D.Electron CNC Z32 Florenz Series Instrucciones de funcionamiento

D. ELECTRON

Since 1977 Hi - Tech

for the Machine - Tool

CNC

Z32

Programming guide (Lathes)

Document M335

C2 – 20.02.08

Read thoroughly before installation

Contains important information on:

•programming

This manual contains information exclusively devoted to the user of D.Electron products to allow a correct usage of delivered

devices. No part of this manual can be duplicated or delivered to third parties for an usage not corresponding to that indicated.

All information here contained have been accurately checked to be exact and reliable, but D.Electron doesn’t assume any

responsibility for possible inaccuracies. D.Electron reserves the right to make all modifications necessary to improve the

performance and reliability of its products.

D.Electron - Via R. Giuliani 140 - 50141 Firenze ITALY Internet: www.delectron.it

Tel ++39 - 055 - 416927 Fax ++39 - 055 - 434220 email [email protected]

CNC Z32 - Programming Guide (LATHES)

CONTENTS

1. INTRODUCTION....................................................................................................................................................1

2. BASE PROGRAMMING.......................................................................................................................................2

2.1 INTRODUCTION.................................................................................................................................................... 2

2.1.1 Machine behavior at reset....................................................................................................................... 2

2.1.2 Line number.............................................................................................................................................. 3

2.1.3 The standard ISO line.............................................................................................................................. 3

2.1.4 Comment lines.......................................................................................................................................... 4

2.1.5 G functions (modals and with stop)....................................................................................................... 4

1.1. F(FEED)PARAMETER AND FEED MANAGEMENT (G93 G94 G95).................................................................... 5

2.2 SPARAMETER AND SPEED MANAGEMENT (G96 G97)...................................................................................... 5

2.3 MFUNCTIONS..................................................................................................................................................... 6

2.4 AUXILIARY FUNCTIONS MA, MB, MC................................................................................................................. 7

2.5 END OF PROGRAM AND END OF SUBPROGRAM (M2 G26)................................................................................. 7

2.6 FUNCTIONS FOR ORIGINS RECALL (WORKPIECE COORDINATE SYSTEM)........................................................... 8

2.6.1 Setup of workpiece coordinates in the part-program.......................................................................... 8

2.7 TPARAMETER AND TOOL CHANGE ................................................................................................................... 10

2.8 TOOL CORRECTIONS:LENGTH (LX AND LZ) AND RADIUS (R) ......................................................................... 11

2.8.1 Position of the theoretical tool tip......................................................................................................... 11

2.9 TOOL PARAMETERS MODIFICATION (DLX, DLZ, DDR)................................................................................... 13

2.10 CANCELLATION AND SUSPENSION OF ORIGINS AND LENGTHS (G53 G54 G45)............................................. 14

2.11 CONTOURING PLANE......................................................................................................................................... 15

2.12 MOVEMENT PROGRAMMING (G0 G1 G2 G3).................................................................................................. 16

2.12.1 Rapid movement (G0)........................................................................................................................... 17

2.12.2 Linear interpolation (G1)....................................................................................................................... 18

2.12.3 Circular interpolation (G2 – G3)........................................................................................................... 19

2.12.4 Helical interpolation (G12 – G13)........................................................................................................ 22

2.13 INCREMENTAL COORDINATES PROGRAMMING (G90 G91).............................................................................. 23

2.14 MIRRORING,ROTATION,TRANSLATION,SCALE FACTOR.................................................................................. 24

2.14.1 Mirroring on the working plane (G56 – G55)...................................................................................... 24

2.14.2 Machining rotation (IR JR QR)............................................................................................................. 26

2.14.3 Machining translation (DA DB)............................................................................................................. 27

2.14.4 Scale factor............................................................................................................................................. 28

2.14.5 Other correction parameters................................................................................................................. 28

2.15 OTHER FUNCTIONS........................................................................................................................................... 29

2.15.1 Dwell (G4 TT..)....................................................................................................................................... 29

2.15.2 Axes change (G16)................................................................................................................................29

2.15.3 Alive axes management (G28, G29)................................................................................................... 30

2.15.4 Suspending and resuming Tool change (G38, G39)........................................................................ 31

2.15.5 Mounted tool reading (G104) ............................................................................................................... 31

2.15.6 Real positions reading (G105) ............................................................................................................. 31

2.15.7 Radial programming (G106)................................................................................................................. 31

2.15.8 Diametrical programming (G107) ........................................................................................................ 32

2.15.9 Axis movement with alarm CNxx12 (G119)....................................................................................... 32

2.15.10 Working field limits (G123).................................................................................................................... 32

3. DIRECT PROGRAMMING OF PROFILE......................................................................................................... 34

4. TOOL RADIUS CORRECTION.........................................................................................................................41

4.1 VECTORIAL COMPENSATION OF TOOL RADIUS ................................................................................................. 42

4.2 PROFILE APPROACH (G41/G42) AND PROFILE RETRACT (G40)..................................................................... 44

4.3 NULL OR NEGATIVE RADIUS.............................................................................................................................. 47

4.4 CONNECTING RADIUS ON EXTERNAL EDGES (G109S, G109T)...................................................................... 47

CNC Z32 - Programming Guide (LATHES)

4.5 INCOMPATIBLE PROFILE ERROR...............................................................................................................48

4.6 DISPLAYED POSITIONS AND RADIUS CORRECTION...........................................................................................48

4.7 EXAMPLE OF A PROFILE WITH RADIUS CORRECTION........................................................................................49

4.8 ALLOWANCE MANAGEMENT ..............................................................................................................................50

5. PARAMETRIC PROGRAMMING......................................................................................................................51

5.1 PARAMETER MANAGEMENT ..............................................................................................................................51

5.1.1 Parameter assignment...........................................................................................................................53

5.1.2 Parameter assignment through a formula..........................................................................................53

5.1.3 Axis movement programming with parameters..................................................................................54

5.1.4 System parameters programming........................................................................................................54

5.1.5 Axes programming through parameters AA, AB, AC........................................................................55

5.2 PROGRAMMING WITH “ADVANCED LINES”(!... !)............................................................................................56

5.2.1 Assigning values to parameters and computing expressions..........................................................56

5.2.2 Executing jumps without return (!GON..!)...........................................................................................57

5.2.3 Executing jumps with return (!GON..–..!)............................................................................................57

5.2.4 Executing conditioned jumps (!IF .. ; GON.. !)....................................................................................58

5.2.5 Controlling more than one condition on the same advanced line...................................................58

5.2.6 Structuring conditioned jumps..............................................................................................................59

5.2.7 Jump to a CMOS subprogram (! GOP.. !)...........................................................................................60

5.2.8 Jump to a CMOS subprogram with label (! GOP.. –N..!)..................................................................61

5.2.9 Jump to a CMOS subprogram with two labels (! GOP.. –N.. –N..!)................................................61

5.3 CONDITIONING BLOCKS OF PROGRAMS (--IF)..................................................................................................62

5.4 PROGRAM BLOCK REPETITION (--DO --LOOP)...............................................................................................64

5.4.1 Specifying the repetition number (LOOP {N})....................................................................................64

5.4.2 Repetition condition................................................................................................................................64

5.4.3 Anticipated exit condition --DO --LOOP (--EXIT DO)........................................................................65

5.5 WRITING CMOS PROGRAMS (--DEFINE P..).................................................................................................66

5.6 WRITING A TEMPORARY SUBPROGRAM SUBTEMP (--DEFINE S..)..............................................................66

6. Z32 FIXED CYCLES AND MACROS ...............................................................................................................68

6.1 Z32 FIXED CYCLES (G881 -G886).................................................................................................................68

6.1.1 G881: Normal drilling.............................................................................................................................71

6.1.2 G882: Deep drilling with chip breakage..............................................................................................71

6.1.3 G883: Deep drilling with chip extraction..............................................................................................72

6.1.4 G884: Tapping with compensating chuck...........................................................................................73

6.1.5 G885: Rigid tapping..............................................................................................................................73

6.1.6 G886: Reaming.......................................................................................................................................73

6.2 G901: MACRO FOR INTERNAL/EXTERNAL GROOVE MACHINING ......................................................................74

6.3 G902: MACRO FOR FACIAL GROOVES MACHINING...........................................................................................81

6.4 G903: MACRO FOR ROUGHING OF TRAPEZOIDAL SECTIONS,WITH PASSES ALONG Z....................................86

6.5 G904: MACRO FOR ROUGHING OF TRAPEZOIDAL SECTIONS,WITH PASSES ALONG X....................................88

6.6 THREADING .......................................................................................................................................................90

6.6.1 G33 function............................................................................................................................................90

6.6.2 Variable pitch threading (G34, G35)....................................................................................................92

6.6.3 G905: Threading macro.........................................................................................................................93

6.6.4 G906: Facial threadings........................................................................................................................98

6.7 G907: ROUGHING MACRO................................................................................................................................99

7. POLAR AXES.....................................................................................................................................................110

7.1 LIMITATIONS ON THE USAGE OF POLAR AXES.................................................................................................111

7.2 EXAMPLE.........................................................................................................................................................111

CNC Z32 - Programming Guide (LATHES)

1. INTRODUCTION

This manual contains a simplified description of Z32 control programming.

This document doesn’t contain a detailed description of all functionalities available, focusing only on the most

common and useful for the programming of lathe machines.

For a complete and detailed description of all functionalities available in the Z32 numerical control, please consult

“Programming Manual” M96.

This manual is valid for SIS xxx.xx version or later.

CNC Z32 - Programming Guide (LATHES)

2. BASE PROGRAMMING

2.1 Introduction

The base programming Z32 numerical controls follows the indications of ISO directions.

The program for a workpiece (or part-program) is a text file composed by a series of instructions stored in

sequential way.

The ISO lines are composed by a line number (not mandatory) and by a series of elementary instructions.

2.1.1 Machine behavior at reset

The machine behavior at reset is defined as the condition assumed by the machine when the pushbutton “Reset” is

pressed on the console. This behavior is important because it determines the machine functionality in its base

condition.

The reset condition is activated in the following ways:

- At CNC power up

- At the start of a program execution

- After pressing the pushbutton “Reset”

•Offset behavior at reset

The behavior of the zero offset at reset, is function of machine setup.

Depending on the setup, the following can happens:

- The machine sets its base origin (axis positions related to machine zero)

- The machine sets as active the origin (zero offset) number 1 on all continuous axes

- The machine leaves as active the last programmed offsets

Please consult the machine tool builder for further information.

•Parameter behavior at reset

All parameters used for the parametric programming of part-program are set to zero upon reset.

The following parameters behaves differently:

- Tool parameters. Upon reset all parameter values contained in the active tool description are

assigned. The active tool is the tool actually inserted on the spindle. If the tool parameters contain

technological parameters, like parameter F (feed) or parameter S (speed), these values are set at

reset with the corresponding values in the tool table. Parameters normally contained in the tool

description, are length L and radius R.

•Behavior of working plane at reset

As described later on, there are functions allowing to setup the working plane of the machine. This is done

through the G25 function.

At reset the machine switches to the configuration defined by setup made by the machine tool builder

For example, in a standard lathe the working plane is the Z-X plane.

Please consult the machine tool builder for further information.

•Axes behavior at reset (alive axes at reset)

Upon reset the axes can be alive or not. An alive axis is an axis whose position is controlled by the

numerical control. A non alive axis is an axis without control. A machine setup data defines the behavior at

reset. During part-program execution an axis can be switched alive or not alive through instructions G28

and G29.

- If the alive axes are defined as reset-transparent, the reset will not alter the actual map of alive

axes.

- If the alive axes are defined as non reset-transparent, the reset restores the map of alive axes

defined in the setup.

Please consult the machine tool builder for further information.

•All geometric transforms, translations, mirroring, rotations, scale factors, etc. are disabled at reset.

CNC Z32 - Programming Guide (LATHES)

•All functions and settings related to RTCP (rotating tool centre point) are disabled at reset.

•At reset, all high speed settings are restored with the corresponding parameters contained in the machine

setup. Please consult the machine tool builder for further information.

Warning: it is important to remember that at the beginning of a part-program execution, a reset

condition is forced. Thus the machine initiates the execution starting from the reset state, and every

modification to be made on this state must be expressly programmed in the part-program.

2.1.2 Line number

The line number is composed by the letter “N” followed by a number (also decimal). The line number programming

is not mandatory. As an example, all following syntaxes are equivalent:

G0 Z100

and

N10 G0Z100

Line number format: The line number can be an integer or decimal number, with the decimal position

indicated either with a point or a comma. It is possible to insert some space characters between the letter

N and the number. As an example, it is possible to write:

N100

N 100.2

N100,34

The only limitation is the total number of numeric characters before and after the decimal delimiter, which

cannot be more than 9 characters.

Line number as jump destination: The line number may be used as “jump destination” in the logic-

mathematic programming. For a description of this functionality, please consult this manual in the logic-

mathematic programming section.

2.1.3 The standard ISO line

After the optional line number N, the ISO line is composed by a sequence of elementary instructions. Each

instruction is composed by two parts:

- ADDRESS

- VALUE

The address is composed by alphabetic characters and specifies the type of operation desired.

The value, normally numeric, specifies the operation to be executed.

Between address and value, an arbitrary number of spaces can be inserted.

The same line may contain more than one couple address-value.

The followings are all valid ISO lines:

N10 G0 Z100

N20 G0 X 100 Z20

G0Z0X0Y0

Format of numeric values:

CNC Z32 - Programming Guide (LATHES)

- At least one number must be programmed (the zero value is programmed with one or more “0”

characters)

- The division between integer and decimal part may be indicated either with “.” (point) and with “,”

(comma).

All following sample programming are valid ISO lines:

X.1

X .1

X,1

X0,1

X 0.1

X00000,1000

- All numbers cannot have more than 9 significant digits before or after the decimal delimiter.

All following sample programming are valid ISO lines:

X123456789

X0.123456789

X0.0000123456789

X12345.6789

Invalid programming samples:

X1234567.12345

X12345.67890000

X1.00000001234

- A number cannot contain space characters.

2.1.4 Comment lines

A part-program may contain comment lines.

A comment is contained between parenthesis.

Example:

G0 Z100 (initial approach)

2.1.5 G functions (modals and with stop)

The G functions are preparatory functions responsible to prepare the CNC to interpret the following functions.

The number following the G letter identifies the particular function for which the Z32 must be prepared. The value

following the G letter must always be a numeric value (CANNOT be an expression result).

Only some G functions (i.e. only some numeric values) are interpreted and executed from Z32. If a not

implemented G function is programmed, Z32 issues the related alarm.

The functions are those contained in the ISO regulations, with some adaptations. In particular:

•The initial zero digits of G codes can be omitted (G0 is equivalent to G00)

•More than one G function can be programmed in the same block: in this case the G functions are

recognized and executed by the CNC as they are encountered in the programmed line: if contrasting

G functions are programmed, the last programmed G function remains active.

•Some particular G functions require additional data to complete their definition.

•MODAL functions are those G functions whose effect will be maintained also in the blocks following the

one where they were programmed: modal G functions are normally deactivated by other special G

functions.

•Some G functions require the machine STOP: the profile must be completely defined when they are

executed. In this case no contouring with open profile, or contouring with radius compensation can be

active.

CNC Z32 - Programming Guide (LATHES)

1.1.F (Feed) parameter and Feed management (G93 G94 G95)

The F parameter defines the feed velocity during machining and it is programmed writing the letter F followed by

the desired feed value (numeric value with a maximum of 9 significant digits).

•Programmed after

G94 it defines the F velocity in “units” per minute. Example:

With linear axes measured in millimeters, F100 means 100 mm/min.

With linear axes measured in inches, F100 means 100 in/min.

With round axes measured in degrees, F100 means 100 deg/min.

G94 is active upon reset and it is thus the normal mode if not otherwise specified.

•Programmed after G95 it defines the feed velocity as “units” per spindle round. “Units” can be millimeters,

inches or degrees, depending on the axis type.

•Programmed after

G93 it defines the velocity as the inverse of time (expressed in minutes) necessary to

execute the programmed movement. In this case the F value to be programmed is equal to the velocity

desired on the trajectory, divided by the length of the trajectory itself:

F = Velocity (mm/min or in/min) / Space (mm or inches)

2.2 S parameter and Speed management (G96 G97)

The S parameter defines the spindle rotational speed and is programmed writing the letter S followed by the

desired speed value (numeric value with a maximum of 9 significant digits). The S function doesn’t activate the

spindle rotation, activated through the auxiliary functions M3 or M4.

•Programmed after G97 it defines the spindle rotational speed in rpm.

G97 is active upon reset and it is thus the normal mode if not otherwise specified.

•Programmed after G96 it sets the mode “Constant cutting speed". This is a typical functionality of lathes:

the spindle rotational speed is computed in such a way that the cutting speed is equal to the programmed

S value (expressed in m/min), considering the tool distance from the rotation centre of the spindle.

Note on G96: In order to avoid excessive speed when the distance from spindle center is very small, aside

G96 the parameter MS is activated (programmable also before the S value) which sets the maximum spindle

rotational speed (in rpm) allowed. The active MS value is that present at the moment of last programmed S: if

the parameter MS is newly programmed, the limit doesn't change until a new programming of S value.

The tool may jump over the rotation centre: the speed is in every case determined by the absolute value of

the distance from spindle center, while the center crossing is limited by the programmed MS. It is possible to

program:

G96 S100 MS4000 M3

This programming imposes a cutting speed of 100 m/min.

With a maximum speed limit of 4000 rpm.

In lathe machinings, it is very common the combined usage of G96 and G95 functions.

Example:

G96 S100 MS4000 M3

G95 F0.3

cutting speed 100 m/min, maximum speed 4000 rpm, feed 0.3 mm/round

CNC Z32 - Programming Guide (LATHES)

2.3 M Functions

The M functions (miscellaneous) are mainly related to the machine tool behavior and their functionality is mostly

defined by the machine tool builder.

All M functions require a machine stop.

The ISO standards indicate the functionality of many M codes: only some M codes are decoded and managed by

the Z32, and only these codes will be discussed.

The numeric value (two integer digits) following the letter “M”, indicates the programmed M function. All leading

zeros can be omitted (G0 = G00).

ISO “M” codes

M0 - stop

It stops the program execution; program resuming trough Start pushbutton. This function also stops

spindle and coolants.

M1 – conditioned stop

Same behavior as M0, but M1 activity is conditioned by a dedicated logic input: for further details, please

consult the machine tool builder. This function also stops spindle and coolants.

M2 – End of program

Exits the control EXECUTION mode and terminates all automatic operations.

M3 – Spindle clockwise

Requests a clockwise rotation of the spindle, with the previously programmed S (speed).

M3 – Spindle counterclockwise

Requests a counterclockwise rotation of the spindle, with the previously programmed S (speed).

M5 – Spindle stop

Requests the spindle stop. It stops also the coolants.

M6 – Tool change

Requests the mounting of last programmed T (in the same or preceding blocks) on the spindle. It also

stops spindle and coolants. After the M6 execution, the NC takes into account the description of the tool

mounted on the spindle, updating accordingly all parameters.

M7 – coolant #1 delivery

Requests delivery of coolant #1.

M8 – coolant #2 delivery

Requests delivery of coolant #2.

M9 – Coolant stop

Requests stop of coolants delivery.

M19 – Spindle orientation

Requests the spindle orientation.

This function also stops spindle and coolants.

The machine tool builder can define other M functions for particular usage and purposes of the machine. For

further details, please consult the machine tool builder.

Special “M” codes

A category of M functions is defined as “Special” M. Unlike normal M functions, interpreted exclusively by the

machine PLC, every special M code is associated with a service part-program. A typical example of special M is

the M6 for tool changing.

The definition and programming of subprograms associated with special M codes, are activities reserved to the

machine tool builder.

During the execution of the subprogram associated to a special M, the progressive block number counting is

suspended (in block search the special M appears as a single block, not searchable in an intermediate point).

The subprogram associated to the special M may be executed as a single block.

Tabla de contenidos

Manuales populares de Sistema de control de otras marcas

Pentair Pool Products

Pentair Pool Products Compool Manual de usuario

ComfortNET

ComfortNET CTK04 Manual de usuario

Fireye

Fireye InSight II 95DSS3 Manual de usuario

CAME

CAME G3000 Manual de usuario

Idemia

Idemia MorphoAccess VP MD Manual de usuario

Axis

Axis P1445-LE-3 Manual de usuario

HEIDENHAIN

HEIDENHAIN TNC 150 B Manual de usuario

CNC-Step

CNC-Step High-Z T-Series Manual de usuario

Doosan

Doosan DVF Series Manual de usuario

Honeywell

Honeywell KAP 140 Manual de usuario

Honeywell

Honeywell vk41 series Manual de usuario

AirBench

AirBench FPW Guía de instalación

Cypress

Cypress HHR-3160 Manual de usuario

CAME

CAME GLT40AOS Manual de usuario

Zonex

Zonex GEN II -VVT Guía del usuario

Altronics

Altronics K 9650 Manual de usuario

micro-trak

micro-trak RoadMaster Manual de usuario

micro-trak

micro-trak Calc-An-Acre II Manual de usuario