Mazatrol smart руководство пользователя

SAFETY PRECAUTIONS

Preface

Safety precautions relating to the CNC unit (in the remainder of this manual, referred to simply as the NC unit) that is provided in this machine are explained below. Not only the persons who create programs, but also those who operate the machine must thoroughly understand the contents of this manual to ensure safe operation of the machine.

Read all these safety precautions, even if your NC model does not have the corresponding functions or optional units and a part of the precautions do not apply.

Rule

1.This section contains the precautions to be observed as to the working methods and states usually expected. Of course, however, unexpected operations and/or unexpected working states may take place at the user site.

During daily operation of the machine, therefore, the user must pay extra careful attention to its own working safety as well as to observe the precautions described below.

2.Although this manual contains as great an amount of information as it can, since it is not rare for the user to perform the operations that overstep the manufacturer-assumed ones, not all of “what the user cannot perform” or “what the user must not perform” can be fully covered in this manual with all such operations taken into consideration beforehand.

It is to be understood, therefore, that functions not clearly written as “executable” are “inexecutable” functions.

3.The meanings of our safety precautions to DANGER, WARNING, and CAUTION are as follows:

: Failure to follow these instructions could result in loss of life.

DANGER

: Failure to observe these instructions could result in serious harm to a human

life or body.

WARNING

: Failure to observe these instructions could result in minor injuries or serious

machine damage.

CAUTION

SAFETY PRECAUTIONS

Basics

! After turning power on, keep hands away from the keys, buttons, or switches of the operating panel until an initial display has been made.

WARNING ! Before proceeding to the next operations, fully check that correct data has been entered and/or set. If the operator performs operations without being aware of data errors,

unexpected operation of the machine will result.

!Before machining workpieces, perform operational tests and make sure that the machine operates correctly. No workpieces must be machined without confirmation of normal operation. Closely check the accuracy of programs by executing override, single-block, and other functions or by operating the machine at no load. Also, fully utilize tool path check, Virtual Machining, and other functions, if provided.

!Make sure that the appropriate feed rate and rotational speed are designated for the particular machining requirements. Always understand that since the maximum usable feed rate and rotational speed are determined by the specifications of the tool to be used, those of the workpiece to be machined, and various other factors, actual capabilities differ from the machine specifications listed in this manual. If an inappropriate feed rate or rotational speed is designated, the workpiece or the tool may abruptly move out from the machine.

!Before executing correction functions, fully check that the direction and amount of correction are correct. Unexpected operation of the machine will result if a correction function is executed without its thorough understanding.

!Parameters are set to the optimum standard machining conditions prior to shipping of the machine from the factory. In principle, these settings should not be modified. If it becomes absolutely necessary to modify the settings, perform modifications only after thoroughly understanding the functions of the corresponding parameters. Modifications usually affect any program. Unexpected operation of the machine will result if the settings are modified without a thorough understanding.

Remarks on the cutting conditions recommended by the NC

! Before using the following cutting conditions:

—Cutting conditions suggested by the Machining Navigation Function

—Cutting conditions for tools that are suggested to be used by the Machining Navigation Function

Confirm that every necessary precaution in regards to safe machine setup has been taken – especially for workpiece fixturing/clamping and tool setup.

!Confirm that the machine door is securely closed before starting machining. Failure to confirm safe machine setup may result in serious injury or death.

SAFETY PRECAUTIONS

Programming

!During surface velocity hold control, as the current workpiece coordinates of the surface velocity hold control axes approach zeroes, the spindle speed increases significantly. For the lathe, the workpiece may even come off if the chucking force decreases. Safety speed limits must therefore be observed when designating spindle speeds.

!Even after inch/metric system selection, the units of the programs, tool information, or parameters that have been registered until that time are not converted. Fully check these data units before operating the machine. If the machine is operated without checks being performed, even existing correct programs may cause the machine to operate differently from the way it did before.

!If a program is executed that includes the absolute data commands and relative data commands taken in the reverse of their original meaning, totally unexpected operation of the machine will result. Recheck the command scheme before executing programs.

!If an incorrect plane selection command is issued for a machine action such as arc interpolation or fixed-cycle machining, the tool may collide with the workpiece or part of the machine since the motions of the control axes assumed and those of actual ones will be interchanged. (This precaution applies only to NC units provided with EIA functions.)

!The mirror image, if made valid, changes subsequent machine actions significantly. Use the mirror image function only after thoroughly understanding the above. (This precaution applies only to NC units provided with EIA functions.)

!If machine coordinate system commands or reference position returning commands are issued with a correction function remaining made valid, correction may become invalid temporarily. If this is not thoroughly understood, the machine may appear as if it would operate against the expectations of the operator. Execute the above commands only after making the corresponding correction function invalid. (This precaution applies only to NC units provided with EIA functions.)

!The barrier function performs interference checks based on designated tool data. Enter the tool information that matches the tools to be actually used. Otherwise, the barrier function will not work correctly.

!The system of G-code and M-code commands differs, especially for turning, between the machines of INTEGREX e-Series and the other turning machines.

Issuance of the wrong G-code or M-code command results in totally non-intended machine operation. Thoroughly understand the system of G-code and M-code commands before using this system.

SAFETY PRECAUTIONS

!For the machines of INTEGREX e-Series, programmed coordinates can be rotated using an index unit of the MAZATROL program and a G68 command (coordinate rotate command) of the EIA program. However, for example, when the B-axis is rotated through 180 degrees around the Y-axis to implement machining with the turning spindle No. 2, the plus side of the X-axis in the programmed coordinate system faces downward and if the program is created ignoring this fact, the resulting movement of the tool to unexpected positions may incite collisions.

To create the program with the plus side of the X-axis oriented in an upward direction, use the mirror function of the WPC shift unit or the mirror imaging function of G-code command (G50.1, G51.1).

!After modifying the tool data specified in the program, be sure to perform the tool path check function, the Virtual Machining function, and other functions, and confirm that the program operates properly. The modification of tool data may cause even a field-proven machining program to change in operational status.

If the user operates the machine without being aware of any changes in program status, interference with the workpiece could arise from unexpected operation.

For example, if the cutting edge of the tool during the start of automatic operation is present inside the clearance-including blank (unmachined workpiece) specified in the common unit of the MAZATROL program, care is required since the tool will directly move from that position to the approach point because of no obstructions being judged to be present on this path.

For this reason, before starting automatic operation, make sure that the cutting edge of the tool during the start of automatic operation is present outside the clearance-including workpiece specified in the common unit of the MAZATROL program.

!If axis-by-axis independent positioning is selected and simultaneously rapid feed selected

for each axis, movements to the ending point will not usually become linear. Before using

these functions, therefore, make sure that no obstructions are present on the path.

CAUTION

!Before starting the machining operation, be sure to confirm all contents of the program obtained by conversion. Imperfections in the program could lead to machine damage and operator injury.

SAFETY PRECAUTIONS

Operations

!Single-block, feed hold, and override functions can be made invalid using system variables #3003 and #3004. Execution of this means the important modification that makes the corresponding operations invalid. Before using these variables, therefore, give thorough notification to related persons. Also, the operator must check the settings of the system variables before starting the above operations.

!If manual intervention during automatic operation, machine locking, the mirror image function, or other functions are executed, the workpiece coordinate systems will usually be shifted. When making machine restart after manual intervention, machine locking, the mirror image function, or other functions, consider the resulting amounts of shift and take the appropriate measures. If operation is restarted without any appropriate measures being taken, collision with the tool or workpiece may occur.

!Use the dry run function to check the machine for normal operation at no load. Since the feed rate at this time becomes a dry run rate different from the program-designated feed rate, the axes may move at a feed rate higher than the programmed value.

!After operation has been stopped temporarily and insertion, deletion, updating, or other commands executed for the active program, unexpected operation of the machine may result if that program is restarted. No such commands should, in principle, be issued for the active program.

!During manual operation, fully check the directions and speeds of axial movement.

!For a machine that requires manual homing, perform manual homing operations after turning power on. Since the software-controlled stroke limits will remain ineffective until manual homing is completed, the machine will not stop even if it oversteps the limit area. As a result, serious machine damage will result.

!Do not designate an incorrect pulse multiplier when performing manual pulse handle feed operations. If the multiplier is set to 1000 times and the handle operated inadvertently, axial movement will become faster than that expected.

BEFORE USING THE NC UNIT

Limited Warranty

The warranty of the manufacturer does not cover any trouble arising if the NC unit is used for its non-intended purpose. Take notice of this when operating the unit.

Examples of the trouble arising if the NC unit is used for its non-intended purpose are listed below.

1.Trouble associated with and caused by the use of any commercially available software products (including user-created ones)

2.Trouble associated with and caused by the use of any Windows operating systems

3.Trouble associated with and caused by the use of any commercially available computer equipment

Operating Environment

1.Ambient temperature

During machine operation: 0° to 50°C (32° to 122°F)

2.Relative humidity

During machine operation: 10 to 75% (without bedewing)

Note: As humidity increases, insulation deteriorates causing electrical component parts to deteriorate quickly.

Keeping the Backup Data

Note: Do not attempt to delete or modify the data stored in the following folder. Recovery Data Storage Folder: D:\MazakBackUp

Although this folder is not used when the NC unit is running normally, it contains important data that enables the prompt recovery of the machine if it fails.

If this data has been deleted or modified, the NC unit may require a long recovery time. Be sure not to modify or delete this data.

CONTENTS

1 CONTROLLED AXES

1-1 Coordinate Words and Controlled Axes

Under standard specifications, there are three-dimensional controlled axes. With an added feature and a special option, the machine can control up to a maximum of six axes, including the three fundamental axes. The direction of machining can be designated using a predetermined coordinate word consisting of an alphabetic character.

MEP001

Table turning direction

MEP002

1 CONTROLLED AXES

— NOTE —

UNITS OF PROGRAM DATA INPUT 2

2 UNITS OF PROGRAM DATA INPUT

2-1 Units of Program Data Input

The movements on coordinate axes are to be commanded in the MDI mode or machining program. The movement data are expressed in millimeters, inches or degrees.

2-2 Units of Data Setting

Various data commonly used for control axes, such as offsetting data, must be set for the machine to perform an operation as desired.

The units of data setting and those of program data input are listed below.

Note 1: Inch/metric selection can be freely made using either bit 4 of parameter F91 (“0” for metric, “1” for inches; validated through power-off and -on) or G-code commands (G20, G21).

Selection using the G-code commands is valid only for program data input.

Variables and offsetting data (such as tool offsetting data) should therefore be set beforehand using the appropriate unit (inch or metric) for the particular machining requirements.

Note 2: Metric data and inch data cannot be used at the same time.

2-3 Ten-Fold Program Data

Using a predetermined parameter, machining program data can be processed as set in units of one micron. There may be cases that a machining program which has been set in units of one micron is to be used with a numerical control unit based on 0.1 micron increments. In such cases, use of this parameter allows the machine to perform the required machining operations without rewriting the program.

Use bit 0 of user parameter F91 for this purpose.

All types of coordinate data (axis movement data) not provided with the decimal point will be multiplied by a factor of 10. This does not apply, indeed, to preset tool-offsetting data designated with addresses H and D.

2 UNITS OF PROGRAM DATA INPUT

— NOTE —

3 DATA FORMATS

3-1 Tape Codes

This numerical control unit (in the remainder of this manual, referred to as the NC unit) uses command information that consists of letters of the alphabet (A, B, C …. Z), numerics (0, 1, 2 ….

9), and signs (+, –, /, and so on). These alphanumerics and signs are referred to collectively as characters. On paper tape, these characters are represented as a combination of a maximum of eight punched holes.

Such a representation is referred to as a code.

The NC unit uses either the EIA codes (RS-244-A) or the ISO codes (R-840).

Note 1: Codes not included in the tape codes shown in Fig. 3-1 will result in an error when they are read.

Note 2: Of all codes specified as the ISO codes but not specified as the EIA codes, only the following codes can be designated using the data I/O (Tape) parameters TAP9 to

TAP14:

[ Bracket Open

] Bracket Close

# Sharp

Asterisk = Equal sign

:Colon

However, you cannot designate codes that overlap existing ones or that result in parity error.

Note 3: EIA/ISO code identification is made automatically according to the first EOB/LF code appearing after the NC unit has been reset. (EOB: End Of Block, LF: Line Feed)

1.Significant information area (LABEL SKIP function)

During tape-based automatic operation, data storage into the memory, or data searching, the NC unit will ignore the entire information up to the first EOB code (;) in the tape when the unit is turned on or reset. That is, significant information in a tape refers to the information contained in the interval from the time a character or numeric code appears, following the first EOB code (;) after the NC unit has been reset, until a reset command is given.

2.Control Out, Control In

The entire information in the area from Control Out “(” to Control In “)” will be ignored in regard to machine control, while they will surely be displayed on the data display unit. Thus, this area can be used to contain information, such as the name and number of the command tape, that is not directly related to control.

During tape storage, however, the information in this area will also be stored. The NC unit will enter the Control In status when power is turned on.

Operator information is printed out.

3.EOR code (%)

In general, the EOR (End Of Record) code is punched at both ends of a tape and has the following functions:

—To stop rewinding (only when a rewinding device is provided)

—To start rewinding during tape data search (only when a rewinding device is provided)

—To terminate the storage of tape data.

DATA FORMATS 3

4.Tape creation method for tape operation (Only when a rewinding device is used)

The two meters of dummy at both ends and the EOR (%) at the head are not required when a rewinding device is not used.

EIA/ISO identification is made automatically by detecting whether EOB or LF initially appears after the NC unit has been reset.

MEP006

Fig. 3-1 Tape codes

DATA FORMATS 3

Codes in section [1] will only be stored as tape data when they are present in a comment section, and ignored elsewhere in the significant information area.

Codes in section [2] are non-operative and will always be ignored (but undergo the parity-V check).

A dotted area indicates that the EIA Standard provides no corresponding codes.

3-2 Program Formats

A format predetermined for assigning control information to the NC unit is referred to as a program format. The program format used for our NC unit is word address format.

1.Words and addresses

A word is a set of characters arranged as shown below, and information is processed in words.

Word

Numeral

Alphabet (address)

Word configuration

The alphabetic character at the beginning of a word is referred to as an address, which defines the meaning of its succeeding numeric information.

Table 3-1 Type and format of words

3DATA FORMATS

1.Code O8 here indicates that program number can be set as an unsigned integer of eight digits following O, and for X+54, “+” indicates that the value can be signed (negative) and the two-digit number (54) indicates that the decimal point can be used and that five digits before and four after the decimal point are effective (5 + 4 = 9 digits are effective for a designation without decimal point).

2.The alpha sign (α) denotes additional axis address. +44 will be used when α is specified for rotational axis.

3.The number of digits in the words is checked by the maximum number of digits in the addresses.

4.When data with decimal point is used for address for which decimal input is not available, decimal figures will be ignored.

5.If the number of integral digits exceeds the specified format, an alarm will result.

6.If the number of decimal digits exceed the specified format, the excess will be rounded.

2.Blocks

A block, unit of instruction, contains a number of words which constitute information necessary for the NC machine to perform an operation. The end of each block must be indicated by an EOB (End Of Block) code.

3.Programs

A number of blocks form one program.

4.Program end

M02, M30, M99, M998, M999 or % is used as program end code.

3-3 Tape Data Storage Format

As with tape operation, tape data to be stored into the memory can be either of ISO or EIA code. The first EOB code read in after resetting is used by the NC unit for automatic identification of the code system ISO or EIA.

The area of tape data to be stored into the memeory is, if the NC unit has been reset, from the character immediately succeeding the first EOB code the EOR code, and in all other cases, from the current tape position to the EOR code. Usually, therefore, start tape data storage operation after resetting the NC unit.

3-4 Optional Block Skip

1.Function and purpose

Optional block skip is a function that selectively ignores that specific block within a machining program which begins with the slash code “/”.

Any block beginning with “/” will be ignored if the [BLOCK SKIP] menu function is set to ON, or will be executed if the menu function is set to OFF.

For example, if all blocks are to be executed for a type of parts but specific blocks are not to be executed for another type, then different parts can be machined using one and the same program that contains the “/” code at the beginning of the specific blocks.

DATA FORMATS 3

2.Operating notes

1.Blocks that have already been read into the pre-read buffer cannot be skipped.

2.This function is valid even during sequence number search.

3.During tape data storage (input) or output, all blocks, including those having a “/” code, are inor outputted, irrespective of the status of the [BLOCK SKIP] menu function.

3-5 Program Number, Sequence Number and Block Number: O, N

Program numbers, sequence numbers, and block numbers are used to monitor the execution status of a machining program or to call a machining program or a specific process within a machining program.

Program numbers are assigned to command blocks as required. A program number must be set using the letter O (address) and a numeric of a maximum of eight digits that follow O. Sequence numbers identify command blocks forming a machining program. A sequence number must be set using the letter N (address) and a numeric of a maximum of five digits that follow N. Block numbers are counted automatically within the NC unit, and reset to 0 each time a program number or a sequence number is read. These numbers will be counted up by one if the block to be read does not have an assigned program number or sequence number.

All blocks of a machining program, therefore, can be uniquely defined by combining program number, sequence number, and block number as shown in the table below.

3-6 Parity-H/V

One method of checking if the tape is correctly created is by parity checks. Parity checks are performed to check a tape for errors in punched codes, that is, for punching errors. There are two types of parity checks: parity-H and parity-V.

1.Parity-H check

Parity-H checks are intended to check the quantity of punched holes which form one character, and performed during tape operation, tape loading, and sequence-number searching.

A parity-H error occurs in the following cases:

—ISO Codes

If a code with an odd number of punched holes is present in the significant information area.

—EIA Codes

If a code with an even number of punched holes is present in the significant information area or if non-punched holes (sprockets only) are present after a significant code in one block.

Example 1: Parity-H error (for EIA codes)

This character leads to a Parity-H error.

One block

This non-punched character will result in a Parity-H error.

These non-punched characters will not result in a Parity-H error.

MEP007

If a parity-H error occurs, the tape will stop at the position next to the error code.

2.Parity-V check

Parity-V checks will be performed during tape operation, tape loading, or sequence-number searching, if parity-V check item on the PARAMETER display is set to ON. Parity-V during memory operation, however, will not be checked.

A parity-V error occurs in the following case:

If an odd number of codes are present in the significant information area from the first significant code in the vertical direction to the EOB code (;), that is, if an odd number of characters are present in one block.

In the event of a parity-V error, the tape stops at a code next to the EOB (;). Example 2: An example of parity-V error

1 2 3 4 5 6 7

This block leads to a Parity-V error.

MEP009

Note 1: During a parity-V check, some types of code are not counted as characters. See Fig. 3-1, “Tape codes” for further details.

Note 2: Space codes in the area from the first EOB code to the first address code or slash code “/” are not subjected to counting for parity-V check.

3 DATA FORMATS

Notes:

1.The codes marked with ▲ are selected in each group when the power is turned ON or executing reset for initializing modal.

2.The codes marked with » are able to be selected by a parameter as an initial modal which is to become valid when the power is turned ON or executing reset for initializing modal. Changeover of inch/metric system, however, can be made valid only by turning the power ON.

3.G-codes of group 00 are those which are not modal, and they are valid only for commanded blocks.

4.If a G-code not given in the G-code list is commanded, an alarm is displayed. And if a G- code without corresponding option is commanded, an alarm is displayed (808 MIS-SET G CODE).

5.If G-codes belong to different groups each other, any G-code can be commanded in the same block. The G-codes are then processed in order of increasing group number. If two or more G-codes belonging to the same group are commanded in the same block, a G-code commanded last is valid.

4 BUFFER REGISTERS

4-1 Input Buffer

1.Overview

During tape operation or RS-232C operation, when the preread buffer becomes empty, the contents of the input buffer will be immediately shifted into the pre-read buffer and, following this, if the memory capacity of the input buffer diminuishes to 248 × 4 characters or less, next data (up to 248 characters) will be preread from the tape and then stored into the input buffer.

The input buffer makes block-to-block connections smooth by eliminating any operational delays due to the tape-reading time of the tape reader.

These favorable results of prereading, however, will be obtained only if the execution time of the block is longer than the tape-reading time of the next block.

TEP010

2.Detailed description

—The memory capacity of the input buffer is 248 × 5 characters (including the EOB code).

—The contents of the input buffer register are updated in 248-character units.

—Only the significant codes in the significant information area are read into the buffer.

—Codes, including “(” and “)”, that exist between Control Out and Control In, are read into the input buffer. Even if optional block skip is valid, codes from / to EOB will also be read into the input buffer.

—The contents of the buffer are cleared by a reset command.

4-2 Preread Buffer

1.Overview

During automatic operation, one block of data is usually preread to ensure smooth analysis of the program. During tool radius compensation, however, maximal five blocks of data are preread to calculate crossing point or to check the interference.

In the high-speed machining mode (G05P2), moreover, up to 8 blocks of data are preread, and in the mode of high-speed smoothing control up to 24 blocks of data are stored with the currently executed block in the middle (i. e. 12 blocks being preread).

2.Detailed description

—One block of data is stored into the prepared buffer.

—Only the significant codes in the significant information area are read into the pre-read buffer.

—Codes existing between Control Out and Control In are not read into the pre-read buffer. If optional block skip is valid, codes from / to EOB will not also be read into the pre-read buffer.

—The contents of the buffer are cleared by a reset command.

—If the single block operation mode is selected during continuous operation, processing will stop after pre-reading the next block data.

5 POSITION PROGRAMMING

5-1 Dimensional Data Input Method

5-1-1 Absolute/Incremental data input: G90/G91

1.Function and purpose

Setting of G90 or G91 allows succeeding dimensional data to be processed as absolute data or incremental data.

Setting of arc radius (with address R) or arc center position (with addresses I, J, K) for circular interpolation, however, must always refer to incremental data input, irrespective of preceding G90 command.

2.Programming format

G90 (or G91) Xx1 Yy1 Zz1 αα1 (α: Additional axis) where G90: Absolute data input

G91: Incremental data input

3.Detailed description

1.In the absolute data mode, axis movement will be performed to the program-designated position within the workpiece coordinate system, irrespective of the current position.

N1 G90G00X0 Y0

In the incremental data mode, axis movement will be performed through the programdesignated distance as relative data with respect to the current position.

N2 G91G01X200. Y50. F100

N2 G90G01X200. Y50. F100

Y

200.

Tool

100.

N1

N2

X

MEP011

Commands for a movement from the origin of the workpiece coordinate system are given with the same values, irrespective of whether the absolute data mode or the incremental data mode is used.

5 POSITION PROGRAMMING

2.The last G90 or G91 command works as a modal one for the following blocks.

(G90) N3 X100. Y100.

This block will perform a movement to the position of X = 100 and Y = 100 in the workpiece coordinate system.

(G91) N3 X-100. Y50.

This block will perform a movement of –100 on the X-axis and +50 on the Y-axis, and thus result in a movement to the position of X = 100 and Y = 100.

3.Multiple G90 or G91 commands can be set in one block, and thus only a specific address can be set as absolute data or incremental data.

N4 G90X300. G91Y100.

In this example, dimensional data X300 preceded by G90 will be processed as an absolute data input, and Y100 preceded by G91 as an incremental data input. Therefore, this block will result in a movement to the position of X = 300 and Y = 200 (100 + 100) in the workpiece coordinate system.

Y 200.

N4

100.

Moreover, G91 (incremental data input mode) will work for the succeeding blocks.

4.Either the absolute data mode or the incremental data mode can be freely selected as initial mode by setting the bit 2 of user parameter F93.

5.Even in the MDI (Manual Data Input) mode, G90 and G91 will also be handled as modal commands.

5-2 Inch/Metric Selection: G20/G21

1.Function and purpose

Inch command/metric command selection is possible with G-code commands.

2.Programming format

G20: Inch command selection

G21: Metric command selection

3.Detailed description

1.Changeover between G20 and G21 is effective only for linear axes; it is meaningless for rotational axes.

Example: Preset unit of data input and G20/G21 (for decimal-point input type Ι)

2.To perform G20/G21 changeover in a program, you must first convert variables, parameters, and offsetting data (such as tool length/tool position/tool diameter offsetting data) according to the unit of data input for the desired system (inch or metric) and then set all these types of data either on each data setting display or using the programmed parameter input function.

Example: If Initial inch selection is OFF and offsetting data is 0.05 mm, the offsetting data must be converted to 0.002 (0.05 ÷ 25.4 ≈ 0.002) before changing the G21 mode over to the G20 mode.

3.In principle, G20/G21 selection should be done before machining. If you want this changeover to be performed in the middle of the program, temporarily stop the program by an M00 command after G20 or G21 and convert the offsetting data as required.

Example: G21 G92 Xx1 Yy1 Zz1

MM

MM

MM

G20 G92 Xx2 Yy2 Zz2

M00 → Convert offsetting data here.

M

F10 → Set an F (Feed rate) command anew.

Note: Do not fail to give an F command appropriate to the new unit system after changeover between G20 and G21. Otherwise, axis movements would be performed using the last F value before the changeover, without any conversion, on the basis of the new unit system.

4.Whether G20 or G21 is to be selected upon switching-on can be specified by the bit 4 of user parameter F91 (Initial Inch parameter).

5-3 Decimal Point Input

1.Function and purpose

The decimal point can be used to determin the units digit (mm or inch) of dimensional data or feed rate.

2.Programming format