Content      ..     9      10      11     

HNC-818. User Manual - page 11

14. Spindle Functions

14.1 Constant Linear Speed Cutting Control (T) (G96, G97)

Specifies the circumferential speed (relative speed between the tool and

the workpiece) after S. With respect to the tool position change, rotate

the spindle at specified circumferential speed all the time.

Format

constant linear speed control

G46 X_ P_; limit spindle speed

G97 S_ ; cancel the spindle constant linear speed control

Parameter

Description

P

In G96 command: It specifies the axis for the constant

linear speed control. The axis specified by

0 is

determined by the system axis parameter. The values

1, 2, and 3 indicate the X, Y and Z axis respectively.

In G46 command: It specifies the maximum spindle

speed

(r/min) limitation when the constant linear

speed is defined by G46.

S

Define the constant linear speed in G96 (mm/min or

inch/min).

The defined spindle speed (r/min) after the constant

linear speed is canceled in G97.

X

The minimum spindle speed (r/min) limitation when

the constant linear speed is defined.

G96 P_ S_ ; enable the spindle

Description

which can be canceled by each other.

2.

G46 is valid only when the constant linear speed function is valid.

3.

Only when the spindle can automatically change speed (e.g.: servo

spindle, frequency spindle), can the constant linear speed function

be used.

4.

During the constant linear speed control, when the spindle speed

exceeds the maximum spindle speed, it will be limited at the

maximum speed.

1.

G96/G97 are modal commands

Attention

309

14. Spindle Functions

Example

40

31

27

R5

R15

%3318

N1 T0101; Select No. 1 tool and define coordinate system

N2 G00 X40 Z5; Go to the start point

N3 M03 S460; Rotates spindle at 460r/min

N4 G96 P0 S80; The constant linear speed is valid, with the speed of

80m/min).

N5 G46 X400 P900; Limit the spindle speed range: 400-900 r/min

N6 G00 X0; The tool goes to the center, and the spindle speed increases

until the maximum speed 900r/min.

N7 G01 Z0 F60; Close to the workpiece

N8 G03 U24 W-24 R15; Conduct machining for the arc of R15

N9 G02 X26 Z-31 R5; Conduct machining for the arc of R5

N10 G01 Z-40; Conduct machining for the outer circle of ĭ26

N11 X40 Z5; Back to the tool setting location

N12 G97 S300; Cancel the constant linear speed function, and rotate the

spindle at the speed of 300r/min

N13 M30; Stop spindle, end the main program, and reset

311

18. Spindle Functions

14.2 C/S Axis Switching Function (CTOS/STOC)

In complex applications, such as rigid tapping function, the spindle need

to be used as a rotation axis in addition to a spindle. In this case, the C/S

axis switching function is available.

Format

STOC/G108 IP;

CTOS/G109 IP;

Parameter

Description

IP

IP can be defined as A/B/C. The number following it

indicates the channel spindle number, which ranges

from 0 to 3.

When IP is not specified after STOC, No. 0 spindle

will be switched to the C axis by default.

When IP is not specified after CTOS, the C axis will

be switched to No.0 spindle by default.

Attention

1.

In the same G code, it is not recommended to frequently use the

STOC/CTOS macro commands

2.

When the spindle is switched to the C axis, the unit of the C axis is

deg/min.

3.

It is not allowed to use the random line function to jump among

lines between STOC and CTOS, or jump from other line to a line

between STOC and CTOS.

4.

The random line function does not support the C axis of STOC.

Example

%900 Program name

G54

M03S600

STOC; Switch the spindle to the C axis

G28 C0; The C axis returns to the origin.

G1 C45 F2000

312

14. Spindle Functions

…

CTOS; Switch the C axis to the spindle

M03S600

M30

Attention

M30 cannot restore the status of the C/S axis.

14.3 Spindle Synchronization (G116, G117)

During dual spindle synchronization, one spindle is the master axis, and

the other is the slave axis. The reference spindle for synchronization is

called the master axis, while the axis moves with the master axis is called

the slave axis. During polygon machining, the tool axis is the master axis,

and the workpiece axis is the slave axis.

Format

G116 J_/K_ P_/Q_ R_; establish synchronization

G117; cancel synchronization

Parameter

Description

J

The logical axis number of the master axis.

K

The logical axis number of the slave axis.

P

The rotation speed ration of the master axis, ranging

from 1 to 1000.

Q

The rotation speed ration of the slave axis, ranging

from -1000 to 1000 and cannot be 0.

When Q is a positive value, the rotation direction of

the slave axis is the same as that of the master axis.

When Q is a negative value, the rotation direction of

the slave axis is opposite to that of the master axis.

R

Phase angle (0 to 360)

Example

T0101

G0 X100 Z20

M3 S1000

313

15. Programmable Data Input

15.1 Programmable Data Input (G10, G11)

You can dynamically modify system data in the program with

G10/G11.The modified system data takes effect immediately.

Format

Function

G Code

G54-G59: the origin of the

G10 L2 Pp IP_

workpiece coordinate system

G54.X: the origin of the extended

G10 L20 Pp IP_

workpiece coordinate system

System parameter output

G10 L53 PpRr

Cancel user-defined input

G11

Milling tool geometry

G10 L10 PpRr

compensation value H input

Milling tool geometry

G10 L12 PpRr

compensation value D input

Turning tool compensation value

G10 L14 Pp X_ Z_ R_ Q_ Y_ J_

input

K_

Description

G10 is a modal command, which enables the programmable data input

mode until it is canceled by G11.

G54-G59 origin of the workpiece

G10 L2 Pp IP_

coordinate system

Parameter

Description

Pp

Specify the workpiece origin offset in the relative

workpiece coordinate systems from 1 to 6:

y

1 indicates the G54 workpiece coordinate system

y

2 indicates the G55 workpiece coordinate system

y

3 indicates the G56 workpiece coordinate system

y

4 indicates the G57 workpiece coordinate system

y

5 indicates the G58 workpiece coordinate system

y

6 indicates the G59 workpiece coordinate system

IP

The workpiece origin offset of each axis for absolute

commands.

Added to the workpiece origin offset of each axis for

incremental commands.

Example 1

%0002

316

15. Programmable Data Input

Milling tool geometry compensation value H input

G10 L10 Pp Rr;

Parameter

Description

Pp

Tool offset number

Rr

Tool compensation data

Milling

tool

geometry

G10 L12 Pp Rr;

compensation value D input

Parameter

Description

Pp

Tool offset number

Rr

Tool compensation data

Turning tool compensation input

G10 L14 Pp X_ Z_ R_ Q_ Y_ J_ K_;

Parameter

Description

Pp

Tool offset number

X

Tool compensation data X

Z

Tool compensation data Z

R

Tool nose compensation R

Q

Imaginary too nose direction

Y

Tool compensation data Y

J

Tool radial wear J

K

Tool axial wear K

319

16. Axis Control Functions

16.1 Cycle Function of the Rotation Axis

Overview

The rotation axis cycle function can be used to prevent the overflow of

the rotation axis coordinate value.

You may enable the rotation axis cycle function by setting relevant

parameters.

Take the C axis as an example, you need to set the parameter AXIS

TYPE (104001) of axis 4 to 3 in the coordinate axis parameters , and set

the parameter FEEDBACK POS CYCLE ENABLED (505014) of the

corresponding device to 1in the device interface parameters.

Description

For incremental commands, the movement amount is the command

value.

For absolute command, you may set the parameter R-AXIS SHORT

PATH SELECTION EN (104082) of the corresponding axis to 1 in the

coordinate axis parameters, and set the rotation direction of the rotation

axis to the direction of the short path from the start point to the end point.

Example

G90 C0

Sequence

Actual

Absolute Coordinates

N1 G90 C-150.0

No.

Movement

after Movement

N2 G90 C540.0

N1

-150

210

N3 G90 C-620.0

N2

-30

180

N4 G91 C380.0

N3

-80

100

N5 G91 C-840.0

N4

380

120

N5

-840

0

Attention

For some machines with rotation axis (such as working tables), due to

the mechanical structure, the rotation axis can rotate only in one

direction during movement. In this case, it is not recommended to use the

absolute command but the incremental command programming to avoid

the opposite direction of rotation caused by programming errors.

321

16. Axis Control Functions

16.2 Reference of Grating Ruler with Distance-Code

Overview

Using a linear measuring system with distance-coded reference point

symbols, you do not need to install a deceleration switch on the machine

for returning to the reference point, and the machine can return to a fixed

machine reference point. It makes the operation much faster and easier in

the actual use.

Principle

The principle for the linear measuring system with distance-coded

reference point symbols is to adopt a standard linear grid line and a

channel with distance-coded reference point symbols which is parallel to

the linear grid line. The distance between two reference point symbols in

the same group is the same, but the distance between the adjacent

reference point symbols of two different groups is variable. Each

segment distance plus a fixed value, then the CNC axis can determine

the absolute position according to the distance. See the figure below

(example: LS486C):

Reference point

symbol

10.04

10.06

10.08

10.10

10.02

20.02

20.02

20.02

20.02

20

20

20

20

20

A

B

C

D

E

For example, the machine moves from point A to point C through the

middle point B. If the system detects

10.02

, it will know which

reference point the axis is at. Similarly, when the machine moves from

point B to point D through the middle point C and the distance from the

point C to point D is 10.04, the system will know which reference point

the axis is at. Therefore, if the axis moves more than two reference points

(20 mm), the system will be able to get the absolute position of the

machine.

322

16. Axis Control Functions

Parameter settings

Take the X-axis as an example to illustrate the parameter settings for

linear grating ruler with distance code:

10.02

10.04

Distance between

0

20

40

distance-coded

reference points

1.

Setting reference returning mode

Set the parameter REF POINT RETURN MODE (100010) of the

axis 0 in coordinate axis parameters to 4 when the feedback from

the distance-code is in the same direction of reference returning;

otherwise set it to 5.

2.

Setting distance between distance-coded reference points

Set the parameter DISTANCE CODE REF SPACE(mm) (100018)

of the axis 0 in coordinate axis parameters. This parameter indicates

the distance between two adjacent distance-coded reference points

in the incremental measuring system. As shown in the figure above,

the distance between two distance-coded reference points is set to

20.

3.

Setting distance-code offset

Set the parameter DISTANCE CODE DEVIATION(mm) (100019)

of the axis 0 in coordinate axis parameters. This parameter indicates

the incremental interval between distance-coded reference points in

the incremental measurement system. As shown in the figure above,

it indicates the incremental value

0.02 from

10.02 to

10.04.

Therefore, the distance-code offset is set to 0.02.

4.

Setting reference point zero

After the distance code is returned to the zero point, return a defined

point to the zero point, and set this point to the machine zero. Then

set the coordinate value after the current point is returned to zero for

REF POINT POS(mm) (100017) of the coordinate axis 0. This

point will be used as the machine origin to define coordinate system

when you return a point to the zero point next time.

323

17. Other Functions

17.3 Axis Release (G101) and Axis Obtaining (G102)

Format

G101 IP_

Parameter

Description

IP

Set the axis to be released. Options:

X/Y/Z/A/B/C/U/V/W/S0/S1/S2/S3

G102 IP_

Parameter

Description

IP

Set the axis to be obtained. Options:

X/Y/Z/A/B/C/U/V/W/S0/S1/S2/S3

Description

G101 is used to release the axis by the channel. The address word

following G101 can be any numbers, but it is recommended to specify it

as 0.

G102 is used to obtain the axis by the channel. The address word

following G102 must be a logical axis number.

Attention

1.

Generally, the same logical axis can belong to only one channel at

the same time.

2.

After a channel obtains an axis, you need to set the G5X origin of

the axis. If it cannot be specified on the settings interface, you may

use G10 to specify it.

3.

Axis release or obtaining cannot be executed during axis movement.

327

17. Other Functions

17.4 Command Channel Loader (G1030) and Running (G103.1)

Format

G103 P="program name" Q={channel number,...}

Parameter

Description

P

The name of the program to be loaded.

Q

The number of the channel where the program will be

loaded. Separate multiple channels with a comma

symbol (,).

G103.1 Q={channel number,...}

Parameter

Description

Q

The number of the channel where the program will

run. Separate multiple channels with a comma symbol

(,).

Description

When G103.1 is executed, the channel where the program will be loaded

must be in the auto mode.

When G103 is executed, the channel where the program will be loaded

should not have selection programs.

These two commands are generally used for multi-channels.

Example

Assuming that there is a dual-channel machine, channel 1 makes channel

2 load and run program O01.

%1

N1 G54

N2 G103 P="O01" Q={2}

N3 G103.1 Q={2}

.......;

M30

When channel 1 completes the line N3, channel 2 starts to run O01.

329

17. Other Functions

17.5 Channel Synchronization (G104)

Format

G104 P_ Q={channel number,}

Parameter

Description

Q

The number of the channel to be synchronized.

Separate multiple channels with a comma symbol (,).

P

Signal value, ranging from 0 to 40.

Description

G104 is generally used for the process synchronization of multiple

channels.

Example

Assuming there is a dual-channel milling machine, and the X axis is the

public axis, with the following configuration:

Logical Axis No. of

Logical Axis No. of

Channel 0

Channel 1

X axis

0

---

Y axis

1

3

Z axis

2

4

Programs of Channel 1

Programs of Channel 2

%1

%2

N1G54X0Y0Z0

N1G104

P1

Q={1,2};

N2G02X10Y10R20

synchronization statement 1

N3G1X0Y0Z0

N2G102 X0; obtain X axis

N4G101 X0; release X axis

N3G54X0Y0Z0

N5G104

P1

Q={1,2};

N4G02X10Y10R20

synchronization statement 1

N5G0X0Y0Z0

N6G104

P2

Q={1,2};

N6G101 X0; release X axis

synchronization statement 2

N7G104

P2

Q={1,2};

N7G102 X0

synchronization statement 2

N8G0X100

N8M30

N9M30

As listed in the table above, channel 1 and 2 load their own programs

330

Content      ..     9      10      11