Content      ..     15      16      17      18     ..

9/Series CNC Lathe. Operation and Programming Manual - page 17

Chapter 20

Tool Control Functions

Example 20.6

Programming Tool Life Management Data

Program Block

Description

G10L3;

Starts loading tables.

P1I1Q60;

Begins loading data for tool group 1. Type 1 (number of uses)

measurement. Threshold 60%.

T1H5D7L25;

Places tool 1 in group 1 with length offset number of 5, cutter

radius offset number 7, and expected life of 25 uses.

T2H2;

Places tool 2 in group 1 with length offset number of 2, no

cutter radius offset number and expected life of 25 uses.

T15H7;

Places tool 15 in group 1 with length offset number of 7, no

cutter radius offset number and expected life of 25 uses.

P2;

Begins loading data for tool group 2. Type 0 measurement

(default). Threshold at 80% (default).

T12H3D6L40;

Places tool 12 in group 2 with length offset number of 3, cutter

radius offset number of 6, and expected life of 40 minutes.

T13;

Places tool 13 in group 2 with length and radius offset numbers

of 0 and expected life of 40 minutes.

P4I0Q90;

Begins loading data for tool group 4. Type 0 (time)

measurement. Threshold at 90%.

T20H3D6;

Places tool 20 in group 4 with length offset number of 3, cutter

radius offset number of 6, and expected life of 0 minutes.

Q50;

Resets the threshold at 50% for group 4.

G11;

Ends the loading operation.

M02;

Backing up tool management tables

This feature causes the control to automatically generate a G10L3 program

that stores all of the information that it finds in the current tool

management table. Any time that this G10 program is executed, it clears

any information that is currently in the management tables and replaces it

with the information that is in the G10 program.

To generate the G10L3 backup program of the tool management tables,

follow these steps:

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

20-25

Chapter 20

Tool Control Functions

2.

Press the {TOOL MANAGE} softkey.

(softkey level 2)

WORK

TOOL

TOOL

TOOL

RANDOM

CO-ORD

WEAR

GEOMET

MANAGE

TOOL

COORD

BACKUP

SCALNG

ROTATE

OFFSET

3.

Press the {BACKUP DATA} softkey. The prompt “BACKUP

FILENAME:” is displayed on the input line.

(softkey level 3)

TOOL

TOOL

BACKUP

DIR

DATA

DATA

4.

Key in any legal program name and press the [TRANSMIT] key.

This program name is used as the program that stores all of the

backed up tool management data. The control generates the tool

management G10 program.

20.4.4

This section describes how to activate a tool using tool life management.

Programming a T-word

When using tool life management, remember:

Using Tool Management

Your system installer sets up a boundary for T-words used with tool life

management in AMP. Any T-word programmed that calls a tool number

less than, or equal to, this boundary is used as a normal tool number.

Any T-word programmed that calls a tool number greater than this

boundary is used as a tool group number for tool management.

When a T-word is programmed using tool life management, the group

that is called with the T-word is equal to the programmed T-word, minus

the value of the boundary set in AMP by your system installer. This

boundary does not include any offset number normally attached to the

T-word. Place holder digits for tool offsets must be programmed,

although their values are ignored. See Example 20.7.

Your system installer must have altered AMP parameters from their

default condition to use tool management. The default condition sets a

tool boundary at 100 and a T-word format of 3 digit geometry + wear.

This default configuration requires a minimum six digit T-word be

programmed to activate any tool group in tool life management. This

configuration does not work if the AMP parameter maximum

allowable T-word remains set to its default of only 5 digits.

20-26

Chapter 20

Tool Control Functions

Example 20.7

Assume your system installer has set the following constraints in AMP:

- the tool group boundary is set as 100

- the T-word format is configured as 2-digit geometry and wear (see

section 20.1)

- the maximum allowable T-word is configured as a 5-digit number

To use tool management program for these constraints:

Ttttoo;

Where :

Is :

Tttt

-- -- the group number (if greater than the group boundary)

-- -- a tool number (if less than the group boundary)

oo

the place holder for the tool offset number

Table 20.B

Result of Different T-words for Example 20.7

T-word

Result

T12;

Since tool number is below boundary and two digits are necessary for offset with

this T-word format, no tool is programmed here. Instead tool geometry and tool

wear offset number 12 is selected.

T1201;

Tool 12 and geometry and wear offset number 1 is selected. Tool life management

is not used because tool number 12 is below the group boundary of 100.

T10100;

The first available tool assigned to group 1 is selected along with the offset numbers

assigned to that tool in the tool management table.

T10201;

The first available tool assigned to group 2 is selected along with the offset numbers

assigned to that tool in the tool management table. The geometry and wear offset

number of 01 programmed here is ignored.

T123456;

Error occurs because maximum allowable T-word of 5 digits has been exceeded.

20-27

Chapter

21

Tool Tip Radius Compensation (TTRC)

Function

21.0

This chapter describes Tool Tip Radius Compensation function. Major

topics include:

Chapter Overview

Topic:

On page:

Programming TTRC

21-4

Generation blocks

21-8

Tool paths (Type A)

21-10

Tool paths (Type B)

21-20

Tool path during TTRC

21-30

Special cases

21-35

Error detection

21-52

Generally, cutting tools used on lathes have a rounded cutting edge which

often results in a difference between the cutting tool tip position assumed

in writing a part program, and the actual cutting tool tip position. This

inevitably causes a difference between the programmed shape and the

actual shape cut on the workpiece in taper and arc cutting operations. See

Figure 21.1.

For reference, the term “tool tip radius compensation” has been shortened

to TTRC and is referred to as such in the following sections.

The TTRC functions allows you to use tools with different radii without

requiring a modification of the part program.

21-1

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.1

Taper and Arc Cutting Without TTRC

Without TTRC active,

control assumes tool

has a perfect point

Cutting

tool

Actual tool

tip radius

Part

profile

Material left uncut

due to radius of

tool tip

Put the radius of the tool and tool orientation data into the offset tables in

advance. This function lets the control use the same program to produce

the same workpiece, regardless of the radius of the tool that does the

cutting.

This feature also uses tool orientation data taken from the tool geometry

table. You need this tool orientation to compensate for inaccuracies that

can occur from difficulties in measuring tool tip diameter because of a tool

mounting position. If this is not a factor, make sure all tool orientations

use an orientation of either 0 or 9.

CAUTION: If you use a 2-turret lathe, be aware that the X tool

offset and the tool orientation values will be opposite of the A

turret values for the second mirrored (B).

We use these terms in this section:

inside ---- Refer to an angle between two intersecting programmed tool

paths as inside if, in the direction of travel, the angle measured

clockwise from the second tool path into the first is less than or equal

to 180°. See Figure 21.2. If one or both of the moves are circular, the

angle is measured from a line tangent to the tool path at their point of

intersection.

21-2

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

outside ---- Refer to an angle between two intersecting programmed tool

paths outside if, in the direction of travel, the angle measured clockwise

from the second tool path into the first is greater than 180°. See

Figure 21.2. If one or both of the moves are circular, the angle is

measured from a line tangent to the tool path at their point of

intersection.

r ---- cutter radius

CR ---- cross-point between two programmed paths after you activate the

TTRC

Figure 21.2

Definition of Inside and Outside

workpiece

Inside angle (less than 180°)

Outside angle (greater than 180°)

workpiece

There are two types of cutter compensation available on the 9/Series

control:

type A (as described on page 21-10)

type B (as described on page 21-20)

21-3

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

This table highlights the differences between the two types:

Type of Move

Type A

Type B

Entry Move Into

-- The tool takes the shortest possible

-- The tool stays at least one radius away

TTRC

path to its offset position.

from the start-point of the next block at

all times.

-- Extra motion blocks can be generated

to attempt to prevent gouging of the

part as may occur in Type A.

Tool

-- Same as Type B.

-- Same as Type A.

Path

Exit Move From

-- The tool takes the shortest path to the

-- The tool takes the shortest path to the

TTRC

end-point of the exit move for both

end-point of exit move for inside

inside and outside corners.

corners only.

-- For outside corners, the tool stays at

least one radius away from the

end-point.

Your system installer determines whether to use type A or type B by a

control in AMP.

21.1

These G-codes are used for TTRC:

Programming TTRC

G-code:

TTRC, :

G41

left

G42

right

G40

cancel

Left or right is defined as offsetting the tool to the left or right of the

programmed cutting path when facing the direction of cutter motion.

Important: If you set a negative value in the offset tables as the tool

radius, this reverses compensation direction (tool left or right) for the G41

and G42 codes. G41 and G42 are also reversed during the mirroring

operation. See chapter 14.

All of these G-codes are modal and belong to the same modal group.

21-4

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.3

TTRC Direction

G42; Compensation

right

G40; Compensation

cancel

Programmed tool path

and direction

G41; Compensation

left

Important: The TTRC function is not available during any of the thread

cutting cycles. TTRC must be canceled before any threading routine can

be performed.

Program the TTRC function with this format:

G41(or G42)X ___ Z ___ T ___ ;

Where :

Is :

G41(or G42)

TTRC direction, G41=left, G42=right

X, Z

End-point of entry move into TTRC. Program an entry move only on

axes in the currently active plane. Axis motion must take place in

order for TTRC to be active on an axis.

T

Designates the offset numbers and pulls data: 1) from the wear and

geometry tables for the tool radius, and 2) from the geometry table for

tool orientation. See chapter 20 for information on programming a

T-word. The T-word is optional in the G41 or G42 blocks. The T-word

may also be designated in any previous or following program block.

21-5

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Important: The TTRC feature is not available for any motion blocks that

are programmed in MDI mode. See page 21-30. The TTRC mode can be

altered by programming either G41, G42, or G40, or the tool radius can be

changed in an MDI program. However, none of the tool paths executed in

MDI will be compensated. Any changes made to TTRC are not applied

until the next block executed in automatic mode.

Figure 21.4

Tool Radius Wear

WEAR = R’- R

Cutting edge before

tool wear

R’

Worn cutting

R

edge

G40 (TTRC cancel) is active when power is turned on, when E-STOP is

reset, when the control is reset, or when an M02 or M30 end-of-program

block is executed.

Example 21.2

Tool Tip Radius Compensation Sample Path

Assume: T01 = 5mm tool radius total from both geometry and wear tables.

Also assume a tool orientation of 0.

Program Block

Comment

N1G00G42X30.Z35.T01;

rapid to start and set TTRC right

N2G01Z52.F.1.;

feed move to Z52

N3G03Z68.R15.;

arc of radius 15

N4G01.Z95.;

feed move to Z95

N5Z102.X18.;

feed move to Z102 X18

N6G40X0Z0;

exit TTRC

N7 M30

end of program

21-7

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.5

Results of TTRC Program Example

Cutting tool center path

X

N2

N4

N3

N5

N1

N6

start

Z

point

21.2

In certain instances, TTRC creates a non-programmed move called a

TTRC Generation Blocks

generated block. These blocks improve cycle time and corner-cutting

quality.

G39, G39.1

TTRC generates blocks for type A or B moves as follows:

Type of Move

Type A

Type B

Entry Move

No block is generated

Block is generated

Tool Path

Block is generated

Block is generated

Exit Move

No block is generated

Block is generated

Important: These blocks are created only if:

G41 is active and cutting an inside angle that is less than 90°

G42 is active and cutting an outside angle that is more than 270°

21-8

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

The generated block between the two tool paths can be programmed as

linear or circular with these G-codes:

G39(or G39.1);

Where :

Causes:

G39

linear transition blocks. If neither G39 or G39.1 is programmed, G39

is the default. This command is modal.

G39.1

circular transition blocks. When cutting straight line-to-arc or

arc-to-straight line moves, the generated block will always be linear,

and the G39.1 will be ignored. This command is modal.

Figure 21.6

TTRC Generated Blocks (G39 vs G39.1)

G39 (Linear generated block)

G39.1 (Circular generated block)

Start of

Linear

Start of

Circular

2nd cut

generated

2nd cut

generated

block

block

r

r

r

Programmed

r

r r

path

r

G42 Tool path

End of

End of

r

= Tool radius

1st cut

1st cut

G39 or G39.1 can be programmed in any block. However, they must be

programmed in or before the block that causes a TTRC generated block.

Important: For linear generated blocks, your system installer can define a

minimum block length in AMP. If the generated move length is less than

the system-defined minimum block length, no generated block is created.

The tool path proceeds to the intersection of the two compensated paths. If

the generated move length is equal to, or greater than, the system-defined

minimum block length, a generated block is created.

Throughout this chapter, we show drawings where a generated block is

created. Both G39 and G39.1 are shown in these drawings where

applicable.

21-9

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

21.3

The easiest way to demonstrate the cutting tool’s the actual tool paths when

using TTRC type A is by pictorial representation. The following

TTRC Tool Paths (Type A)

subsections describe the cutter path along with a figure to clarify the

description

21.3.1

An entry move is defined as the path that the cutting tool takes when the

TTRC Type A Entry Moves

TTRC function first becomes activated in a program. Figure 21.7 shows a

typical entry move.

Figure 21.7

TTRC Entry Move

Programmed tool path

Cutting tool center path

Cutting tool

G42 TTRC right

Compensation entry move

Workpiece

Important: Any entry move into TTRC must be a linear move. Initial

activation of TTRC by designation of either the G41, G42, or T-word that

initializes TTRC in a circular cutting mode (G02 or G03) is not allowed.

The G41, G42, or T-word can be designated in a circular block to change

TTRC direction or tool radius, as long as TTRC is already active.

The entry move of the cutting tool for type A TTRC takes the shortest

possible path to its offset position. This position is at right angles to and

on the left or right side of the next programmed move in the currently

defined plane.

Figure 21.8 and Figure 21.9 show examples of typical entry moves using

type A TTRC.

21-10

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.8

Tool Path for Entry Move Straight Line-to-Straight Line

0

£q£90

90

£q£180

G41

G41

r

r

Programmed

Programmed

path

path

r

q

r

q

G42

G42

Start-point

Start-point

180

£q£270

270

£q£360

Start-point

Start-point

G41

G41

r

r

Programmed

Programmed

path

q

path

r

r

q

G42

G42

21-11

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

If the next programmed move is circular (an arc), position the tool at right

angles to a tangent line drawn from the start-point of that circular move.

Figure 21.9

Tool Path for Entry Move Straight Line-to-Arc

0

£q£90

90

£q£180

G41

G41

Programmed path

Programmed path

r

r

q

q

G42

r

r

G42

Start-point

Start-point

Start-point

Start-point

180

£q£270

270

£q£360

G41

G41

r

r

q

q

r

r

G42

G42

Programmed path

Programmed path

There is no limit to the number of blocks that can follow the programming

of G41 or G42 before an entry move takes place. The entry move will

always be the same regardless of the number of blocks that do not program

motion in the current plane for compensation.

21-12

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Example 21.3

Sample Entry Move After Non-Motion Blocks

Assume current compensation plane is the ZX plane.

N01X0Z0;

N2G41T1;

This block commands compensation left

N3M02;

This is not the entry block since no axis motion takes place in

the current plane.

N4...;

No axis motion in current plane.

N5...;

No axis motion in current plane.

N6...;

No axis motion in current plane.

”

”

”

”

”

”

N999X1Z1;

This is the entry move for the previously programmed G41.

Your system installer selects in AMP the allowable number of non-motion

blocks that is to be allowed during TTRC before the entry move must be

re-initialized. See page 21-30.

For example, assume that your system installer has designated that only

two non-motion blocks can be performed. Then, if more than two blocks

following the entry move do not contain axis motion in the current plane,

the entry move is re-performed at the next block containing axis motion in

the current plane.

Example 21.4

Too Many Non-Motion Blocks After Entry Block

Assume current plane to be the ZX plane.

N1X0.Z0.;

N2G41T1X1.Z1.;

Entry move TTRC left.

N3;

No axis motion in current plane.

N4...;

No axis motion in current plane.

N5X4Z-4;

New entry move TTRC left.

21-13

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.10

Results of Example 21.4

Too many non-motion

r

blocks here

Programmed

r

path

TTRC

reinitialized here

G41

r

r

r

21.3.2

Cancel the TTRC feature by programming G40. Refer to the path that is

TTRC Type A Exit Moves

taken when the tool leaves TTRC as the exit move. The path that the tool

follows during an exit move is dependant on:

The direction of compensation (G41 or G42).

The angle between the last motion made in TTRC (in the current

compensation plane) and the motion of the exit move.

Designating a tool offset number T00 in a program does not cancel TTRC

and does not generate an exit move. TTRC simply continues on as if a tool

radius had been changed to a radius of zero. See page 21-30 for

information about changing cutter radius. The exit move, if T00 is the

active tool radius, is the same path as the programmed tool path.

Important: An exit move cannot be a circular move (G02 or G03). Any

exit move must be programmed on a linear path. Any attempt to generate

an exit move by using a circular path generates a block-format error.

21-14

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.11 through Figure 21.15 show examples of typical exit moves

using type A TTRC. All examples assume that the number of non-motion

blocks before the designation of the G40 command have not exceeded the

number allowed as determined by your system installer in AMP.

Figure 21.11

Tool Path for Exit Move Straight Line-to-Straight Line

End-point

0

£q£90

0

£q£90

End-point

G42

r

G42

q

Programmed

r

q

r

path

Programmed

G41

r

path

G41

0

£q£90

0

£q£90

G42

G42

r

q

r

Programmed

Programmed

q

r

path

r

path

G41

G41

End-point

End-point

21-16

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

If the last programmed move is circular (an arc), positioning the tool at

right angles to a tangent line drawn from the end-point of that circular

move.

Figure 21.12

Tool Path for Exit Move Arc-to-Straight Line

0

£q£90

0

£q£90

G41

G41

Programmed path

Programmed path

r

r

q

q

G42

r

r

G42

Start-point

Start-point

Start-point

Start-point

0

£q£90

0

£q£90

G41

G41

r

r

q

q

r

r

G42

G42

Programmed path

Programmed path

The examples in Figure 21.11 and Figure 21.12 assume that the number of

blocks that do not contain axis motion, in the currently selected plane,

follow the G40 programming before an exit move takes place and does not

exceed an amount selected in AMP by your system installer. If the number

of non-motion blocks following G40 exceeds the limit, the control

generates its own exit move. This may often cause overcutting of the part.

You can modify the path that the tool takes for an exit move by including

an I- and/or K-word in the exit move. Only the I- or K-words that

represent values in the current plane are programmed in the block

containing the exit move. I and K correspond to the X and Z axes

respectively.

21-17

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

The I- and K-words in the exit move block define a vector that is used by

the control to redefine the end-point of the previously compensated move.

I- and K-words are always programmed as incremental values regardless of

the current mode (G90 or G91).

The vector defined by the I- and/or K-words is along a line drawn from the

end-point of the programmed path to a point referenced from the end-point

of the programmed path a distance along the axes in the current plane an

amount as designated with the I- and/or K-words. A new vector is then

defined parallel to the vector defined by the I- and/or K-word and offset

from this vector in the direction and amount of the currently active offset

(G41 or G42). The intersection of this new vector with the current

compensated tool path defines a point which is the new end-point of the

last programmed compensated move.

Figure 21.13

Exit Move Defined By An I, K Vector

Compensated path using I, K vector

Compensated path if no I, K in G40 block

Intercept line

I, K

r

Compensated path

Programmed path

r

Figure 21.13 is the exception. The change in length of the compensated

path is more than one radius of the tool. In this special case, this offset is

limited to one radius of the tool. The direction of the offset is towards the

point of intersection of the I K vector and the current compensated tool

path.

Example 21.6

Exit Move Defined By An I,K Vector But Limited To Tool Radius

Assume T1 radius is 3

N10 Z10.G41T1

N11 X10.Z2.I3K-10.G40;

21-18

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.14

Results of Example 21.6

Compensated path using I, K vector

Compensated path if no I, K in G40 block

N11

Compensated path

r

r

Programmed path

N10

r

I, K

Intercept line

If the vector defined by I and/or K is parallel to the programmed tool path,

the resulting exit move is offset in the opposite direction of the I and/or K

vector by one radius of the tool.

Figure 21.15

Exit Move When I, K Vector Is Parallel to Programmed Tool Path

Compensated path using I, K vector

Compensated path if no I, K in G40 block

Compensated path

r

r

Programmed path

Intercept line

I, K

r

Important: If one I and/or K value is programmed without the second one,

the value of the second I- and/or K-word defaults to 0.

21-19

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

21.4

We demonstrate the actual tool paths taken by the cutting tool when using

TTRC type B by pictorial representation. The following subsections

TTRC Tool Paths (Type B)

describe the cutter path along with a figure to clarify the description.

21.4.1

An entry move is defined as the path that the cutting tool takes when the

TTRC Type B Entry Moves

TTRC function first becomes activated in a program. Figure 21.16 gives

an example of a typical entry move.

Figure 21.16

TTRC Entry Move

Programmed tool path

Cutting tool center path

Cutting tool

G42 TTRC right

Compensation entry move

Workpiece

Important: Any entry move into TTRC must be a linear move. Initial

activation of TTRC by designation of either G41, G42, or T-word in a

circular cutting mode (G02 or G03) is not allowed. The G41 or G42

commands can be designated in a circular block to change TTRC direction,

or a new T-word can be designated to change cutter radius, as long as

TTRC is already active.

The entry move of the cutting tool for type B TTRC can generate extra

motion blocks to attempt to prevent gouging of the part as may sometimes

occur using compensation type A. Type B TTRC keeps the cutting tool at

least one radius away from the start-point of the next block at all times

during an entry move. The final end-point of the entry move is a position

at right angles to and on the left or right side of the next programmed move

in the currently defined plane.

21-20

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.17 and Figure 21.18 show examples of typical entry moves using

type B TTRC.

Figure 21.17

Tool Path for Entry Move Straight Line-to-Straight Line

G39 (Linear Generated Blocks)

G39.1 (Circular Generated Block)

0

£q £90

0

£q £90

E

C

D

D

r

G41

G41

r

r

C

Programmed

Programmed

r

r

q

path

q

path

r

r

r

G42

B

G42

r

B

Start-point

Start-point

A

A

180

£q £270

90

£q £180

A

Start-point

B

r

C

G41

r

Programmed

q

path

G41

r

r

G42

Programmed

q

path

r

G42

A

B

r

C

Start-point

G39 (Linear Generated Blocks)

G39.1 (Circular Generated Block)

270

£q £360

270

£q £360

A

A

Start-point

Start-point

B

r

G41

G41

B

r

r

r

r

C

Programmed

Programmed

r

q

path

q

path

r

r

G42

G42

r

E

D

C

D

21-21

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

If the next programmed move is circular (an arc), position the tool at right

angles to a tangent line drawn from the start-point of that circular move.

Figure 21.18

Tool Path for Entry Move Straight Line-to-Arc

G39 (Linear Generated Blocks)

G39.1 (Circular Generated Block)

0

£q £90

0

£q £90

r

r

r

r

q

r

q

r

r

r

r

G41

G41

Programmed path

Programmed path

G42

Start-point

G42

Start-point

Start-point

90

£q £180

180

£q £270

r

r

q

r

r

q

r

r

Programmed

Programmed path

Path

Start-point

G42

G41

G42

G41

G39 (Linear Generated Blocks)

G39.1 (Circular Generated Block)

270

£q £360

270

£q £360

Start-point

Start-point

r

r

r

r

q

q

r

r

r

r

r

G41

G41

Programmed path

Programmed path

G42

G42

21-22

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

There is no limit to the number of blocks that can follow the programming

of G41 or G42 before an entry move takes place. The entry move is

always the same regardless of the number of blocks that do not program

motion in the current plane for compensation.

Example 21.7

Sample Entry Move After Non-Motion Blocks

Assume current compensation plane is the ZX plane.

N01X0Z0;

N2G41;

This block commands compensation left.

N3M02;

This is not the entry block since no axis

motion takes place in the current plane.

N4...;

No axis motion in current plane.

N5...;

No axis motion in current plane.

N6...;

No axis motion in current plane.

”

”

”

”

”

”

N999X1Z1;

This is the entry move for the previously

programmed G41.

Your system installer selects in AMP the allowable number of non-motion

blocks that are allowed during TTRC before the entry move must be

re-initialized. See section 22.5.2.

For example, assume that your system installer has designated that only

two non-motion blocks can be performed. Then, if more than two blocks

during TTRC do not contain axis motion in the current plane, the entry

move is re-performed at the next block containing axis motion in the

current plane.

Example 21.8

Too Many Non-Motion Blocks During TTRC

Assume current plane to be the ZX plane and the system installer has

designated that only two non-motion blocks can be performed before

TTRC is re-initialized.

N1X0Z0;

N2G41X1Z1;

Entry move TTRC left.

N3...;

No axis motion in current plane.

N4...;

No axis motion in current plane.

N5X4Z-4;

New entry move TTRC left.

21-23

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.19

Too Many Non-Motion Blocks

Too many non motion

r

Programmed

r

blocks here

path

TTRC

reinitialized here

G41

r

r

r

21.4.2

Program a G40 to cancel the TTRC feature. Refer to the path that is taken

TTRC Type B Exit Moves

when the tool leaves TTRC is referred to as the exit move. The path that

the tool follows during an exit move is dependant on:

The direction of compensation (G41 or G42).

The angle between the last motion made in TTRC (in the current

compensation plane) and the motion of the of the exit move.

Designating a tool offset number T00 in a program does not cancel TTRC

and does not generate an exit move. TTRC simply continues on as if a tool

radius had been changed to a radius of zero. See page 21-30 for

information about changing cutter radius). The exit move (if T00 is the

active tool radius) is then equal to the programmed tool path.

Important: An exit move cannot be a circular move (G02 or G03). Any

exit move must be programmed on a linear path. Any attempt to generate

an exit move by using a circular path generates an error.

21-24

Chapter 21

Tool Tip Radius Compensation (TTRC)

Function

Figure 21.20 and Figure 21.21 show examples of typical exit moves using

type B TTRC. All examples assume that the number of non-motion blocks

before the designation of the G40 command has not exceeded the number

allowed as determined by your system installer in AMP.

Figure 21.20

Tool Path for Exit Move Straight Line-to-Straight Line

G39 (Linear Generated Blocks)

G39.1 (Circular Generated Block)

0

£q £90

0

£q £90

E

D

End-point

End-point

D

G42

r

G42

C

r

r

r

q

Programmed

r

q

Programmed

r

C

path

path

r

r

G41

G41

B

r

A

B

A

90

£q £180

180

£q £270

End-point

C

A

B

r

G42

r

q

Programmed

G42

path

r

r

q

G41

Programmed

path

r

G41

B

r

A

C

End-point

G39 (Linear Generated Blocks)

G39.1 (Circular Generated Block)

270

£q £360

270

£q £360

B

r

A

B

A

G42

G42

r

r

q

Programmed

q

Programmed

C

path

r

path

r

r

r

r

G41

G41

r

C

D

End-point

End-point

D

E

21-26

Content      ..     15      16      17      18     ..