9/Series CNC Lathe. Operation and Programming Manual

Chapter 19

Dual Axis Operation

Figure 19.2 shows the position display for a system that contains a dual

axis group containing two axes with a master axis name of X. Whether or

not all axes of a dual group show up on the position display is determined

in PAL by your system installer.

Figure 19.2

Axis Position Display for Dual X Axis

E-STOP

PROGRAM[ MM

]

0.000 MMPM

-7483.647

-0219.550

-2345.673

(ACTIVE PROGRAM NAME)

-7483.647

MEMORY

MAN STOP

PRGRAM

OFFSET

MACRO

PRGRAM

SYSTEM

MANAGE

PARAM

CHECK

SUPORT

19.1

This feature allows you or the programmer to disable selected axes of the

Parking a Dual Axis

dual group. Any axis that is a member of a dual axis group can be parked.

Axes in the dual group may be parked simultaneously. If all axes in the

group are parked, no motion can take place in the dual axis group.

Once parked, no motion is allowed on the parked axis. Programmed and

jog commands (including any homing requests) made to the dual axis

group are ignored by the parked axes.

Axes in the dual group may only be parked or unparked when the control

is in cycle stop and end-of-block state. The control cannot be in the

process of completing any jog request or PAL axis mover request. If an

attempt is made to park/unpark an axis, and if any one of the above

requirements is not true, the control ignores the request to park/unpark the

axis.

19-3

Chapter 19

Dual Axis Operation

CAUTION: Be careful when an axis is unparked. Any

incremental positioning requests you make to the dual axis

group are referenced from the current location of all axes in the

dual group. This includes any manual jogging or any

incremental part program moves. When an axis is unparked, we

recommend you make the next command the dual axis group be

an absolute command to realign the axes in the dual group to

the same position.

Perform an axis park in a dual group through PAL. Refer to your system

installer’s documentation for details on how axes are parked.

Important: Some systems can have special parking requirements when

homing axes in a dual group. See section 19.2 for details on homing dual

axes.

19.2

There are two methods to home axes in a dual axis group. Your system

Homing a Dual Axis

installer determines through PAL which method is available. The two

methods are:

home each axis in the dual group individually

home all axes in the dual group simultaneously

Both of these homing methods can be available for automatic (G28) as

well as manual homing operations.

Your system installer can also define independent speeds and home

positions for each axis in a dual group through AMP. This applies to both

homing methods. Refer to your system installer’s documentation for

details on these speeds and locations.

Homing Axes Individually

This method requires that each axis be homed individually. When a

manual home operation is performed, a home request must be made to

each axis in the dual group on an individual method. Refer to chapter 4 for

details on how to request a manual home operation.

When you use automatic homing (G28), the axes must be homed one at a

time. This is accomplished by parking all other axes in the dual axis group

except the axis that is to be homed and requesting that the AMP-assigned

master axis name be homed in the G28 block. Once homed, that axis

should be parked, the next axis to be homed should be unparked, and the

homing procedure repeated. Refer to chapter 14 for details on how to

request an automatic home operation (G28).

19-4

Chapter 19

Dual Axis Operation

Homing Axes Simultaneously

This method allows a request for all axes in the dual group to be homed at

the same time. This does not mean that all axes reach home at the same

time. Keep in mind that your system installer can define different

feedrates and different home positions for each axis in the dual group.

With proper PAL programming, your system installer can configure all

axes in the dual axis group to home when the request is made to the master

axis. If you use this homing method, all unparked axes home together.

Refer to chapter 4 for details on how to request a manual home operation

and chapter 14 on how to request an automatic home operation (G28).

19.3

You can position axes in a dual axis group using any of the normal

programming or manual motion operations. Only the master axis name

Programming a Dual Axis

can be requested to position a dual axis. Requests to position a dual axis

can be made in manual, automatic, or MDI mode.

For absolute and incremental moves, regardless of the start-point, each axis

in the dual group reaches the requested position (or travel the requested

distance) at the same time. For absolute moves, this means individual axis

feedrates can be modified, depending on the distance each axis must travel

from start to end of the requested move.

Your system installer can assign different maximum cutting, external decel,

and rapid feedrate limitations for each axis in a dual axis group. The

control uses the slowest feedrate for each of these features from any axis in

the dual axis group.

Special consideration must be given when programming these features:

Feature:

Consideration:

Mirror Imaging

Programmable mirror image is applied to all axes in the dual group. Manual

mirror image, however, can be applied to each axis in the dual group individually.

When manual mirroring is performed on selected axes in the dual group,

positioning commands are in effect reversed from the programmed commands to

the master axis. Manual mirror image is selected through PAL. Refer to the

system installer’s documentation and chapter 14 for details.

Scaling

When scaling, specify the scale factor for the master axis of the dual group. All

other axes in the dual group are then scaled using the master axis scale factor.

Refer to chapter 13 for details.

Digitizing

When generating program blocks using digitize, park all but one axis of the dual

axis group. Use this unparked axis to generate the axis positions for the digitize

feature. The blocks created are stored using the master axis name. Refer to

chapter 5 for details.

19-5

Chapter 19

Dual Axis Operation

Important: You can use the PAL axis mover feature if it is necessary to

position dual axis group members separately without requiring any

parking. Refer to the PAL manual and the system installer’s

documentation for details.

Invalid Operations on a Dual Axis

Table 19.A lists the features that are not compatible with dual axes. If you

must execute one of these features on a dual axis, only the AMP master

axis can be used. All other axes in the dual group must be parked.

Refer to your system installer’s documentation to determine which axis has

been assigned in AMP as the master axis.

Table 19.A

Features Not Compatible With Dual Axes

G-code

Feature

G16.1

Virtual C Cylindrical Interpolation

G16.2

Virtual C Cylindrical End Face Milling

G20, G24

Single Pass Roughing

G21

Single Pass Threading

G31-G31.4

External Skip Functions

G33, G34

Thread Cutting Mode

G37-G37.4

Automatic Tool Gauging Skip Functions

G72-G75

Roughing Cycles

G76

Face Grooving Cycle

G77

Grooving Cycle

G78

Multi-Pass Threading Cycle

G84.2, G84.3

Solid Tapping

G86.1

Boring Cycle w/Shift

G87

Back Boring Cycle

19-6

Chapter 19

Dual Axis Operation

19.4

Give consideration to offsets used for a dual axis. In most cases, each axis

can have independent offset values assigned to it. This section describes

Offset Management for a

the difference in dual axis operation when it concerns offsets. How to

Dual Axis

activate/deactivate and enter these offset values is not described here

unless some change specific to a dual axis occurs. See chapter 3 for

implementation details about the offset you are using.

Preset Work Coordinate Systems (G54-G59.3)

The operation of the work coordinate systems is functionally the same for

a dual axis as any other axis. Each axis in the dual group can have its own

independent value entered into the offset table. If you want all axes in the

dual group to have the same offset values, you must manually enter the

same value for each axis in the dual group.

G52 Offsets

All axes in the dual group use the same value for the G52 offset regardless

of whether they are parked. When you specify a G52 offset value using

the master axis name, each axis offsets its coordinate system incrementally

by the G52 amount.

G92 Offsets

When a G92 offset value is specified using the master axis name, the

current position of all axes in the dual group takes on the location of the

specified value.

For example, if you have a dual axis named X, and it consists of two axes,

X1 and X2, when programming the following:

G92X10;

the control causes the current positions of X1 and X2 to become 10

regardless of their current positions when the G92 offset is executed.

Different G92 offset values can be created for each axis if necessary. This

is accomplished by performing a jog offset or by using the PAL axis mover

to change the position of the dual axes relative to each other before the

G92 block is executed.

19-7

Chapter 19

Dual Axis Operation

Set Zero

You can perform a set zero operation on the axes in a dual group on an

individual basis. For example, if you have a dual axis named X and it

consists of two axes, X1 and X2, when the set zero operation is executed

through PAL, you must specify which axis in the dual group to set zero.

When the set zero operation is performed on an axis, the current axis

location becomes the new zero point of the coordinate system.

Cutter Compensation

Only one tool diameter can be active at any one time. Any offset created

by cutter compensation affects all axes in the dual group.

Tool Length Offsets

Functionality is the same as for any other axis; independent values can be

entered for each axis in the dual group. A T-word selects the length offset

number, and the tool length offset is activated for each axis. Refer to

chapter 20 for details on activating tool length offsets.

Additional programming for the G10L10 and G10L11 codes are available

when a dual axis is the tool length axis. Since each axis in the dual group

can have separate offset values, the G10 block must contain an individual

name for each axis being assigned a value. Just programming the master

axis name assigns values only to the master axis. Your system installer

assigns axis names to all axes in the dual group in AMP. Refer to your

system installer’s documentation for details.

END OF CHAPTER

19-8

Chapter

Tool Control Functions

20.0

This chapter describes these tool control functions:

Chapter Overview

Topic:

On page:

Programming a T-word

20-3

Entering tool offset data

20-6

Tool management

20-14

Programming a T-word ---- Different formats available for selecting a

tool number and tool offsets

Tool length offsets ---- Compensate for the difference between the tool

length assumed while programming, and the actual length of the tool

used for cutting. This feature can offset up to 4 axes.

Tool Management and Random Tool ---- Tool life monitoring and tool

changer pocket control

Important: Tool Tip Radius Compensation compensates for the difference

between the tool diameter assumed while programming and the actual

diameter of the tool used for cutting (eliminates overcutting or uncut

portions of a workpiece due to differences in tool orientations and tip

radius) as described in chapter 21.

20-1

Chapter 20

Tool Control Functions

20.1

Modern machining processes usually require a machine that is capable of

selecting different tools. Typically tools are mounted in a turret and

T-words and Tool Length

assigned tool numbers as illustrated in Figure 20.1. The tool length offset

Offsets

data, tool tip radius data, tool wear compensation data and tool orientation

data are set in the offset table corresponding to different offset numbers

See chapter 3.

Figure 20.1

Typical Lathe Tool Turret

The selection of a tool number and an offset number for that tool is done

by programming a T-word. A T-word can be programmed at any location

in a part program.

Important: When you activate the MISCELLANEOUS FUNCTION

LOCK feature, the control displays M-, B-, S-, and T-words in the part

program with the exception of M00, M01, M02, M30, M98, and M99.

Activate this feature through the front panel screen (as described in chapter

2) or by an optional switch installed by your system installer.

20-2

Chapter 20

Tool Control Functions

20.1.1

Important: If tool life management is being used on the system, see the

Programming a T-word and

tool management section in this chapter for details on programming a

Tool Offsets

T-word. This section assumes that the tool life management feature is not

being used.

Your system installer determines the format for a T-word in AMP.

Table 20.A shows the 6 available format selections.

Table 20.A

T-word Formats

* FORMAT TYPE

WEAR OFFSET #

GEOMETRY OFFSET #

(1) 1 DGT GEOM + WEAR

last digit

same as wear

(2) 2 DGT GEOM + WEAR

last two digits

same as wear #

(3) 3 DGT GEOM + WEAR

last three digits

same as wear #

(4) 1 DGT WEAR

last digit

same as tool #

(5) 2 DGT WEAR

last two digits

same as tool #

(6) 3 DGT WEAR

last three digits

same as tool #

^* For details on which format is being used on a specific control refer to documentation prepared by the system installer.

To use Table 20.A find the format being used on your system. Then go

down the wear offset # column and find which digits of the T-word are

used as the wear offset number. Any other digits to the left of the wear

number are used as the tool number. If there are no digits remaining to the

left of the wear number, the control uses tool number 0. The third column,

geometry offset #, tells if the geometry number is the same number as the

number used for wear or tool. Just because geometry may use the same

offset number as wear it is not necessarily calling the same offset value.

Example 20.1

Using T-word Format #5

T213;

This T-word first calls for tool number 2 to be rotated into position, then data is accessed from

the offset tables (chapter 3) for values under tool geometry offset number 2, and tool wear offset

number 13.

20-3

Chapter 20

Tool Control Functions

Example 20.2

Using T-word Format #3

T2013;

This example first calls for tool number 2 to be rotated into position, then data is accessed from

the offset tables (chapter 3) for values under tool geometry offset number 13, and tool wear

offset number 13.

From these simple examples translation to the other formats should be

relatively easy. The tool number is always the digits closest to the T-word.

The maximum value that a tool number can have is determined by the

system installer in AMP.

To cancel the tool length offset, program a T-word with a geometry and

wear offset number of 0. The control does not cancel the active tool

number since a tool number of 0 is invalid. If the wear or geometry offset

number is the same as the tool number, a T-word of 0 cancels the offsets

but not the tool number.

Example 20.3

Canceling Tool Offsets (Any T-word Format)

Assume that tool number 1 is the active tool number.

T0 ;

This example cancels all offsets and keeps tool number 1 in the turret. The system installer has the

ability to force a tool change when T0 is programmed if he desire with a specific PAL program.

Refer to your system installers documentation for details.

Important: Your system installer determines in AMP whether or not all

tool length offsets are canceled when the control is reset or an M02 or M30

end of program block is read.

Important: A T-word also calls up geometry and wear radius data for use

in TTRC. See chapter 21.

20-4

Chapter 20

Tool Control Functions

20.1.2

Your system installer has the option in AMP to determine exactly when the

geometry and wear offsets take effect and when the tool position changes

Activating Tool Length

to the new shifted location. This manual makes the assumption that the

Offsets

system is configured to immediately shift the coordinate system by the

geometry and wear amounts, and delay the move that re-positions the tool

to the same coordinate position in the current work coordinate system. See

the documentation prepared by your system installer to determine the

application in a specific system.

Provided your system is configured as described above, the control

activates a tool offset as described below:

The control reads a block that activates or deactivates a tool length

offset. This is a block that contains a T-word for the above

configuration.

The control immediately shifts the work coordinate system the amount

of the tool geometry and tool wear amounts called by the T-word.

Different values can be entered for the offsets for each axis in the offset

table. The tool position display changes reflecting this shift. The

absolute position display does not change.

The offset is interpolated into the next move that generates axis motion

on the offset axis, unless you are in incremental mode. If you are in

incremental mode, the offset is not interpolated into the next move of

the axis.

Example 20.4

Immediate Shift/Delay Move in Incremental and Absolute Modes

Absolute Mode

Incremental Mode

G00Z0

Rapid Mode

G00Z0

Rapid Mode

G90

Absolute Mode

G91

Incremental Mode

T01

Activate tool 1. Program display

T01

Activate tool 1. Program display

changes Z position to -3.

Axis moves to +1

Axis moves to -2

If immediate shift, immediate move is selected in AMP, the control

generates its own linear block to create the offset and positions the tool to

the coordinates in the shifted work coordinate system as they were before

the system was shifted. If axis words are present in the block that activates

or deactivates a tool length offset, the control adds this generated move to

the programmed move.

Important: A T-word cannot be programmed in a block that generates a

circular motion (G02 or G03). If you want to change tools during circular

blocks the T-word must be programmed in its own block where no axis

motion takes place.

20-5

Chapter 20

Tool Control Functions

20.2

You can enter data in the tool offset tables by programming the correct

G10 command. This section describes the use of the G10 commands for

Entering Tool Offset Data

the lathe tool offset table.

Using (G10L10, G10L11)

Important: Only the value in the offset table value changes when a G10

code modifies a tool offset table value. If the changed offset value is

currently being used by the control, the active offset value is not changed

until it is called again from the offset table using a T-word.

When the control is in incremental mode (G91), any values entered in an

offset table using the G10 command are added to the currently existing

offset values. When the control is in absolute mode (G90), any values

entered in an offset table using the G10 command replace the currently

existing offset values.

This is a representation of the basic format for modifying the offset tables.

G10 L(10-11)P__ X__ Z__ R__ Q__ T__ O__

Where :

Is :

L(10-11)

Designates which offset table is being modified.

L10-Modifies the tool geometry table.

L11-Modifies the tool wear table.

The tool offset number that is having its values changed is specified following the P address.

The value to add to (in G91 mode) or replace (in G90 mode) the tool length offset for the X axis.

This value may be a diameter or radius value as determined with the O-word.

The value to add to (in G91 mode) or replace (in G90 mode) the tool length offset for the Z axis.

The value to add to (in G91 mode) or replace (in G90 mode) the tool tip radius amount.

The value to add to or replace the tool orientation amount

(valid only when setting data for the geometry table).

A T-word that corresponds to the tool number that is being changed.

Determines if the value being entered into the offset table is a radius or diameter value. This

only applies when setting data for the controls diameter axis (typically the axis perpendicular to

the spindle). If no O-word is programmed the control uses the current radius/diameter mode

active on the control.

O1-indicates a radius value

O2-indicates a diameter value

Important: Any axis word may be entered here along with/or without the

X- or Z-words. The lathe offset table allows the entry of offsets for up to

four different axis, tool radius, and tool orientation for each offset number.

Any values not specified in the G10 block remain unchanged.

20-6

Chapter 20

Tool Control Functions

Example 20.5

Using G10 to Change The Tool Offset Table

N00001

G90;

N00002

G10 L10 P4 Z2.1 Q1;

Offset number 4 has a new value of 2.1 for tool offset in the Z

direction and new orientation value of 1 in geometry table. The

current value for any axis not specified and for the tool radius

remain unchanged.

N00003

G10 P4 L11 Z1.1;

Offset number 4 has a new value of 1.1 for tool offset in the Z

direction in the wear table.

N00004

G91;

N00005

G10 L10 P4Z-1 Q1;

Offset number 4 has a new value of 0.1 (1.1 -- 1.) for tool offset

in the Z direction and new orientation value of 2 (1 + 1). The

current value for any axis not specified and for the tool radius

remain unchanged.

Important: G10 blocks cannot be programmed when TTRC is active.

20.3

Use the random tool feature to speed up production by saving cycle time

Random Tool

when a tool is returned to the tool changing device. This is done by

allowing the tool changer to randomly return the cutting tool to the most

convenient pocket in the tool changing device. The control remembers

what pocket the tool is returned to, and it is able to call the same tool from

the new pocket at any time.

Important: This feature can be used with normal tool selection or the tool

life management feature.

This feature has no effect on tool length offsets or cutter compensation.

These features must still be activated correctly as described in their

individual sections.

The random tool feature automatically decides the pocket that contains the

requested tool based on the information in the pocket assignment table. If

the requested tool has not been assigned to a pocket, the control generates

an error.

Based on the current pocket number, which is maintained by PAL, the

control tells PAL which pocket to move to, and how far, and in which

direction to move. The control also tells PAL where the tool currently in

use can fit in the tool turret.

Important: This feature is very PAL dependant. Before using this feature

make sure your system installer has written the PAL program to allow the

use of Random Tool.

The control automatically updates the tool pocket assignment table when

you make tool changes. The control indicates to PAL the best location to

return the tool to. PAL then decides where the tool gets placed in the tool

holder. The pocket that is vacated by the new tool is marked as empty.

20-7

Chapter 20

Tool Control Functions

Manually Entering Random Tool Data

Data can be entered into the random tool table either manually, as

described here, by programming, or by running a backup program of the

tool data. These other methods are described later in this section.

To manually enter the random tool data, follow these steps:

Press the {OFFSET} softkey.

(softkey level 1)

PRGRAM

OFFSET

MACRO

PRGRAM

SYSTEM

MANAGE

PARAM

CHECK

SUPORT

FRONT

ERROR

PASS-

SWITCH

PANEL

MESAGE

WORD

LANG

Press the {RANDOM TOOL} softkey. The pocket assignment table

screen is displayed as shown below. This screen shows the current

tool to pocket assignments. Your system installer designates the

number of tool pockets available on a system in AMP.

(softkey level 2)

WORK

TOOL

RANDOM

CO-ORD

WEAR

GEOMET

MANAGE

TOOL

COORD

BACKUP

SCALNG

ROTATE

OFFSET

20-8

Chapter 20

Tool Control Functions

POCKET ASSIGNMENT TABLE

PAGE 1 OF 2

PKT

TOOL

PKT

TOOL

PKT

TOOL

001

0002

002

003

0001

004

005

0003

006

XXXX

007

0007

008

XXXX

009

010

011

012

013

014

015

016

017

018

XXXX

019

0006

020

XXXX

021

022

023

024

025

026

027

028

029

030

031

032

033

034

035

036

037

038

039

RAPLCE

CLEAR

CUSTOM

ACTIVE

BACKUP

VALUE

The columns labeled PKT give the tool changer pocket numbers. The

columns labeled TOOL give the tool number of the tool in the

corresponding pocket. Pockets with no tools assigned to them show no

information next to the pocket number. Pockets with tools shown as

XXXX indicate that a custom tool (tool that requires more than one

pocket) has been assigned to use that pocket.

Move the cursor to the pocket number with the assignment or change

is to be made. Press the up, down, right, or left cursor keys on the

operator panel. Move the cursor full pages by holding down the

[SHIFT] key while pressing the up or down cursor keys. The

selected pocket appears in reverse video.

Important: If random tool is not to be used for your system, make sure

that none of the tool pockets have tool numbers assigned to them.

To modify tool data there are three choices:

To remove a tool assigned to a pocket, press the {CLEAR VALUE}

softkey. The selected tool is deleted from the table.

To enter a tool number for the pocket, press the {REPLCE VALUE}

softkey, key in the new tool number, and press the [TRANSMIT] key.

The old tool value is replaced with the new value just keyed in.

20-9

Chapter 20

Tool Control Functions

To enter a custom tool (a tool that requires more than one tool pocket)

enter the tool number of the custom tool in the pocket that is to be used

as the “shaft pocket”. The shaft pocket is where the tool changer is

positioned when the particular custom tool is to be used. Enter the

number of pockets needed (to a max of 9), a comma, followed by the

position of the shaft pocket in this group of pockets. Press the

[TRANSMIT] key enters the data into the table.

The screen shows XXXX for the tool number of any pockets that have

been configured as part of a custom tool, and show the tool number in the

pocket where PAL is told to go in order to find the tool.

For example, in the pocket assignment screen, pocket number 19 is a shaft

pocket for custom tool number 6. This custom tool requires 3 pockets,

pockets 18, 19, and 20. When the {CUSTOM} softkey was pressed for

pocket number 19, a value of 3,2 was entered.

Programming random tool data

This feature is available so that it is not necessary to always manually enter

the data into the pocket assignment table. By programming the correct

G10.1 blocks all information may be entered into the tool pocket table.

Note the control may automatically generate a G10.1 program by using the

backup softkey as described later in this section.

Important: G10 blocks cannot be programmed when TTRC is active.

Programming of random tool data can only be done on a tool pocket if data

has not already been configured for that pocket. If you need to make

changes to a tool pocket that already has a tool assigned to it, you must

either clear and re-load the entire random tool table as discussed below

(you can not use a G10.1 to clear individual pocket data), or use the

softkeys to manually access the random tool table and change the data

using the keyboard.

Clearing the Random Tool Table

This block clears all information in the random tool table:

G10.1 L20 P0 Q0 O0 R0;

20-10

Chapter 20

Tool Control Functions

Format for Programming Random Tool Table

Use this block to set data for the random tool pocket assignment table:

G10.1 L20 P__ Q__ O__ R__;

Where :

Is :

G10.1 L20

This tells the control that the block will be setting data for the random tool pocket

table. The G10.1 L20 is not modal, it must be programmed in every block that

sets data for the random tool pocket assignment table.

P__

The value following the P-word determines the pocket number that is being set.

Q__

The value following the Q-word determines the tool number of the tool that is in

the pocket determined with the P-word.

O__

The value following the O-word enters the number of pockets that are needed for

the tool. Normally a value of one is entered here however, for custom tools that

require more than one pocket, program the number of pockets that are required.

R__

The value following the R-word enters the pocket number of the shaft pocket for

the tool. Normally a value of one is entered here. However, for custom tools

that require more than one pocket, program the location relative to the other

pockets for that tool that the tool changer goes to to access that tool.

For example, this block

G10.1L20P1Q20O1R1;

tells the control that tool number 20 is in pocket number 1;

G10.1L20P3Q23O4R2;

tells the control that tool number 23 has its shaft pocket as pocket number

3, four pockets are required for the custom tool and the second of these

four pockets is the shaft pocket. This means that pockets 2, 3, 4, and 5 are

used for the custom tool number 23.

20-11

Chapter 20

Tool Control Functions

Backup Random Tool Table

The control has a feature that allows you to back up (save) the information

in the random tool table. The control generates a G10.1 program from the

information already in the table. To do this follow these steps:

Press the {OFFSET} softkey.

(softkey level 1)

PRGRAM

OFFSET

MACRO

PRGRAM

SYSTEM

MANAGE

PARAM

CHECK

SUPORT

FRONT

ERROR

PASS-

SWITCH

PANEL

MESAGE

WORD

LANG

Press the {RANDOM TOOL} softkey.

(softkey level 2)

WORK

TOOL

RANDOM

CO-ORD

WEAR

GEOMET

MANAGE

TOOL

COORD

BACKUP

SCALNG

ROTATE

OFFSET

Press the {BACKUP} softkey. The control prompts you for a

program name. Key in the program name that is to contain the

information from the random tool table and press the [TRANSMIT]

key. This program name cannot already exist in control memory.

This allows the control to generate a program that automatically loads the

necessary data into the random tool table. This program can be edited as

changes to tool table are needed.

The control automatically places this G10.1 program in control memory. If

you want to send the program to a peripheral device, it must be sent from

control memory as described in chapter 9. The program cannot be sent

directly to a peripheral.

20-12

Chapter 20

Tool Control Functions

Starting a Program with a Tool Already Active

You can begin a part program with a tool already active in the chuck. In

order for random tool to be able to properly handle that tool, it must enter

information about that tool in the random tool table.

Important: If you use random tool when the tool was loaded into the

chuck, it do not need to enter any data since random tool remembers what

tool is loaded even after power is turned off. This procedure is only

necessary if a tool is loaded manually or if random tool was not used when

the tool was loaded.

The control needs the following information to properly handle a tool that

is already active in the chuck. Tool number, number of pockets the tool

uses, and position of the shaft pocket relative to these other pockets (refer

to the section on manual entry of data for details on shaft pocket and

custom tool data). Do this in the following way:

Press the {ACTIVE} softkey. The control prompts you for the tool

number, the number of pockets, and the position of the shaft pocket

relative to the these other pockets all separated by commas.

(softkey level 3)

RAPLCE

CLEAR

CUSTOM

ACTIVE

BACKUP

VALUE

The control displays the configuration of the tool that it thinks is

currently loaded into the chuck. If these values are incorrect, replace

them using the correct tool information. Enter a value for tool

number, number of pockets, and position of the shaft pocket all

separated by commas on the input line. Data can be edited on the

input line as described in chapter 2.

When the data for the tool that is currently in the chuck is correct,

press the [TRANSMIT] key. The control is now able to return the

tool that is in the chuck to the best location in the tool changer at the

proper time.

Important: You can also use the {ACTIVE} softkey to clear the currently

active tool and specify no tool is currently in the spindle. To specify no

tool is in the spindle press the {ACTIVE} softkey and delete any

information that appears at the prompt. When the [TRANSMIT] key is

pressed, the active tool is cleared and the random tool assumes no tool is in

the spindle.

20-13

Chapter 20

Tool Control Functions

20.4

Use the automatic tool management feature to monitor the life of a tool,

determine when the tool should be replaced, and provide a replacement

Automatic Tool Life

tool when that tool is requested in a program.

Management

Tool are assigned to selected groups. Instead of calling a specific tool in a

program, the programmer calls a tool group. The control then selects the

first tool assigned to that group. If that tool has exceeded its entered tool

life, then a replacement tool is selected from the next tool number assigned

to that group. If that tool has exceeded its expected tool life, then the next

tool in the group is selected. This continues until no more tools are

available in that tool group. When a group is called that no longer has any

available tools, an error is generated.

The correct tool length and tool radius offsets are assigned independently

for each tool in the group.

20.4.1

This section describes how to set up the tool groups and the information

that must be entered for each tool group. This section described the

Tool Directory Data

manual method of entering this information. Page 20-26 describes a

method of entering all information into the tables by programming.

Assigning Tool Numbers to Groups

Normally tools that are assigned to the same group have similar

characteristics (such as a boring tool or a drilling tool). If one tool in the

group is worn, the control should be allowed to select any tool in the same

group and still be able to cut the same part using the same program.

Your system installer determines in AMP the usable range of tool group

numbers by determining a boundary. Any tool number that is programmed

above this boundary is used as a tool group number (the value of the

boundary is subtracted from the tool number programmed). Any tool

number that is programmed below this boundary is used as a normal tool

number. A maximum of 200 group numbers are available.

Enter different tool length offset numbers, and radius offset numbers into

the tool management table with the tool numbers in each group. When you

select a tool from a group by the control, the tool length and radius offset

numbers are activated with them getting the data for the tools radius,

length’s for each axis, and orientation from the tool offset tables. See

chapter 3 on entering tool data for details.

20-14

Chapter 20

Tool Control Functions

Tool Life Measurement Type

The control can measure the life of a tool using one of three possible

methods:

Tool Life Type

Method Selected

Meaning

time

This is selected by choosing 0 as the type of tool life

measurement.

Time measures tool life as the length of time that a

cutting tool is operated at a cutting feedrate.

The value for the expected tool life is entered in units of

minutes.

number of times

This is selected by choosing 1 as the type of tool life

used

measurement.

Number of times used measures tool life as the number

of times that the tool is selected as the active tool.

The value for the expected tool life is entered as the

number of times the tool may be used to cut parts; this

number is per program.

Regardless of the number of times that a tool is selected

as active in a specific program, it only counts as one use

each time the program is executed.

distance

This is selected by choosing 2 as the type of tool life

measurement.

Distance measures tool life as the distance that the tool

has been moved using a cutting feedrate.

The value for the expected tool life is entered in units of

inches or millimeters depending on the mode that the

control is operating in at the time.

For multi-axis moves, the vectorial distance traveled by

the tool is the distance used for tool life measurement.

Select the tool life type (selected as either 0, 1, or 2) on a per-group basis.

Different groups may use different tool life types however each tool in the

group uses the same tool life type.

20-15

Chapter 20

Tool Control Functions

Tool life Threshold Percentage

A threshold level may also be assigned to a tool group. The threshold level

is assigned as a percentage of the total expected life of the tool. When a

tool reaches this threshold level, it is classified as old for that tool group.

A tool is classified as old only to allow the operator to see that a tool is

close to expiration. If the tool is being used when it reaches the threshold

level, it continues to be used as normal until the tool reaches the “expired

state” (100% of the expected tool life).

The tool life threshold percentage is selected on a per-group basis.

Different groups can use different threshold percentage, however each tool

in the group uses the same threshold percentage.

Entering Tool Group Data

To enter tool group data, you must create the tool groups. This is done

automatically when the group is selected to edit. To enter tools into groups

and enter other tool group data follow these steps:

Press the {OFFSET} softkey.

(softkey level 1)

PRGRAM

OFFSET

MACRO

PRGRAM

SYSTEM

MANAGE

PARAM

CHECK

SUPORT

FRONT

ERROR

PASS-

SWITCH

PANEL

MESAGE

WORD

LANG

Press the {TOOL MANAGE} softkey.

(softkey level 2)

WORK

TOOL

RANDOM

CO-ORD

WEAR

GEOMET

MANAGE

TOOL

COORD

BACKUP

SCALNG

ROTATE

OFFSET

Press the {TOOL DIR} softkey. The control displays the current tool

directory screen showing all of the current tools and the groups that

they have been assigned to (see the following figure). The control

displays the prompt “EDIT GROUP:”.

(softkey level 3)

TOOL

BACKUP

DIR

DATA

20-16

Chapter 20

Tool Control Functions

Figure 20.2

Typical Tool Group Directory Screen

ENTRY GROUP NO:

TOOL GROUP DIRECTORY

PAGE 1 0F 1

(FILE NAME)

GROUP

TOOL NUMBER

EDIT

DELETE

GROUP

ALL

At this point, you can delete any or all tool groups that already exist for

some reason follow these steps:

To delete:

Press:

select tool group

the {DELETE GROUP} softkey. Key in the desired group number to delete

and press the [TRANSMIT] key. This deletes all information in the tool group

including the tool offset numbers, threshold rate, tool numbers, etc.

all of the tool groups

the {DELETE ALL} softkey. The control prompts “DELETE ALL TOOL

MANAGEMENT DATA? (Y/N):”. Entering “Y”deletes all tool management

data that has been entered into the management tables (this does not delete

any G10 programs that are backups or used to set the tool management

tables). Entering “N”aborts the delete operation.

Key in the group number that is to be edited. When you select the

correct group, press the [EDIT GROUP] key. Figure 20.3 shows all

of the information for that tool group that is displayed.

20-17

Chapter 20

Tool Control Functions

Figure 20.3

Typical Tool Group Data Screen

ENTER DATA:

EDIT TOOL GROUP 1

PAGE

1 OF 1

(FILE NAME)

THRESHOLD RATE =80%

ENTRY

TOOL NUMBER

LIFE TYPE = TIME

OFF NO

CHANGE

INSERT

DELETE

CHANGE

TOOL

TYPE

T RATE

From this screen, you can:

Operation:

Description:

Change tools

Alter one of the tool numbers that has already been entered in the group. Move the cursor to the tool number to be changed

by pressing the up or down cursor keys (move the cursor full pages by holding down the shift key while pressing a cursor

key). Press the {CHANGE TOOL} softkey. Key in the new tool number and press the [TRANSMIT] key.

Insert tools

Insert a new tool number for that group. Move the cursor to the location to insert a new tool number at by pressing the up or

down cursor keys (move the cursor full pages by holding down the shift key while pressing a cursor key). Press the

{INSERT TOOL} softkey. Key in the new tool number and press the [TRANSMIT] key. The actual range of allowable tool

numbers is 1 to 9999.

Delete tool

Remove a tool number from that group. Move the cursor to the tool number to be removed by pressing the up or down

cursor keys (move the cursor full pages by holding down the shift key while pressing a cursor key). Press the {DELETE

TOOL} softkey. Respond yes or no and press [TRANSMIT].

Change life type

Alter how the control records and measures tool life for that group. Press the {CHANGE TYPE} softkey. The prompt “LIFE

TYPE...”is displayed on line 2 of the CRT. The same life type is assigned to all tools in any one tool group. Key in the

number of the desired tool life measurement type for that group and press the [TRANSMIT] key. 0 for “time,”1 for “number of

tool uses,”and 2 for “distance.”

Change life threshold rate

Alter the percentage of a tool’s expected life so that a tool is labeled as old. This percentage applies to all tools in the

selected group. To alter the threshold percentage (the percentage of total tool life that has been used before a tool will be

classified as old) press the {CHANGE T RATE} softkey. Key in the percentage of the total tool’s life so that the tool is

classified as old and press the [TRANSMIT] key. Tool life threshold rate is explained earlier in this section.

Change Color

(softkey level 4)

EDT LN

EDT CT

EDIT

RENEW

SCROLL

OF #

COMP #

LIFE

TOOL

COLOR

The application of these operations was described in detail earlier in this

section. All of this information can be entered into the tool groups using

the programming method described on page 20-22 .

20-18

Chapter 20

Tool Control Functions

20.4.2

This section assumes that tools have already been assigned to their specific

groups. This section describes specific information that is to be entered

Assigning Detailed Tool

into the tool life management tables for the individual tools. This

Data

information may also be entered into the tool management tables using the

programming method described on page 20-22. This information includes:

Tool length offset number

Tool diameter/radius offset number

Expected life of a tool

Tool length and diameter/radius offset number

Use this feature of tool life management so the programmer does not need

to know what tool has been called by tool life management and still have

the correct tool offsets and cutter compensation activated.

Important: The control only automatically enters the tool length and

cutter compensation offset numbers. This may or may not activate the tool

length offset or cutter compensation features. These features must still be

activated as normal.

Expected Tool Life

Use this feature of tool life management to set the expected life of a tool.

The type of tool measurement used is assigned to the tool group as

described in section 20.5.1. This tool measurement type determines the

units that are used for the expected tool life.

As a tool is used the amount of usage is recorded and displayed as the

accumulated tool life (the amount of the expected tool life that has been

used). This is displayed individually for each tool on the tool data display

screen. The accumulated tool life can be reset to zero by pressing the

{RENEW TOOL} softkey.

The following is a description of the units that should be entered for the

different tool life measurement types:

If tool life is measured in units of time (0 is selected as tool life type),

then the units for the expected tool life is minutes. Enter the minutes of

operation that the tool is expected to operate and still be within the

tolerance required for the part being cut. The accumulated life of a tool

is only measured when that tool is the active tool, and it is performing a

cutting operation. Moves that are rapid, or blocks that do not produce

axis motion are not added to the accumulated tool life.

20-19

Chapter 20

Tool Control Functions

If tool life is measured by the number of uses (1 is selected as tool life

type), then the units for the expected tool is the number of programs that

the tool may be selected as an active tool in. The accumulated life of a

tool is increased by one if that tool is selected in a program as the active

tool. Remember that the same tool may be active more than once in a

program, however its accumulated life only increments by one. Enter

the total number of program executions that can use the tool before the

tool no longer meets the required tolerance for the part being cut.

If tool life is measured in units of distance (2 is selected as tool life

type), then the units for the expected tool life is either inches or

millimeters (depending on the current operating mode of the tool).

Enter the distance of travel that the tool is expected to cut and still be

within the tolerance required for the part being cut. The accumulated

life of a tool is only measured when that tool is the active tool, and it is

performing a cutting operation. Moves that are are rapid, or blocks that

do not produce axis motion are not added to the accumulated tool life.

For multi-axis moves (including arcs and helices) the distance added to

the accumulated life is the vectorial distance, not necessarily the

distance traveled on each axes.

During turning cycles only the distance that the tool travels along the

workpiece contour is added to the accumulated life. The other three

moves of the cycle are not added regardless of if they are executed at

cutting speed. The entire finishing pass for the contouring routine (if

any) is used to increase the accumulated tool life.

Entering Specific Tool Data

The following steps describe the method of entering specific tool data for

tool management. This includes tool offset numbers, and expected tool

life:

Important: This section assumes that the steps required to assign tools to

specific groups has been performed as described in section 20.5.1.

Press the {OFFSET} softkey.

(softkey level 1)

PRGRAM

OFFSET

MACRO

PRGRAM

SYSTEM

MANAGE

PARAM

CHECK

SUPORT

FRONT

ERROR

PASS-

SWITCH

PANEL

MESAGE

WORD

LANG

20-20

Chapter 20

Tool Control Functions

Press the {TOOL MANAGE} softkey.

(softkey level 2)

WORK

TOOL

RANDOM

CO-ORD

WEAR

GEOMET

MANAGE

TOOL

COORD

BACKUP

SCALNG

ROTATE

OFFSET

Press the {TOOL DATA} softkey. The control displays the prompt

“EDIT GROUP:”.

(softkey level3)

TOOL

BACKUP

DIR

DATA

Key in the group number to edit using the keys on the operator panel

and press the [TRANSMIT] key. Figure 20.4 shows all of the

information for that tool group that is displayed.

Figure 20.4

Typical Tool Data Screen

ENTER DATA=

GROUP

DATA

TYPE=TIME

PAGE

1 OF 1

(FILE NAME)

THRESHOLD RATE

80%

TOOL

T.LEN

CUTTER

EXPECT

ACCUM

TOOL

OFF NO

CMP NO

LIFE

STATUS

100

EXPIRED

100

OLD

100

EDT LN

EDT CT

EDIT

RENEW

SCROOL

OFF #

COMP #

LIFE

TOOL

COLOR

20-21

Chapter 20

Tool Control Functions

From this screen it is possible to perform the following operations.

The application of these operations was described in detail earlier in

this section.

Operation:

Description:

Enter or alter the tool

To enter or alter a value for the tool length offset number, move the cursor

length offset number

to the tool number of the tool to alter and press the {EDIT LN OFF}

softkey. Key in the new offset number that calls the correct data from the

offset tables for that tool for its tool length offset number and press the

[TRANSMIT] key. The old value for tool length (if any) is discarded and

the new value replaces it.

Enter or alter the tool

To enter or alter a value for the tool radius offset number, move the cursor

radius offset number

to the tool number of the tool to alter and press the {EDIT CT CMP}

softkey. Key in the new offset number that calls the correct data from the

offset tables for that tool for it’s radius and press the [TRANSMIT] key.

The old value for radius offset numbers (if any) is discarded and the new

value replaces it.

Enter or alter the

To enter or alter a value for the expected life of a tool, move the cursor to

expected life of a tool

the tool number of the tool to alter and press the {EDIT LIFE} softkey.

Key in the new expected life of the tool (in units as determined by the tool

life type) and press the [TRANSMIT] key. The old value for expected life

(if any) is discarded and the new value replaces it.

Reset the accumulated

To reset the accumulated tool life to zero, move the cursor to the tool

tool life to zero

number of the tool to alter and press the {RENEW TOOL} softkey. The

old accumulated life of the tool is discarded and a value of zero is entered

as the new accumulated tool life. This is normally performed after an old

or expired tool has been replaced with a new tool. This updates the

status of the tool and remove any “OLD,”or “EXPIRED”status.

Change color used to

Each tool group may be assigned its own tool color. To change the color

graph the tool selected

selected for a tool on the CRT press the {SCROL COLOR} softkey. This

on the CRT for color

alters tool color for the current tool when tool paths are displayed in either

systems

quick check graphics, or active tool path graphics.

(softkey level 4)

EDT LNEDT CT

EDIT

RENEW

SCROL

OFF #

COMP #

LIFE

TOOL

COLOR

20.4.3

This feature allows the rapid loading of information into the tool

Programming Data and

management tables. This is done by executing a program that

automatically loads the tool management tables. This program can also be

Backing Up Tool

generated automatically when the tool management tables are backed up as

Management Tables (G10L3,

described later in this section.

G11)

Data is sent to the tool management tables when the control executes this

G10 block:

G10L3;

This block indicates to the control that any information following this

block is to be used to set the tool management tables.

20-22

Chapter 20

Tool Control Functions

Important: G10 blocks may not be programmed when TTRC is active.

CAUTION: Any time that a G10L3; block is executed the

control automatically clears all information that is in the

management tables for all tools and tool groups.

Any time after the G10L3 command, parameters may be programmed to

enter what tool group is being entered, the type of tool life measurement

that is being used, and the tool life threshold percentage. The format for

this block is:

P__I__Q__;

Where :

Is :

P__

The value entered with the P-word is used to program what tool group number is

being edited. The following blocks assign tools to that tool group.

I__

The value entered with the I-word is used to program the type of tool life

measurement that is to be used for all the tools in that group. I0 sets a type of

time, I1 sets a type of number of uses, and I2 sets a type of distance. See

section 20.5.1 for details. If more than one I-word is programmed for a tool group

the control uses the last programmed I-word for that group. If no I-word is

programmed for a group the control uses I1 as a default value.

Q__

The value entered with the Q-word is used to program the threshold percentage

for that tool group. Enter the percentage of the total expected tool life that

causes the tools in the group to be classified as old. See section 20.5.1 for

details on threshold percentage. If the Q-word is not programmed in a block the

control uses a default value of 80%. If more than one Q-word is programmed for

a tool group the control uses the last programmed Q-word for that group. If no

Q-word is programmed for a tool group the control uses Q80 as the default value.

20-23

Chapter 20

Tool Control Functions

The following program blocks assign tools to groups, length and cutter

compensation offset numbers, and expected tool life to specific tools. This

information is assigned to the last group number programmed in a block

using the P-word. The format for these blocks is:

T__ H__ D__ L__;

Where :

Is :

T__

The value entered with the T-word is the tool number of the tool to be assigned to

that group.

H__

The value entered with the H-word is the tool length offset number from the tool

geometry and wear tables that is to be assigned to this tool. The H-word is only

valid if programmed in the same block as a T-word.

D__

The value entered with the D-word is the tool radius number from the tool

geometry and wear tables that is to be assigned to this tool. The D-word is only

valid if programmed in the same block as a D-word.

L__

The value entered with the L-word is used to program the value of the expected

tool life for that tool. The controls interpretation of this is dependant on the value

set with the I-word in this program block. The value programmed with the L-word

remains active for all following tools in that group until replaced with a different

L-word, or a new tool group is programmed with a P-word.

All of the tools should then be programmed for that group in individual

blocks. When all of the tools for that group have been entered, change

groups by programming a different P-word in a block.

When all of the tools for all of the different groups have been entered, end

the execution of editing the tool life management table by programming

either a M02 or M30 end of program blocks or by entering this block:

G11;

This cancels the G10 data setting mode for tool management.

Important: Any information that was contained for a specific tool group

that has been written to using a G10L3 command as described above is

overwritten by the information programmed with the G10 blocks. All

previous data for tool management for any of the groups is lost.

20-24

9/Series CNC Lathe. Operation and Programming Manual - page 16