9/Series CNC Lathe. Operation and Programming Manual

Chapter

Chamfering and Corner Radius

16.0

During cornering, the 9/Series control has the option of performing either a

chamfer (a linear transition between the blocks) or a corner radius (an arc

Chapter Overview

transition between blocks).

Chamfer size

This word is used to define a chamfer length that connects two

intersecting tool paths. This word determines the distance that

the chamfer begins and ends from the tool paths intersection.

Corner radius

This word is used to define the radius of an arc that is tangent

to two intersecting tool paths.

This chapter describes chamfering and corner radius in detail. Major

topics include:

Topic:

On page:

Chamfering

16-2

Corner radius

16-4

Both the chamfer and the corner radius features are generated between two

motion blocks that must be programmed in the same plane. The motion

block with the corner chamfering (,C) or the corner radius (,R) word is

defined as the first cornering block. The next motion block in the

cornering plane is defined as the second block.

If more than one ,C- or ,R-word is programmed in the same block, only the

right-most word is used; others are ignored. The second block can also

have a corner chamfering or corner rounding word in it. If it does, the

second block is also used as the first block of the next corner chamfering

or corner rounding.

CAUTION: If you make a programming error of some type is

made in the block defining the second tool path in the chamfer

or radius blocks, the control is not able to cut the correct

chamfer or radius. Instead, the first block is executed to its

programmed endpoint. This can cause damage to the part or

cutting tool.

16-1

Chapter 16

Chamfering and Corner Radius

There is a limit of 4 non-motion blocks allowed between the first and

second motion blocks defining the corner transition. A non-motion block

is any block that does not generate axis motion in the currently active

plane. The control generates an error if more than 4 non-motion blocks are

programmed between the cornering plane.

Use the chamfering and corner radius features are often used in

conjunction with QuickPath Plus. They can be programmed in either

absolute (G90) or incremental (G91) modes.

16.1

Program a chamfer size following the address ,C to cut a chamfer between

Chamfering

consecutive tool paths. The chamfer word must follow a comma (,) and is

programmed in the first of two paths connected by the chamfer. The value

following the ,C address is the amount of tool path cut of each

programmed tool path by the chamfer. The angle that the chamfer makes

with the tool paths is dependant on the size of the chamfer.

Measure the chamfer size from the intersection of the two blocks.

If the block:

Then:

linear

distance programmed with the ,C-word is measured from the

intersection of the two tool paths along the linear path.

circular

then the chamfer distance programmed is applied as a chord length

on the arc measured from the intersection between the two blocks.

This applies regardless of the combination of arcs and lines to be

chamfered.

The ,C-word can be programmed any where in a block as long as no space

is programmed between the comma and the chamfer distance.

Example 16.1

Basic Chamfering Using ,C

N10 Z25.0 X0.0 F.1.;

N20 G01X20.,C5.0;

N30 Z5.0;

16-2

Chapter 16

Chamfering and Corner Radius

Figure 16.1

Results of Chamfering Using ,C from Example 16.1

2.0

20.0

Example 16.2

Linear to Circular Motions with Chamfer

N10X0.Z0.F.1;

N20X10.Z10.,C5;

N30G02X20.Z20.R10;

Figure 16.2

Results of Linear to Circular Motions with Chamfer, Example 16.2

N30

Actual start point of

Chamfer

block N30 and end

point of chamfer block

block

C (chord length)

Programmed end point

of block N20

N20

Actual end point of block N20 and

start point of chamfer block

16-3

Chapter 16

Chamfering and Corner Radius

16.2

Use the ,R command to program a radius between two intersecting tool

paths. The R command must be programmed after a comma (,). Program

Corner Radius

the ,R followed by the radius size in the block where the first path is

programmed. The control looks ahead to the block commanding the

second path and automatically inserts the circular rounding bock to meet

that path. This inserted circular block is always tangent to both

programmed tool paths. If the control cannot generate an arc that is

tangent to both paths with the programmed ,R, then the control generates

an error.

Block:

Description:

The first corner radius

always terminates at the point on the block where the rounding block

is tangent to the first block

The rounding

terminates at the point where the generated rounding block is tangent

to the second rounding block.

The second rounding

starts from the end point of the generated circular block and continues

on to the programmed end point of the second block.

The R-word can be programmed any where in a block as long as no space

is programmed between the ,R and the radius length.

Important: If the two motion blocks are tangent to each other, then any

corner rounding commands are ignored.

Example 16.3

Programming a Radius for a Circular Path into a Linear path.

N10Z10X30.F.1;

N20G02X10.Z10.R10,R3;

N30Z30.X10.;

16-4

Chapter 16

Chamfering and Corner Radius

Figure 16.4

Results of Radius and Chamfer, Example 16.4

5.0

20.0

10.0

R 5.0

2.0

40.0

20.0

16.3

When using chamfering and corner radius, remember:

Considerations with

If the control is executing in single block mode, the control enters the

Chamfering and Corner

cycle stop state after executing the first block and the adjacent chamfer

Radius

or corner radius.

If non-motion blocks are programmed separating the two intersecting

blocks for the corner radius and chamfer features, the control executes

the chamfer or radius immediately after the first block. The non-motion

blocks are executed after the control has executed the chamfer or radius.

Any negative signs programmed with the ,C- or ,R-words are ignored.

Use the absolute value of the word to cut the chamfer or radius. For

example ,C-10 is used as ,C10.

An error is generated if the length of a chamfer is larger than the

programmed length of the first or second move, or for corner rounding

if the programmed corner radius is so large that the tangent point on

both of the two programmed blocks does not exist.

An error is generated if you attempt to change planes between blocks

that are chamfer or corner radius blocks.

16-6

Chapter 16

Chamfering and Corner Radius

You must program ,C and ,R in blocks that contain axis motion in the

current plane. If they are programmed in a block that does not contain

axis motion in the currently active plane, the control generates an error.

,C and ,R cannot be programmed in a block that contains any of the

following:

- Any fixed cycle G-codes

- Any dwell commands

- Thread cutting blocks

- Programmable zone G-codes

Your system installer determines in AMP the resolution of the ,C- and

,R-words for both inch and metric programming. Refer to

documentation prepared by your system installer for details.

END OF CHAPTER

16-7

Chapter

Spindles

17.0

This chapter describes spindle speed control, orientation, and direction, and

the virtual C axis.

Chapter Overview

Topic:

See page:

Spindle Speed Control

17-1

Controlling Spindles (G12.1, G12.2, G12.3)

17-9

Spindle Orientation (M19, M19.2, M19.3)

17-10

Spindle Direction (M03, M04, M05)

17-12

Virtual C Axis

17-13

Synchronized Spindles

17-23

If you are using a dual-processing system, spindle control is different.

Refer to page 30-13 for details.

17.1

Relative speed of the revolving workpiece to the cutting tool tip is referred

Spindle Speed Control

to as the cutting speed. Required cutting speeds can be attained by

designating proper spindle speeds. Figure 17.1 illustrates the relationship

between workpiece diameter (D), spindle speed (N) and cutting speed (V).

Figure 17.1

Relationship between Cutting Speed, Spindle Speed, and Diameter

Nrpm

Chuck

Vm/_min

D Diameter

Workpiece

17-1

Chapter 17

Spindles

In this case, cutting speed V is expressed with this equation:

V = (3.14159)(D)(N)/1000

To cut a 150-mm-diameter workpiece at a cutting speed of 200 m/min, the

spindle speed to provide the required cutting speed is calculated to be

approximately 1325 rpm using the above equation. This means that by

designating “S1325;” in a part program, cutting is conducted at a cutting

speed of 200 m/min.

When cutting tapers, which have different workpiece diameters at different

cutting points, spindle speeds need to vary during the cutting process to

maintain proper cutting speed. To compensate for this problem, the control

has a feature to allow designating the required cutting speed V, directly in a

part program. With this feature, the control changes spindle speed as the

diameter of the workpiece changes to maintain a fixed cutting speed. This

feature is referred to as the “constant surface speed mode” or CSS.

The spindle function has two modes:

Constant Surface Speed Mode (G96) maintains a workpiece’s speed

across a tool equal to a desired cutting speed dependent on the working

diameter. See page 17-3.

Constant Spindle RPM Mode (G97) maintains a constant spindle speed

equal to the programmed S-word making cutting speed independent of

the working diameter. See page 17-9.

Spindle Speed (S-word)

Use the S-word to program the spindle speed for all configured spindles.

The common S-word can be applied per spindle by associating the S-word

in the same block with the spindle directional M-codes. See page 17-12

for information about spindle directional M-codes. If no directional

M-code is programmed in the block with the S-word, then the S-word is

applied to the active controlling spindle.

CAUTION: The displayed S-word always shows the

controlling spindle’s programmed spindle speed. When the

non-controlling spindles are configured, their S-word display

must be handled by some other means. See the system

installer’s documentation for display capabilities of the active

spindle speed for auxiliary spindles.

17-2

Chapter 17

Spindles

The S-word units represent revolutions per minute (RPM) in most cases.

Only during CSS programming are the S-word units different. While CSS

mode is active, the S-word units represent surface feet per minute. Only

the controlling spindle can change its S-word mode from RPM to CSS.

17.1.1

The G96 command maintains a constant cutting speed (programmed by the

S parameter) by monitoring the cutting tool’s position with respect to the

Constant Surface Speed

center line of the spindle.

Mode (G96)

In the G96 mode the S-word is used to program the cutting speed. Actual

units for the S-word are surface meters per minute in metric or surface feet

per minute in the inch system. To maintain a cutting speed of 200 m/min,

for example, write the program as:

G96 S200;

G96 mode must also first be enabled by programming an M58 code. See

the notes on CSS on page 17-6 for details. The G96 code is modal and

remains active until it is cancelled by the G97 code or disabled with an

M59 code.

Important: When changing from G97 to G96 mode, if an S-word is

specified in the G96 block, the cutting speed changes to the value indicated

by the S-word. If no S-word is contained in the G96 block the control uses

the current cutting speed of the tool as the CSS cutting speed. The spindle

speed then changes relative to the tool position to maintain this CSS

cutting speed.

Important: The system installer determines in AMP what axis is used to

determine the cutting diameter. The programmer has the option of

changing the diameter axis by programming a P-word when in the G96

mode. P-words range from P1 to P9. A P-word to change diameter axis

may be programmed in any block where in the G96 mode as long as that

block does not contain a dwell. Refer to the system installer’s

documentation for details on what P-word programs the axis that is

perpendicular to the part diameter. Normally the P-word is not

programmed for CSS. If not programmed the system installer’s default

axis is used. This manual assumes the X axis determines the cutting

diameter.

Your system installer determines CSS axis assignment in AMP. You can

change the CSS axis by programming a P-word (P0 through P9) in the

G96 block when activating CSS.

17-3

Chapter 17

Spindles

Each P-word corresponds to a specific axis assigned to it in AMP. Any

CSS axis changes made by programming a P-word in the G96 block

remain in effect regardless of what mode the control is in. The default

CSS axis is assigned to P0 and is active on power-up and after a control

reset.

Use this equation to calculate constant surface speed:

N = K V/D

RPM = Surface speed per minute / (.262 x diameter)

Where :

Is :

Spindle speed (rpm)

Constant 318.31 (1000/p) for metric system or 3.8197 (12/p) for inch system

Surface speed (m/min or feet/min)

Cutting diameter (mm or inch)

Figure 17.2 shows how the spindle speed changes as the cutting diameter

changes when:

constant K is 318.31

the necessary surface speed is 200 m/min

the maximum spindle speed is 3500 rpm

17-4

Chapter 17

Spindles

Figure 17.2

Constant Surface Speed Mode (G96)

Chuck

Æ 200

Æ 100

CAUTION: During the blocks when CSS mode (G96) is

active, the programmed S-word units are surface speed per

minute. For systems allowing multiple spindles, when CSS is

active, the S-word units for all spindles is surface speed per

minute. To maintain RPM units on the non-controlling

spindles, do not program them while CSS is active on the

controlling spindle.

Cutting Tool Position

Cutting Diameter (mm)

Spindle Speed (rpm)

200

318

100

636

3500 *

* The calculated spindle speed would be infinite because the diameter of

the workpiece at cutting position 3 is zero (0). However, since the

maximum spindle speed is set in AMP, the control sets the spindle speed at

this maximum value.

17-5

Chapter 17

Spindles

Important: If it is desirable to prevent the spindle speed from reaching a

maximum RPM a ceiling can be placed on the spindle speed at a rate

below the maximum AMP setting. For details, see the CSS notes on page

17-6.

Relationships between spindle speeds and cutting diameters are shown in

Table 17.A for different surface speeds.

Table 17.A

Spindle RPM as related to cutting diameter and programmed CSS

Programmed Surface Speed, Feet/min. (meters/min.)

100(30)

200(61)

300(91)

400(122)

500(152)

1000(305)

1500(457)

2000(610)

1(25)

382

764

1146

1527

1910

3820

5730

7640

2(51)

191

382

573

764

955

1910

2865

3820

3(76)

127

254

382

509

637

1273

1910

2546

4(102)

191

286

382

477

955

1432

1910

5(127)

153

229

306

382

764

1146

1528

Cutting

6(152)

127

191

255

382

637

955

1273

Diameter,

8(203)

143

191

239

477

716

955

Inches

10(254)

115

153

191

382

573

764

(mm)

12(305)

127

159

318

477

637

14(356)

109

163

273

409

546

16(406)

143

239

358

477

18(457)

127

212

318

424

20(508)

115

191

286

382

25(635)

153

229

306

30(762)

127

191

255

Notes on Constant Surface Speed

Normally the system installer sets a maximum speed in AMP; however,

the programmer has the option of lowering this maximum speed if

desired. An allowable upper limit for RPM can be programmed by a

G92 followed by an S value in RPM. This upper limit is valid only for

the G96 mode and is ignored in G97 mode. The value for this upper

limit can not exceed the value set in AMP for the maximum spindle

RPM.

To enter 3500 rpm as the upper limit, program:

G92S3500;

17-6

Chapter 17

Spindles

In G96 mode, spindle speeds increase as the workpiece diameter

decreases. When the spindle speed reaches the upper limit, it is held at

this value even if the theoretical spindle speed exceeds that value. This

maximum RPM may also be affected by the maximum gear speed set

for a specific gear in AMP.

Important: The G92s command to set a new max spindle RPM in CSS

may not be programmed while CSS is active.

Important: The G92, maximum spindle RPM limit for CSS,

programmed in a block is applied as the CSS limit for the currently

active controlling spindle (selected with the G12 code). For systems

allowing multiple spindles, if the controlling spindle is changed between

the G92 and CSS activation, then the required G92 limit may not be

active for the proper spindle.

The G92 maximum spindle RPM is canceled only after power is shut

down, a control reset is performed, or when the control goes into

E-STOP. M02 or M30 cannot cancel this value. When canceled, the

system installers maximum speed becomes effective again.

Spindle speed during rapid traverse

In the G96 mode, when rapid axis feed starts, spindle speeds are

controlled in one of two ways:

The spindle speed changes as X axis moves.

The control calculates the spindle speed attained at the end of the move

and uses that spindle speed for the entire rapid move.

The system installer selects in AMP which spindle speed control type he

wants.

Activating and deactivating CSS mode with M-codes (M58/M59)

Use M58 or M59 to turn constant surface speed mode on or off.

When M59 is programmed, the control ignores G96 mode and the

spindle revolves at the same speed as when this M-code is executed.

When M58 is executed, the G96 mode becomes active again.

If an S-code is programmed in the same block as an M59, G96 mode is

ignored and the S-code value is registered in memory as a constant

surface speed S-code, but the spindle speed does not change with

diameter.

17-7

Chapter 17

Spindles

When programming M58, the M59 code is cancelled and the G96 mode

becomes active again. The spindle maintains the same surface speed

that was in effect prior to the execution of M59 unless an S-code was

specified in the M59 block.

CAUTION: Restoring the constant surface speed mode might

cause the spindle speed to change rapidly depending on the

cutting tool position.

Displayed spindle speed during CSS

The CRT display normally shows the current spindle speed in RPM

following the S-word. This is true during CSS also. The display shows

the actual spindle RPM, not the surface speed.

CSS R-word programming

The optional R-word lets you specify a surface footage value to be

applied at a point other than the current axis position. The R-word

defines the incremental distance from the current tool tip to the spindle

centerline. The sign of the R-word defines on which side of the spindle

centerline the tool tip is positioned.

The R-word is recognized only in a G96 block; its value is valid as long

as CSS mode is active and may only be changed when a G96 is

programmed in the block.

If you change the S-word (surface footage) while in G96 mode and if an

R-value was previously programmed in a G96 block, the R-value is not

cancelled.

Important: An R0 and no R-word do not mean the same thing. An

R-word of zero means that the spindle centerline is the tool tip position.

No R-word means to use the current position.

17-8

Chapter 17

Spindles

17.1.2

In the G97 mode, the spindle revolves at the programmed RPM regardless

of the position of the cutting tool.

RPM Spindle Speed Mode

(G97)

For example, to revolve the spindle at 500 rpm, program:

G97 S500 M03;

The G97 code is modal and remains active until it is cancelled by the G96

code.

Important: If an S-word is specified in the G97 block when you change

from G96 to G97 mode, the control uses the S-word as the new RPM

value. If no S-word is contained in the G97 block, the control uses the

current RPM of the tool as the programmed spindle RPM. The spindle

speed then remains at this constant RPM.

17.2

Use the G12 code to program the active controlling spindle for all

Controlling Spindles

programmed axes motions for features and modes requiring spindle

operation. The G12 code is modal as only one spindle can be the

(G12.1, G12.2, G12.3)

controlling spindle. All other spindles are auxiliary spindles.

G12.1 — Spindle 1 Controlling

G12.2 — Spindle 2 Controlling

G12.3 — Spindle 3 Controlling

Table 17.B lists the allowed spindle capabilities.

Table 17.B

Spindle Capabilities

Control Type

Number of Spindles

Spindle Type

9/230 or 9/240

Primary

9/260

Primary

Auxiliary 2

9/290

Primary

Auxiliary 2

Auxiliary 3

The spindle 1, as well as spindle 2 and 3, must be configured in AMP, and

the associated spindle parameters must be set properly to provide for the

required spindle functions.

17-9

Chapter 17

Spindles

For systems with no spindle configured, simulated spindle feedback is

provided for the primary spindle. This allows all control features that

require spindle feedback, i.e., IPR feedrate, threading, CSS, to simulate the

feedback from a spindle even through the AMPed system configuration

contained no spindle. The default is 4000 count-per-rev device.

Important: On the 9/260 and 9/290 controls, if the auxiliary spindles are

programmed but have not been configured as active through AMP, these

errors are given as decode errors on any blocks that have the G12.2 or

G12.3 code:

“SPINDLE 2 NOT CONFIGURED” and/or

“SPINDLE 3 NOT CONFIGURED”

17.3

For each possible spindle configured, the control is equipped to perform a

Spindle Orientation

spindle orient operation. This operation is used to rotate the spindle to a

given angle. Typically this may be used to orient the spindle for

(M19, M19.2, M19.3)

load/unload operations, to position a chuck for automatic chuck wrench

operation, etc. This orient operation is not the same as using a spindle as

an axis for positioning. See virtual C axis, section 17.5. An orient

operation is performed separately from axis motions and cannot be

interpolated with normal axis motions.

There are two types of spindle orients available. They are:

Open-loop orient - The spindle does not use a feedback device for this

type of orient. The final destination of the spindle when performing an

open-loop orient is determined by PAL. Typically there is some form of

hardware switch used to determine the spindle is at the proper position.

When the open-loop orient is performed the spindle is turned at an

AMP-defined RPM and in an AMP-defined direction.

Closed-loop orient - The spindle must be equipped with a feedback

device. The final destination of the spindle when performing a

closed-loop orient may be determined in AMP, or entered in a program

block requesting an orient. When the closed-loop orient is performed,

the spindle is positioned at an AMP-defined RPM.

If the spindle is:

the orient will:

turning

complete in the same direction as the spindle is currently revolving.

If the spindle is turning faster than the orient speed defined in AMP, it

first slows to that orient speed before performing the orient.

not turning

be performed in whichever direction that results in the spindle

reaching the required position by using the shortest angular distance.

17-10

Chapter 17

Spindles

Important: A spindle orient is also sometimes automatically requested by

the control when performing some of the drilling cycles described in

chapter 26. This drilling cycle orient orients to either the AMP-defined

position if using a closed-loop orient type or to the position defined as the

open-loop orient position.

Important: In systems allowing multiple spindles (9/260 ad 9/290), only

one M19 code can be in a block. If two or more M19 codes appear in one

block, e.g., M19.2 M19#, this error message appears, “ONLY ONE M19

ALLOWED PER BLOCK.”

Refer to your system installer’s documentation to determine which orient

your system is equipped to perform. This manual assumes that a

closed-loop type orient is available. If an open-loop orient is used, refer to

the system installer’s documentation for details on its operation, as it is

highly PAL dependant.

Both open- and closed-loop spindle orients can be requested either by

programming the appropriate spindle orient code (M19, M19.2, M19.3) in

a program block, or by requesting one through PAL. If closed-loop orient

is requested through PAL, the orient angle is fixed at the default orient

angle preset by the system installer in AMP.

If a closed-loop orient is requested by programming the appropriate

spindle orient code (M19, M19.2, M19.3), the option exists to orient the

spindle to the AMP-defined orient position or to a position programmed

with an S parameter in the M19 block. The S parameter defines an angle

at which the spindle is positioned relative to an angle of zero that is fixed

for a specific machine. Refer to the documentation prepared by the system

installer. This S parameter always programs an absolute angular position.

The angle programmed is not affected by incremental or absolute

programming mode (if open-loop orient is being used, the value

programmed with the S parameter is ignored).

The M19 code is modal. However, each time it is necessary to orient to a

specific angle, an M19 with an S-word must be programmed.

Programming an S-word alone replaces the current modal spindle speed

used later when the M19 mode is canceled. Cancel the M19 spindle orient

by programming one of the other spindle mode M-codes.

17-11

Chapter 17

Spindles

To cancel spindle orient:

Program:

Meaning:

Spindle 1

M03

Spindle 1 clockwise

code M19

M04

Spindle 1 counterclockwise

M05

Spindle 1 stop

Spindle 2

M03.2

Spindle 2 clockwise

code M19.2

M04.2

Spindle 2 counterclockwise

M05.2

Spindle 2 stop

Spindle 3

M03.3

Spindle 3 clockwise

code M19.3

M04.3

Spindle 3 counterclockwise

M05.3

Spindle 3 stop

17.4

Use the spindle directional M-codes to program each configured spindle

Spindle Direction

program controlled spindle rotation.

(M03, M04, M05)

Table 17.C lists the spindle direction codes.

Table 17.C

Spindle Directional Codes

Spindle Type

Directional Code

This means:

Primary

M03

Spindle 1 clockwise

M04

Spindle 1 counterclockwise

M05

Spindle stop

Spindle 2

M03.2

Spindle 2 clockwise

M04.2

Spindle 2 counterclockwise

M05.2

Spindle 2 stop

Spindle 3

M03.3

Spindle 3 clockwise

M04.3

Spindle 3 counterclockwise

M05.3

Spindle 3 stop

Each spindle can have independent rotational control, and the rotational

speed is programmed by using the S-word. If a directional spindle code is

programmed in the same block as the S-word, then that S-word is applied

to each of the block’s associated spindles.

17-12

Chapter 17

Spindles

Example 17.1

9/290 Control with 3 Spindles Configured in AMP

N0001 M05

Spindle 1 stop

N0002 M05.2 M05.3

Spindles 2 & 3 stop

N0003 M03 M04.2 S150

Spindle 1 clockwise 150 rpm

Spindle 2 counterclockwise 150 rpm

N0004 M03.2 M03.3 S10

Spindle 2 clockwise 10 rpm

Spindle 3 counterclockwise 10 rpm

Important: On the 9/260 and 9/290 controls, if the auxiliary spindle

directional M-codes are programmed but the auxiliary spindles have not

been configured as active through AMP, these errors are given as decode

errors on any blocks that have directional M-codes of the associated

spindle programmed:

“SPINDLE 2 NOT CONFIGURED” and/or

“SPINDLE 3 NOT CONFIGURED”

17.5

The Virtual C Axis feature allows the control to interpolate a rotary axis

(typically the lathe spindle) with the machine axes. This allows for

Virtual C Axis

circular machining along the circumference or across the face of a

workpiece while it is rotated, as shown in Figure 17.3 and Figure 17.5.

If the spindle is used as the virtual C axis, it may require that an alternate

motor and/or higher precision feedback device be used. The alternate

motor would be configured as a closed-loop rotary axis. Refer to the

documentation provided by your system installer.

This description assumes that the lathe spindle has been configured in

AMP to be used as the virtual C axis.

We refer to this axis:

As:

the virtual C axis

the axis along the spindle center line (also called the park axis)

the axis perpendicular to the spindle center line (also called the feed axis)

Refer to the literature provided by your system installer for the axis names

used by your machine.

17-13

Chapter 17

Spindles

To function as a virtual C axis, the lathe spindle must have a precision

encoder that provides position data to the control. There can be only one

encoder marker per revolution of the spindle. When the virtual C axis

feature is activated, the control switches spindle operation from an

open-loop spindle to a closed-loop virtual C positioning axis.

CAUTION: It is the responsibility of the operator (or the

control’s PAL program) to change spindle gears as required to

attain one revolution of the encoder per revolution of the

spindle prior to execution of the G16.1.

While the virtual C axis feature is active, programmed spindle commands

(M03, M04, M05, or M19) do not affect the operation of the lathe spindle.

It is up to the control’s PAL program to interpret these part program

commands and take appropriate action, such as directing them to a “live

tool” spindle.

Typically a live tool powered by an external drive and mounted on the X

and Z axes is used to machine contours on the workpiece during virtual C

operation. Operation of the live tool is controlled through PAL.

The control uses the $VIRTC PAL flag to indicate to PAL that the virtual C

axis feature is active. Refer to the documentation prepared by your system

installer for details.

Virtual C Programming Restrictions

When the virtual C axis feature is enabled, these programming restrictions

apply:

The control must be in feedrate per minute mode (G94), not feedrate per

revolution mode, before beginning virtual C programming

Work coordinate system offsets (G52, G54--G59, and G92) for the park

and feed axes (Z and X) are temporarily cancelled when in G16.1 mode.

Offsets for other axes are not affected

Tool offsets and cutter compensation/TTRC offsets are allowed during

Virtual C programming

Cutter compensation ignores the tool orientation and treats the

programmed tool as a mill tool (orientation 0)

Activation of offsets through PAL is disabled

Jog on the fly is disabled

Integrand circle/arc programming is not permitted during G02/G03

blocks. Only direct radius (R) programming is allowed

17-14

Chapter 17

Spindles

Only the primary spindle (selected with G12.1) can be used in coordination

with virtual C. On systems allowing auxiliary spindles, if the auxiliary

spindle is the controlling spindle when virtual C is activated, this error

message appears, “ILLEGAL CODE DURING VIRTUAL C.”

17.5.1

Cylindrical interpolation coordinates the motion of the virtual C axis with

that of the linear machine axes to machine contours on the side of a

Virtual C Axis,

cylindrical workpiece as shown in Figure 17.3. Virtual C cylindrical

Cylindrical Interpolation

interpolation mode is turned on using a G16.1 block and turned off with a

G15 block (or a G16.2 block requesting end face milling). A G15 block

can not contain any axis words.

Figure 17.3

Virtual C Axis Cylindrical Interpolation

Lathe Live Tool

The following are not allowed during cylindrical interpolation:

automatic motion to and from home G27, G28, G29, or G30

work coordinate changes and shifts G53, G54-G59, G59.1, G59.2,

G59.3, G50/G92, G52, G92.1

all turning and threading cycles

all drilling, tapping, and boring cycles

Cylindrical Interpolation Block Format

The format for the G16.1 block (virtual C axis cylindrical interpolation) is:

G16.1 R__ F__; C__ Z__;

17-15

Chapter 17

Spindles

Where:

Is:

the radius at which the feed axis (typically the X axis) is positioned at the start of

cylindrical interpolation. Can be used to alter the feed axis depth if programmed in a

G16.1 block during cylindrical interpolation.

the angular coordinate (if in G90 absolute mode) or the angular distance (if in G91

incremental mode) to which the virtual C axis is to move.

the coordinate (if in G90 absolute mode) or the linear distance (if in G91 incremental

mode) to which the Z axis is to move.

the feedrate to be used by the feed axis to position to radius R, and used by the Z axis

when commanded to move while G16.1 is active.

It also controls the virtual C axis speed as though it were a rotary axis. See chapter 18.

These parameters and their application are described in detail in the

paragraphs that follow:

The valued entered for the R parameter should place the tool at the radius

of the desired cutting depth into the part.

Important: R must be programmed in the initial G16.1 block. If R is not

programmed in the initial G16.1 block, the error message “CYLINDER

RADIUS IS ZERO” appears. At power turn-on, program-end (M02, M30,

or M99) or control reset, the virtual C axis feature is turned off and the R

value is set to zero. It must then be re-entered in the next G16.1 block.

The radius specified by the R parameter is modal and does not need to be

included in subsequent cylindrical interpolation blocks. Programming a

G16.1 block with a different R value modifies the feed depth to the new

radius. Feed depths cannot be changed using the X parameter when G16.1

is active. Programming an X generates the error message “FEED AXIS

MOTION NOT ALLOWED.”

Figure 17.3 illustrates the tool position if the AMP parameter Feed Axis

Park Location is selected as “Farthest from Machine Zero.” If “Nearest

to Machine Zero” were selected, then the tool would be positioned for

cutting into the part from the negative side of the X axis. Refer to the

information provided by your system installer.

A C or Z axis position may be programmed with the R parameter in the

initial G16.1 block. However, once G16.1 mode is established, only the Z

parameter can be programmed in the same block as the R parameter.

When it is, the Z axis motion executes first followed by feed axis motion to

radius R.

If a C axis position is programmed, the C axis rotates to the specified

angle. If the C and Z axes are programmed together in the same block,

then a vector motion results around the circumference of the part.

17-16

Chapter 17

Spindles

If G02 or G03 circular interpolation is made active while in G16.1

cylindrical interpolation mode, a circular cut can be made around the

circumference of the part (such as the shape cut in Figure 17.3). This is

accomplished by programming the C and Z axis endpoints along with the

desired circle radius R as described in chapter 14. The R parameter now

defines the radius of the circular path to be cut, not the feed axis position.

Important: When programming circular interpolation in G16.1 mode,

only radius programming (using R) may be used. Integrand programming

(using I, K) is not allowed and generates the error message “CIRCLE

PROGRAMMING ERROR.” See chapter 14.

Important: C axis motion is programmed as an angular value. When

programming circular interpolation in G16.1 mode, this angular value has

to be derived from a C axis arc length (based on the cutting radius). Refer

to Example 17.2.

To perform G02/G03 circular interpolation while in G16.1 mode, the linear

axis (Z) and the virtual C axis (C) must move to the endpoint of the arc of

radius R made on the side of the cylinder.

In incremental mode (G91) the C axis arc length along with the

programmed Z move length, must position the C and Z axes at a legal

endpoint for the arc radius defined by the R value in the G02/G03 block.

In absolute mode (G90) the coordinate defined by the C axis arc along with

the coordinate programmed for the Z axis, must position the C and Z axes

at a legal endpoint for the arc radius defined by the R value in the

G02/G03 block.

When cylindrical interpolation is activated, the circle plane is set to ZC.

The C and Z axes become the two axes of the circle plane and remain so,

as long as the G16.1 mode is active. If the active plane is changed, the

change does not become effective until the G16.1 mode is cancelled, and is

superceded if the G16.1 plane is reactivated.

Cylindrical Interpolation Operation

When virtual C axis cylindrical interpolation is activated, the control

terminates any spindle operations and defines the current spindle position

as zero degrees. If the AMP parameter Automatic Home on Virtual C

Entry is set to “YES,” a homing operation was performed prior to this.

The control then switches spindle operation from an open-loop spindle to a

closed-loop positioning axis.

Important: If orientation of the part is important, or if you expect to leave

G16.1 mode and then return and continue work on a specific area of the

part, the primary spindle should be homed each time you enter the G16.1

17-17

Chapter 17

Spindles

mode. If the AMP parameter Automatic Home on Virtual C Entry is

set to “NO” (refer to the documentation provided by your system installer),

you need to home the virtual C axis, typically by programming a M19S0.

The control positions the tool on the cylindrical work surface with two

distinct moves. In the first move, all programmed axis moves in the initial

G16.1 block (including the C axis) are executed. This move takes place at

the rapid feedrate for the axes.

In the second move, the feed axis (X) is moved at the active cutting

feedrate to the radius specified by R.

The blocks following the G16.1 block determine the contour to be

machined on the side of the cylindrical workpiece. The moves of the

virtual C axis and the machine axes are interpolated to produce the

programmed contours.

The following example makes a circumferential cut, followed by a 90

degree arc, followed by a linear cut, all made into the side of a cylindrical

workpiece. The C axis angle in the G03 block of this program was derived

from the equation that follows this example. Figure 17.4 illustrates the

results.

Example 17.2

Virtual C Axis, Cylindrical Interpolation

G91 M05;

G16.1;

C10. Z-40.;

C60.;

G03 Z8. C18.335 R8.;

Z20.;

G16.1 R30.;

G15;

The angle for the C move in the G03 block above was determined by using

this equation, with L = 8 and R = 25.

360

( L )

-------------

2 p( R )

17-18

Chapter 17

Spindles

17.5.2

End face milling coordinates the motion of the virtual C axis with that of

the linear machine axes to machine contours on the end face of a

Virtual C Axis,

workpiece as shown in Figure 17.5. Virtual C axis end face milling is

End Face Milling

turned on using a G16.2 block and turned off with a G15 block (or a G16.1

block requesting cylindrical interpolation). A G15 block can not contain

any axis words.

Figure 17.5

Virtual C Axis End Face Milling

Y (simulated)

Lathe Live Tool

The following are not allowed during end face milling:

Automatic motion to and from home G27, G28, G29, or G30

Work coordinate changes and shifts G53, G54-G59, G59.1, G59.2,

G59.3, G50/G92, G52, G92.1

All Turning and Threading cycles

All Drilling, Tapping, and Boring cycles

For ease of programming and to help the programmer visualize contours, a

simulated axis (end face milling axis) perpendicular to the X axis is

utilized with this feature. This axis name, its incremental axis name (if

Lathe Type A), and its integrand name are defined in AMP. This

description assumes that those names are Y, V, and J respectively. Refer to

the literature provided by your system installer for specific information.

17-20

Chapter 17

Spindles

End Face Milling Block Format

The block used to activate virtual C axis end face milling has this format:

G16.2 X__ Y__ Z__ R__ F__

Where :

Is :

The coordinate (if in G90 absolute mode) or the linear distance (if in G91

incremental mode) to which the X axis is to move. Be aware that this value is

affected by diameter (G08) or radius (G07) programming mode.

The coordinate (if in G90 absolute mode) or the linear distance (if in G91

incremental mode) to which the simulated Y axis is to move.

The coordinate (if in G90 absolute mode) or the linear distance (if in G91

incremental mode) to which the Z axis is to move. This axis determines depth of

cut in End Face Milling.

The radius of the arc to be cut in the face of the part. This parameter can be

used only if G02 or G03 circular interpolation has been activated, and must be

programmed with the correct X and Y coordinates. See chapter 14.

The feedrate to be used by the X, Y, and Z axes when commanded to move while

G16.2 is active.

These parameters and their application are described in detail in the

paragraphs that follow:

Any axis motions except for C axis motions can be programmed in the

G16.2 block. The control generates C axis motion in response to

programmed requests for simulated Y axis motion. This allows the

programmer to enter his contour moves as though he were working with an

XY plane, with cutting depth controlled by the Z axis.

If G02 or G03 circular interpolation is made active while in G16.2 end face

milling mode, circular cuts can be made in the face of the part (for

example, the corners could be rounded in the contour illustrated in

Figure 17.5). This is accomplished by programming the X and Y axis

endpoints along with the desired circle radius R as described in chapter 14.

The R parameter used here defines the radius of the circular path to be cut.

Important: When programming circular interpolation in G16.2 mode,

only radius programming (using R) may be used. Integrand programming

(using I, J) is not allowed and generates the error message “CIRCLE

PROGRAMMING ERROR.”

Important: When programming circular interpolation in incremental

mode (G91), the programmed X move length along with the programmed

Y move length, must position the X and Y axes at a legal endpoint for the

circular radius defined by the R value in the G02/G03 block. In absolute

mode (G90) the coordinate programmed for the X axis along with the

coordinate programmed for the Y axis, must position the X and Y axes at

a legal endpoint for the circular radius defined by the R value in the

G02/G03 block.

17-21

Chapter 17

Spindles

When end face milling is activated, the circle plane is set to XY. The X

axis becomes the primary axis of the circle plane and remains so, as long

as the G16.2 mode is active. If the active plane is changed, the change

does not become effective until the G16.2 mode is cancelled, and is

superseded if the G16.2 plane is reactivated.

End Face Milling Operation

When virtual C axis end face milling is activated, the control terminates

any primary spindle operations and defines the current primary spindle

position as zero degrees. If the AMP parameter Automatic Home on

Virtual C Entry is set to “YES,” a homing operation was performed prior

to this. The control then switches primary spindle operation from an

open-loop spindle to a closed-loop positioning axis.

Important: If orientation of the part is important, or if you expect to leave

G16.2 mode and then return and continue work on a specific area of the

part, the primary spindle should be homed each time you enter the G16.2

mode. If the AMP parameter Automatic Home on Virtual C Entry is

set to “NO” (refer to the documentation provided by your system installer),

you need to home the virtual C axis, typically by programming a M19S0.

The blocks following the G16.2 block determine the contour to be

machined on the end face of the cylindrical workpiece. The moves of the

virtual C axis and the machine axes are interpolated to provide the

programmed contours on the workpiece face.

Example 17.3 generates a square cut in the face of a part similar to that

show in Figure 17.5.

Example 17.3

Virtual C Axis, End Face Milling

G91 M05 X-20.;

G16.2 Z-5.;

Y10.;

X-20.;

Y-20.;

X20.;

Y-10.;

Z5.;

G15;

17-22

9/Series CNC Lathe. Operation and Programming Manual - page 14