. Nothing else in the model changes

during reading, so with the buffer, if there is an error during reading, nothing needs to be done to

recover state and continue interpretation. In previous interpreter versions, there was no parameter

buffer, parameters changed during reading, and it was not safe to continue interpretation after an

error during reading.
 RS274/NGC Interpreter - Version 3

105

Appendix E. Production Rules for theRS274/NGC Language

The following is a production rule definition of what combinations of symbols form a valid line of

RS274/NGC code. Developers, researchers, and NC programmers and machine operators with

computer science backgrounds may find this section useful. NC programmers and machine

operators without computer science backgrounds and SAI installers will probably not find it

useful.

The term “line” is at the top of the production hierarchy. The productions are arranged

alphabetically to make connections easy to trace.

The productions are intended to be unambiguous. That is, no permissible line of code can be

interpreted more than one way. To make the productions below entirely unambiguous, it is

implicit that if a string of characters that can meet the requirements of an ordinary comment also

can be interpreted as a message, that string is a message and not an ordinary comment.

The term comment_character is used in the productions but not defined there. A comment

character is any printable character plus space and tab, except for a left parenthesis or right

parenthesis. This implies comments cannot be nested.

It is implicit in the production rules that, except inside parentheses, space and tab characters may

be ignored, or have been removed by pre-processing.

These production rules do not include constraints implied by the semantics of the Interpreter.

Most of the constraints are in terms of combinations of words (as defined below). Many lines of

code that are readable under these production rules will not be executable because they violate

constraints. Any constraint violation will be detected by the Interpreter and will result in an error

message. The error messages are included in Appendix A.

In the productions, a parameter_index is defined as a synonym for real_value. The constraint on a

parameter_index is that it must be an integer between 1 and 5399 (inclusive).

E.1 Production Language

The symbols in the productions are mostly standard syntax notation. Meanings of the symbols

follow.

= The symbol on the left of the equal sign is equivalent to the expression on the right

+ followed by

| or

. end of production (a production may have several lines)

[ ] zero or one of the expression inside square brackets may occur

{ } zero to many of the expression inside curly braces may occur

( ) exactly one of the expression inside parentheses must occur

E.2 Productions

Any term in this subsection that is used on the right of an equal sign but is not defined in this

subsection (i.e., does not appear on the left in any definition) is defined in the next subsection in

terms of characters.
 RS274/NGC Interpreter - Version 3

106

arc_tangent_combo = arc_tangent + expression + divided_by + expression .

binary_operation = binary_operation1 | binary_operation2 | binary_operation3 .

binary_operation1 = power .

binary_operation2 = divided_by | modulo | times .

binary_operation3 = and | exclusive_or | minus | non_exclusive_or | plus .

comment = message | ordinary_comment .

comment_character = see explanation above .

digit = zero | one | two | three | four | five | six | seven | eight | nine .

expression = left_bracket + real_value + { binary_operation + real_value } + right_bracket .

letter_a = big_a | little_a .

letter_b = big_b | little_b .

letter_c = big_c | little_c .

letter_d = big_d | little_d .

letter_f = big_f | little_f .

letter_g = big_g | little_g .

letter_h = big_h | little_h .

letter_i = big_i | little_i .

letter_j = big_j | little_j .

letter_k = big_k | little_k .

letter_l = big_l | little_l .

letter_m = big_m | little_m .

letter_n = big_n | little_n .

letter_p = big_p | little_p .

letter_q = big_q | little_q .

letter_r = big_r | little_r .

letter_s = big_s | little_s .

letter_t = big_t | little_t .

letter_x = big_x | little_x .

letter_y = big_y | little_y .

letter_z = big_z | little_z .

line = [block_delete] + [line_number] + {segment} + end_of_line .

line_number = letter_n + digit + [digit] + [digit] + [digit] + [digit] .

message = left_parenthesis + {white_space} + letter_m + {white_space} + letter_s +

{white_space} + letter_g + {white_space} + comma + {comment_character} +

right_parenthesis .

mid_line_letter = letter_a | letter_b | letter_c| letter_d | letter_f | letter_g | letter_h | letter_i

| letter_j | letter_k | letter_l | letter_m | letter_p | letter_q | letter_r | letter_s | letter_t

| letter_x | letter_y | letter_z .

mid_line_word = mid_line_letter + real_value .

ordinary_comment = left_parenthesis + {comment_character} + right_parenthesis .

ordinary_unary_combo = ordinary_unary_operation + expression .

ordinary_unary_operation =

absolute_value | arc_cosine | arc_sine | cosine | e_raised_to |

fix_down | fix_up | natural_log_of | round | sine | square_root | tangent .

parameter_index = real_value .

parameter_setting = parameter_sign + parameter_index + equal_sign + real_value .

parameter_value = parameter_sign + parameter_index .
 RS274/NGC Interpreter - Version 3

107

real_number =

[ plus | minus ] +

(( digit + { digit } + [decimal_point] + {digit}) | ( decimal_point + digit + {digit})) .

real_value = real_number | expression | parameter_value | unary_combo .

segment = mid_line_word | comment | parameter_setting .

unary_combo = ordinary_unary_combo | arc_tangent_combo .

white_space = space | tab .

E.3 Production Tokens in Terms of Characters

We have omitted the letters and digits in the list below, since they are all the obvious single

characters. For example, one is ‘1’, big_a is ‘A’, and little_a is ‘a’. The list should be used as if

these obvious items were included. Note that not every letter of the alphabet is included (E, O, U,

V, and W are omitted).

absolute_value = ‘abs’

and = ‘and’

arc_cosine = ‘acos’

arc_sine = ‘asin’

arc_tangent = ‘atan’

block_delete = ‘/’

cosine = ‘cos’

decimal_point = ‘.’

divided_by = ‘/’

equal_sign = ‘=’

exclusive_or = ‘xor’

e_raised_to = ‘exp’

end_of_line = ‘ ‘ (non-printable newline character)

fix_down = ‘fix’

fix_up = ‘fup’

left_bracket = ‘[‘

left_parenthesis = ‘(‘

minus = ‘-’

modulo = ‘mod’

natural_log_of = ‘ln’

non_exclusive_or = ‘or’

parameter_sign = ‘#’

plus = ‘+’

power = ‘**’

right_bracket = ‘]’

right_parenthesis = ‘)’

round = ‘round’

sine = ‘sin’

space = ‘ ‘ (non-printable space character)

square_root = ‘sqrt’

tab = ‘ ‘ (non-printable tab character)

tangent = ‘tan’

times = ‘*’
 RS274/NGC Interpreter - Version 3

108

INDEX

Symbols

- 18

# 17, 18

% 12

* 18

** 18

+ 18

/ 18

_ems array 102

_gees array 102

_setup 101

A

A word 16

ABS 18

absolute value 18

ACOS 18

addition 18

AND 18

arc 23

center format 24

circular 7

elliptical 52

helical 7

radius format 23

arc cosine 18

arc sine 18

arc tangent 18

ARC_FEED 51

ASIN 18

ATAN 18

axis clamp 45

axis offsets 37

B

B word 16

back boring 34

binary operation 17

blank line 15

block delete 14

block delete switch 5, 9, 63

block of code 12

block structure 91, 102, 103

boring 34, 35, 36

bugs 72

C

C word 16

canned cycle 30, 86

canon.hh 66, 89

CANON_AXIS 58

CANON_COMP_SIDE 61

CANON_DIRECTION 55

CANON_FEED_REFERENCE 49

CANON_MOTION_MODE 50

CANON_PLANE 47

canon_pre.cc 66, 89

CANON_SPEED_FEED_MODE 51

CANON_UNITS 48

canonical machining functions 42, 88

case 15

centimeters 46

CHANGE_TOOL 57

CLAMP_AXIS 58

COMMENT 59

comment 18

compiling 65

continuous mode 8, 30, 50

controlled point 6

coolant

flood 5, 39, 45, 59

mist 5, 39, 45, 60

off 38

through-tool 45

coordinate system 14, 25, 46

offsets 36

coordinated linear motion 6

COS 18

cosine 18

current position 8

cutter radius compensation 61, 73–74

algorithm for first move 82

code 77, 79

errors 80

first move 76, 82

material edge contour 75

nominal path contour 78

programming instructions 75
 RS274/NGC Interpreter - Version 3

109

Z-axis motion 74

cycle start button 12, 38

D

D word 16

DAA 66

DALL_AXES 66

DAXIS_ERROR 66

DBB 66

DCC 66

degrees 6, 8, 18

DISABLE_FEED_OVERRIDE 59

DISABLE_SPEED_OVERRIDE 59

distance mode

absolute 36

incremental 36

division 18

documentation

source code 90

drilling 32, 33

driver.cc 66, 89

DWELL 52

dwell 7, 16, 25, 52

E

ELLIPSE_FEED 52

elliptical arc 45

EMC 1

ENABLE_FEED_OVERRIDE 59

ENABLE_SPEED_OVERRIDE 59

END_CANON 47

error condition 46

error handling 70

automatic generation of software 71

macros 71

exact path mode 8, 30, 50

exact stop mode 8, 30, 50

EXP 18

expression 17, 85

evaluation 103

F

F word 16, 37, 40

feed override switch 5, 8, 9, 33, 39, 40, 46, 49, 59

feed rate 7, 8, 40, 48

feed rate mode

inverse time 37

units per minute 37

feed reference 45

file

input 12, 62, 65, 91

output 43, 62, 65

parameter 12, 62

source code 66, 71, 89

tool 9, 62

FIX 18

flood coolant 7, 59

FLOOD_OFF 59

FLOOD_ON 59

FUP 18

G

G code 16, 21

g_modes 102

G0 23

G1 23, 38

G2 23

G3 23

G4 25

G10 14, 25

G17 25, 38

G18 25

G19 25

G20 26

G21 26

G28 26

G30 26

G38.2 26

G40 28, 38, 75

G41 29, 75

G42 29, 75

G43 29

G49 29

G53 14, 29

G54 14, 29, 38

G55 14, 29

G56 14, 29

G57 14, 29

G58 14, 29

G59 14, 30

G59.1 14, 30

G59.2 14, 30
 RS274/NGC Interpreter - Version 3

110

G59.3 14, 30

G61 30

G61.1 30

G64 30

G80 30

G81 32

G82 33

G83 33

G84 33

G85 34

G86 34

G87 34

G88 35

G89 36

G90 36, 38

G91 36

G92 14, 36

G92.1 14, 36

G92.2 14, 36, 38

G92.3 14, 36

G93 37

G94 37, 38

G98 37

G99 37

GET_EXTERNAL_ functions

ANGLE_UNIT_FACTOR 93

FEED_RATE 93

FLOOD 93

LENGTH_UNIT_FACTOR 93

LENGTH_UNIT_TYPE 93

MIST 93

MOTION_CONTROL_MODE 94

ORIGIN functions 94

PARAMETER_FILE_NAME 94

PLANE 94

POSITION functions 94

PROBE_POSITION functions 94

PROBE_VALUE 94

QUEUE_EMPTY 94

SPEED 94

SPINDLE 94

TOOL_LENGTH_OFFSET 95

TOOL_MAX 95

TOOL_SLOT 95

TOOL_TABLE 95

TRAVERSE_RATE 95

gouging 82

H

H word 16

home position 26

I

I word 16

inches 7, 26, 46

INIT_CANON 47

Interpreter

execute 91

interfaces 88

read 91

software 88

speed 68

Interpreter-do-it functions 88, 91

Interpreter-give-information functions 88, 92

inverse time 37

J

J word 16

jog 4

K

K word 16

keyboard input 63

L

L word 16

length units 26

line number 14, 15, 16

line of code 12, 14, 105

linear axes 4, 6

LN 18
 RS274/NGC Interpreter - Version 3

111

M

M code 16, 38

m_modes 102

M0 38

M1 38

M2 12, 38, 71

M3 38, 39

M4 39

M5 38, 39

M6 39

M7 39

M8 39

M9 38, 39

M30 12, 38, 71

M48 38, 39

M49 39

M60 38

material edge contour 75

MDI 3, 62, 63, 65

mechanical component 4, 12, 45

MESSAGE 60

message 19

message display 5, 19, 60

millimeters 7, 26, 46

mist coolant 7, 60

MIST_OFF 60

MIST_ON 60

MOD 18

modal command 19

modal group 20

mode 20

distance 30, 36

feed rate 7, 37

feed reference 49, 52, 53, 54

input 3, 62

path control 20, 30, 50, 94

retract 31, 37

modulus 18

multiplication 18

N

nominal path contour 78

number 17

O

optional program stop command M1 9, 38

optional program stop switch 5, 9, 38, 61

OPTIONAL_PROGRAM_STOP 9, 61

OR 18

order 19

order of execution 41

ORIENT_SPINDLE 55

P

P word 16

pallet shuttle 5, 8, 38

PALLET_SHUTTLE 60

parameter 12

parameter buffer 103

parameter file 12, 13, 62

parameter setting 18

parameter value 17

peck drilling 33

power 18

probe 54, 60

production rule 105

program 12

end 12

sample 84

start 12

PROGRAM_END 61

PROGRAM_STOP 61

Q

Q word 16

quit 63

R

R word 16

real value 17

reaming 34

repeat

word 19

rotational axes 5, 6

ROUND 18

round down 18

round up 18

RS274/NGC language 2, 12, 105

RS274-D 1

rs274ngc.hh 66, 89

rs274ngc_active_g_codes 92

rs274ngc_active_m_codes 92
 RS274/NGC Interpreter - Version 3

112

rs274ngc_active_settings 92

rs274ngc_close 92

RS274NGC_ENDFILE 71

rs274ngc_error_text 93

rs274ngc_errors.cc 66, 89

rs274ngc_execute 92

RS274NGC_EXECUTE_FINISH 70

RS274NGC_EXIT 71

rs274ngc_exit 92

rs274ngc_file_name 93

rs274ngc_init 92

rs274ngc_line_length 93

rs274ngc_line_text 93

rs274ngc_load_tool_table 92

RS274NGC_OK 70

rs274ngc_open 92

rs274ngc_pre.cc 66, 89

rs274ngc_read 92

rs274ngc_reset 92

rs274ngc_restore_parameters 92

rs274ngc_return.hh 66, 89

rs274ngc_save_parameters 92

rs274ngc_sequence_number 93

rs274ngc_stack_name 93

rs274ngc_synch 92

S

S word 16, 40

SAI 1, 62

block delete switch 63

error handling options 63, 65

file input 65

file output 65

installing 65

keyboard input 63

Makefile 67

parameter file 63

tool file 63

select tool 40

SELECT_PLANE 47

SELECT_TOOL 58

selected plane 8, 25

SET_CUTTER_RADIUS_COMPENSATION 61

SET_FEED_RATE 48

SET_FEED_REFERENCE 49

SET_MOTION_CONTROL_MODE 50

SET_ORIGIN_OFFSETS 48

SET_SPINDLE_SPEED 55

SET_TRAVERSE_RATE 48

SIN 18

sine 18

source code 66, 89

space 15

speed override switch 5, 8, 9, 33, 39, 40, 46, 59

spindle 5

force 56, 57

speed 40

torque 56, 57

spindle speed 8

SPINDLE_RETRACT 56

SPINDLE_RETRACT_TRAVERSE 56

SQRT 18

square root 18

Stand-Alone Interpreter 62

start

spindle 39

START_CUTTER_RADIUS_COMP. 61

START_SPEED_FEED_SYNCH 50

START_SPINDLE_CLOCKWISE 56

START_SPINDLE_COUNTERCLOCKWISE 56

STOP 54

stop

program 38

spindle 38, 39

STOP_CUTTER_RADIUS_COMP. 61

STOP_SPEED_FEED_SYNCH 51

STOP_SPINDLE_TURNING 56

straight probe 26

STRAIGHT_FEED 54

STRAIGHT_PROBE 54

STRAIGHT_TRAVERSE 48

subtraction 18

switch

block delete 5, 9, 63

feed override 5, 8, 9, 33, 39, 40, 46, 49, 59

optional program stop 5, 9, 38, 61

speed override 5, 8, 9, 33, 39, 40, 46, 59
 RS274/NGC Interpreter - Version 3

113

T

T word 16, 40

tab 15

TAN 18

tangent 18

tapping 33

THROUGH_TOOL_OFF 60

THROUGH_TOOL_ON 60

tool carousel 5, 8

tool change 5, 8, 57

tool file 9, 62

tool length offset 58

tool select 58

traverse 23

TURN_PROBE_OFF 60

TURN_PROBE_ON 60

U

unary operation 18

UNCLAMP_AXIS 61

Units 46

USE_LENGTH_UNITS 48

USE_NO_SPINDLE_FORCE 56

USE_NO_SPINDLE_TORQUE 56

USE_SPINDLE_FORCE 57

USE_SPINDLE_TORQUE 57

USE_TOOL_LENGTH_OFFSET 58

W

word 15

world model 3, 74, 75, 92, 101

world-give-information functions 88, 93

X

X word 16

XOR 18

Y

Y word 16

Z

Z word 16