HNC-818. User Manual

4. Auxiliary Functions

4.1 M Commands

Auxiliary function commands consist of the address character "M" and

digital numbers. It is used to control the motion of the programs, various

auxiliary switch of the machine, the start and stop of the spindle, end of

the program, etc.

Generally, one program block has only one valid M command. In this

system, up to four M commands can be specified in one block (M

commands in the same group cannot be specified in the same line).

The M commands (M00, M01, M02, M30, and M99) must be in a

separate line. In other words, the program line which contains any of the

M commands mentioned above can contain only one M command, and

cannot have other commands such as G commands or T commands.

The relationship between the M commands and their functions depends

on the specific settings of the machine manufacturer.

Modal

The M functions include non-modal and modal functions:

Non-modal M function (valid only in the current block)

Modal M function (continuously valid)

Modal Group

Modal M commands are grouped according to different functions. Once

the defined modal M command has been executed, it remains valid until

it is canceled by other modal M commands in the same group.

The Modal M function group contains a default function which is the

initial function when the system is powered on.

Pre- and Post- M functions

The M function can also be divided into pre-M function and post-M

function:

Pre-M function

Executed before the axis motion specified by the program block.

Post-M function

Executed after the axis motion specified by the program block.

4. Auxiliary Functions

4.1.1 Default CNC Auxiliary Functions

M00

Pause Program

When the CNC system executes the M00 command, it will pause the

execution of the current program. That facilitates the operator to carry

out dimensional measurements of the tool and the workpiece, turn

around the workpiece, manually change speed, etc.

When the system pauses the program, the feeding on the machine is

stopped, and all existing modal information remains unchanged. If you

want to continue the follow-up procedures, press the Start button on the

control panel.

M00 indicates the non-modal post-M function.

M01

Optional Pause Program

If you activate the Optional Pause key on the control panel, the CNC

system will pause the current program when it executes the M01

command, to facilitate the operator to carry out dimensional

measurements of the tool and the workpiece, turn around the workpiece,

manually change speed, etc. When the system pauses the program, the

feeding on the machine is stopped, and all existing modal information

remains unchanged. If you want to continue the follow-up procedures,

press the Start button on the control panel.

If you do not activate the Optional Pause key on the control panel, the

CNC system will not pause the current program when it executes the

M01 command.

M01 indicates the non-modal post-M function.

M02

End program

M02 is created in the last program block of the main program.

When the CNC system executes the M02 command, all the spindle, feed,

and coolant functions are stopped and the machining is ended.

After the program is ended by M02, you need to recall the program or

press the Restart key under the auto machining sub menu, and press the

Start button on the control panel if you want to re-execute the program.

M02 indicates the non-modal post-M function.

4. Auxiliary Functions

M30

End program and return (valid only when it is in a separate line)

The functions of M30 are similar to those of M02, with an additional

control function of returning to the program header (%).

After the program is ended by M30, you need to repress the Start button

on the control panel if you want to re-execute the program.

M98/M99

Call sub-programs

If the program contains a fixed sequence or frequently repeated pattern,

the sequence or pattern can be stored as a sub-program in the memory to

simplify the programming.

A sub-program can be called for a maximum of 10,000 times (L).

A sub-program can be called from a main program.

In addition, a called sub-program can call another sub-program.

Sub-program structure:

%xxxx; Sub-program number

……; Sub-program content

M99; Sub-program returns

Call sub-program (M98)

M98 PƑƑƑƑ LΔΔΔ

ƑƑƑƑ: The number of the called sub-program

(Arabic

numerals)

ΔΔΔ: The times that the sub-program is called

Call nested sub-programs

A main program can call up to six levels of sub-programs. See the figure

below:

%1000

%1001

%1002

%1008

…

M98P1001

M98P1002

M98P1003

……

…

M99

M30

M99

4. Auxiliary Functions

4.1.2 Auxiliary Functions Defined by PLC

M3/4/5

Spindle Control

The M03 command starts and rotates the spindle in a clockwise direction

(from the positive direction toward the negative direction of the Z axis)

at the speed specified in the program.

The M04 command starts and rotates the spindle in a counter clockwise

direction at the speed specified in the program.

The M05 command stops the spindle rotation.

The M03 and M04 are modal pre-M functions. M05 is a modal post-M

function, which is the default function.

M03, M04, M05 can be canceled by each other.

M06 Tool Change

M06 is used to call a tool that will be installed on the spindle from the

machining center. The tool will be automatically installed on the spindle

when executing this command. Example: M06 T01 can be used to install

the 01 tool on the spindle.

M06 indicates a non-modal post-M function.

For the machines with armless type ATC, the tool change process is as

follows (e.g. to change the tool 15 on the spindle to tool 01, execute M06

T01.):

Move the spindle quickly to the fixed tool change position which

has been defined by the commissioning personnel.

Directionally rotate the spindle.

Rotate the tool magazine to the position (the position of the tool 15

in Group 0).

The cylinder drives the tool magazine, and chucks the tool on the

spindle.

The cylinder releases the tool on the spindle, and blows to clean the

spindle.

The spindle moves upward, and moves away completely from the

tool.

The tool magazine rotates to the tool position of tool 01(the tool

number of Group 0 in the tool magazine changes to 01).

4. Auxiliary Functions

The spindle moves downward, and catches the tool.

The cylinder on the spindle clamps the tool.

10. The tool magazine returns to the original position.

11. Release the orientation of the spindle.

Attention

M06 must be defined in a separate line.

M7/8/9

Coolant Control

M07 and M08 are used to enable the coolant control.

M09 is used to disable the coolant control.

M07 and M08 are modal pre-M functions; M09 is a modal post-M

function, which is the default function.

M64

Workpiece Count

M64 is used to calculate the cumulative count of completed workpiece.

M19/M20

Spindle Orientation

M19 is used for spindle orientation.

M20 is used to cancel the spindle orientation.

M03/M04

The spindle can be switched directly from the position mode to speed

mode by executing the M03/M04 command, without executing G109.

4. Auxiliary Functions

4.2 S Commands

Directly Define Spindle Speed

The S command is used to control the spindle rotation speed. The

number that follows S indicates the spindle speed in revolution per

minute (r/min).

The S command is a modal command, and the S function is valid only

when the spindle speed is adjustable.

Define Spindle Speed with Code

In the lathe with mechanical shifting, you may specify a value behind S

to input a code signal to the machine, thereby controlling the spindle

speed of the machine.

This approach needs to be processed in the ladder graph.

4. Auxiliary Functions

4.3 T Commands

T commands are used for tool selection. The value that follows T

indicates the selected tool number. The relationship between T

commands and the tool is defined by the machine manufacturer.

machining center to input a code signal or a strobe signal into the

machine, thereby controlling the rotation of the tool magazine to the

Milling System

selected tool, and then wait until the completion of the tool change with

the M06 command. For armless type ATC, the M06 and T commands

must be written in the same block. During tool change, the tool number

(e.g. 15) of Group 0 must be the position of the tool clamped on the

spindle in the tool magazine. When you change the tool to another, you

need to firstly return the tool to the corresponding tool position in the

tool magazine (that is No. 15). Then there should be no tool in the

position of No.15, otherwise a collision may occur. The tools in the tool

magazine are automatically managed by the system, and cannot be

modified. After the machine starts, tool position(e.g. No. 15) facing to

the spindle must be the same as tool number of Group 0 in the tool

magazine, and there should be no tool in the corresponding tool position

(e.g. No. 15).

Therefore, when installing tools to the tool magazine, it is recommended

to firstly install the tool on the spindle, then in the MDI mode, run the M

and T commands (e.g. M06 T01) to install the tool through the spindle.

Execute a T command on the

Turning System

T commands are used for tool selection and tool change. The

four/six/eight digits that follow T indicates the selected tool number and

tool compensation number.

For TXX XX (4 digits), the first two digits indicate the tool number, and

the last two digits indicate the tool compensation number.

For TXXX XXX (6 digits), the first three digits indicate the tool number,

and the last three digits indicate the tool compensation number.

4. Auxiliary Functions

For TXXXX XXXS (8 digits), the

first four digits indicate the tool

number, and the last four digits

indicate the tool compensation

number.

The relationship between the tool

You may set parameters to define the number (four by default) of digits

and T commands is specified by the

which follow T code.

machine manufacturer. Please refer

to the user manual of the machine

y When P000061 is set to 2, T code is followed by four digits.

provided by the manufacturer.

y When P000061 is set to 3, T code is followed by six digits.

The same tool may correspond to multiple tool compensations (e.g.

T0101, T0102, T0103), and multiple tools may correspond to the same

tool compensation (e.g. T0101, T0201, T0301).

Execute the T command to rotate the tool turret and select the defined

tool, and at the same time import the tool compensation value(the

geometry compensation value of the tool indicates the offset

compensation plus the wear compensation) in the tool compensation

without being followed by motion commands.

When a program block contains T commands and tool motion commands

simultaneously, the T commands are firstly executed, and then the tool

motion commands are performed.

%0012

N01 T0101

N02 M03 S460

N03 G00 X45 Z0

N04 G01 X10 F100

N05 G00 X80 Z30

N06 T0202

N07 G00 X40 Z5

N08 G01 Z-20 F100

N09 G00 X80 Z30

M10 M30

For details about the tool compensation, see the relevant tool

compensation section in this documentation.

5. Interpolation Functions

5.1 Linear Feed (G01)

G01 enables a linear feed of the tool from the starting point to the end.

Format

Parameter

Description

Under G90command, it indicates the coordinate value of

the end point in the workpiece coordinate system.

G01 IP_ F_

UnderG91command, it indicates the relative

displacement of the end point to the starting point.

Description

Feed speed

G01 enables a linear feed of the tool from the current position to the end

point defined by the program block at the speed specified by F and in

linkage approach.

G01 is a modal code, which can be canceled by G00, G02, G03 or G34.

The feed speed specified by F is constantly valid and does not need to be

specified in every program block.

The speed along each axis is as follows:

G91 G01 XĮ Yȕ ZȖ Ff;

X axis: FĮ = Į x f/L;

Y axis: Fȕ = ȕ x f/L;

Z axis: FȖ = Ȗ x f/L;

Speed of Rotation Axis

For rotation axis, its feed speed is defined by the linear speed.

During linear interpolation, when the linear axis is Į (e.g. X, unit: mm)

and the rotation axis is ȕ (e.g. C, unit: deg), the tangential speed in the

Į/ȕ Cartesian coordinate system is defined by F (mm/min). The speed on

the ȕ axis is obtained based on the time calculated from the formula

above and then converted to deg/min.

5. Interpolation Functions

Example: G91 G01 X20.0 C40.0 F300.0;

Assuming the metric input of the C axis 40.0deg is 40 mm

Then the time required should be:

² +

ؒ0.14907 min

300

The speed on the C axis is:

40 deg

ؒ268.3 deg/min

0.14907 min

Linear Interpolation

Feed speed 300mm/min

End point

200.0

0 (Start point)

300.0

G91 G01 X300.0 Y200.0 F300

Rotation Interpolation

Start point

Feed speed 300 degree/min

End point

G91 G01 C-90 F300

5. Interpolation Functions

After the five-axis RTCP function is enabled, F specifies the movement

speed of the tool center point in the workpiece coordinate system. During

Attention

the five-axis machining, due to the join of the rotation axis, the

movement speed of the tool center point may not match the actual

machine movement speed; therefore, the split-axis speed may exceed the

specified maximum speed limit. In this case, the CNC system will reduce

the machining speed to ensure the split-axis speed within the defined

range.

Use G01 for programming: Linear feed from the point A to B (a straight

line from A to B)

Example

Linear feed from A to B

Actual path

Absolute programming:

G90 G01 X90 Y45 F800

Incremental programming:

Programming path

G91 G01 X70 Y30 F800

5. Interpolation Functions

5.2 Arc Feed (G02, G03)

Run the tool to the end along the specified arc direction at a specified

plane (G17, G18, G19).

Format

⎧G02⎫

⎧I

_⎫

G17

Arc interpolation in the XY

⎨

⎬

⎨

⎬

⎩G03⎭

⎩

⎭

plane

⎧G02⎫

⎧I

_⎫

G18⎨

⎬X

_Z⎨

⎬F

Arc interpolation in the ZX plane

⎩G03⎭

⎩

⎭

⎧G02⎫

⎧J

_⎫

G19⎨

⎬Y

Z⎨

⎬F

Arc interpolation in the YZ plane

G03

⎩

⎭

⎩

⎭

Parameter Description

Parameter

Description

G17

Specify arc interpolation at the XY plane

G18

Specify arc interpolation at the ZX plane

G19

Specify arc interpolation at the YZ plane

G02

CW arc interpolation

G03

CCW arc interpolation

The amount of movement along the X-axis with arc

interpolation or the X-axis coordinate value of the arc end

The amount of movement along the Y-axis with arc

interpolation or the Y-axis coordinate value of the arc end

The amount of movement along the Z-axis with arc

interpolation or the Z-axis coordinate value of the arc end

Arc radius (with signal, "+": inferior arc; "-": excellent arc)

The distance from the arc start point along the X-axis to the

center of the arc (with signal)

The distance from the arc start point along the Y-axis to the

center of the arc (with signal)

The distance from the arc start point along the Z-axis to the

center of the arc (with signal)

Feed speed, valid in the modal mode

5. Interpolation Functions

Arc Interpolation Direction

Definition of clockwise (CW) and counter clockwise (CCW) direction in

each plane: in the Cartesian coordinate system, looking to the XY plane

from the positive direction of Z-axis to the negative direction to define

the CW and CCW direction of the XY plane; similarly, looking to the ZX

plane from the positive direction of the Y-axis to the negative direction to

define the CW and CCW direction of the ZX plane; looking to the YZ

plane from the positive direction of the X-axis to the negative direction

to define the CW and CCW direction of the YZ plane. See the figure

below:

G03

G02

G17

G18

G19

Arc End

Use the position command (X, Y, Z) to specify the arc end.

In the absolute value (G90) mode, the position command (X, Y, Z)

specifies the absolute position of the arc end point; in the incremental

value (G91) mode, the position command (X, Y, Z) specified the distance

from the arc start point to the end point. See the figure below:

End point

End point of Arc:

(X₂, Y₂)

G90: X_=X₂

Y_=Y₂

Start point

G91: X_=X₂-X₁

(X₁, Y₁)

Y_=Y₂-Y₁

5. Interpolation Functions

UVW Programming

In addition to the position command (X, Y, Z), you may use the UVW

command to specify the arc end.

For the turning CNC system (T Series), when the channel parameter

Enable Programming with UVW (040033) is set to 1, you may use

UVW instead of XYZ to represent the movement amount (increment) of

G02/G03 along the XYZ axis, or use XYZ and UVW for one

programming.

Note: Only when the UVW axes are not specified as the motion axis, can

UVW be used to specify the arc end.

Distance from the Start Point to

Use the command (I, J, K) to specify the position of the arc center.

the Arc Center

The parameters (I, J, K) indicate the vector components from the start

point to the arc center, and it is always incremental value for both G90

and G91.

You need to specify the positive ("+") or negative symbol ("-") for the

parameters (I, J, K) based on the direction.

See the figure below:

End point (X₂, Y₂)

End point (Z₂, X₂)

Start point

(X₁, Y₁)

(Z₁, X₁)

Center (X₀, Y₀)

Center (Z₀, X₀)

I_=X₀-X₁

K_=Z₀-Z₁

G17

G18

J_=Y₀-Y₁

I _=X₀-X₁

End point (Y₂, Z₂)

Start point

(Y₁, Z₁)

Center (Y₀, Z₀)

J_=Y₀-Y₁

G19

K_=Z₀-Z₁

5. Interpolation Functions

Circular Programming

If the position commands (X, Y, Z) are all left blank during programming,

the start point overlaps the end point. In this case, the command (I, J, K)

specifies a full circle. If R is used to specify the arc, it becomes an arc of

zero degree. A system alarm will be reported.

Arc radius

In addition to the command (I, J, K) mentioned above, you may specify

the arc center by using the arc radius. The arc is divided into two types:

Central angle less than 180 degrees

Central angle larger than 180 degrees

Therefore, you need know which arc to be programmed. The two types

can be defined by the positive or negative symbols ("+" or "-") of the arc

radius (R). See the figure below:

Central angle > 180 degrees

Arc1 (Central angle < 180 degrees)

G91 G02 X70 Y80 R50 F500;

End point

Arc2 (Central angle > 180 degrees)

G91 G02 X70 Y80 R-50 F500;

Start point

Central angle < 180

degrees

Attention

y Parameters related to arc interpolation

If the radius difference between the arc start point and end point is

greater than the value specified by CIR INTERPOLATION

C-TOL(mm) (000010), or (radius difference between the arc start

point and end point)

/actual radius is greater than the value

specified by Arc ARC PROG POINT RADIUS TOL(mm)

(000011), the system will alarm.

y I/J/K and R are specified simultaneously

If "I, J, K" and "R" are simultaneously specified in a non-full

circular arc interpolation command, the arc defined by R is valid.

y Specify axis outside the defined plane

If the axis is specified outside the defined plane, an alarm will be

reported.

5. Interpolation Functions

Semicircle Programming

When the arc is a semicircle or the central angle is close to 180

degrees, you must use I, J, K to specify the arc center, because a

calculation error may be generated due to the rounding errors if you

use R to specify the arc center.

Example

100

R50

End point

R60

Start point

120

140

200

As shown in the figure above, the tool path programming is as follows:

Absolute programming

G92 X200.0 Y40.0 Z0;

G90 G03 X140.0 Y100.0 R60.0 F300.;

G02 X120.0 Y60.0 R50.0;

G92 X200.0 Y40.0Z0;

G90 G03 X140.0 Y100.0 I-60.0 F300.;

G02 X120.0 Y60.0 I-50.0;

Incremental programming

G91 G03 X-60.0 Y60.0 R60.0 F3000.;

G02 X-20.0 Y-40.0 R50.0;

G91 G03 X-60.0 Y60.0 I-60.0 F300.;

G02 X-20.0 Y-40.0 I-50.0

5. Interpolation Functions

5.3 Cylindrical Helical Interpolation (G02, G03)

In addition to arc interpolation, the G02 and G03 commands can also be

used to define helical interpolation by specifying the movement distance

of the third axis.

Format

⎧G02⎫

⎧I

_⎫

XY Plane Helical Interpolation

G17⎨

⎬X

Z⎨

⎬F

⎩G03⎭

⎩

⎭

⎧G02⎫

⎧I

_⎫

G18

ZX Plane Helical Interpolation

⎨

⎬

⎨

⎬

G03

⎩

⎭

⎩

⎭

⎧G02⎫

⎧J

_⎫

G19

YZ Plane Helical Interpolation

⎨

⎬

⎨

⎬

⎩G03⎭

⎩

⎭

Parameter Description

G17

Specify arc interpolation at the XY plane

G18

Specify arc interpolation at the ZX plane

G19

Specify arc interpolation at the YZ plane

G02

CW arc interpolation

G03

CCW arc interpolation

The amount of movement along the X-axis with arc

interpolation or the X-axis coordinate value of the arc

end

The amount of movement along the Y-axis with arc

interpolation or the Y-axis coordinate value of the arc

end

The Z-axis coordinate value in absolute programming, or

the the Z-axis increment of the end point relative the

start point(even if L command is programmed)

Arc radius (with signal: "+": inferior arc; "-": excellent

arc)

The distance from the arc start point along the X-axis to

the center of the arc (with signal). The value of height

variation for a spiral circle at YZ plane in conic

interpolation.

The distance from the arc start point along the Y-axis to

the center of the arc (with signal)

Parameter

Description

5. Interpolation Functions

The distance from the arc start point along the Z-axis to

the center of the arc (with signal).

Feed speed, valid in the modal mode

Helical rotation number (positive number without a

decimal point)

For the rotation direction of helical interpolation, refer to the arc

Rotation Direction

direction projected on a two-dimensional plane.

Circular Programming

If the position commands (X, Y, Z) are all left blank during programming,

the start point overlaps the end point. In this case, the command (I, J, K)

specifies a full circle. If R is used to specify the arc, it becomes an arc of

zero degree. A system alarm will be reported.

Example

The figure below shows the helical machining:

K=5

Absolute programming

X30 Y0 Z0

G90 G03 X0 Y0 Z50 I-15 J0 K0 L10 F3500

5. Interpolation Functions

5.4 Specify Imaginary Axis and Sine Interpolation (G07)

Format

G07 IP_

Parameter

Description

Specify axis:

0: imaginary axis

1: real axis

Description

If an axis is specified as an imaginary axis, this axis is only used for

interpolation calculation without any motion. For example, if the G07 X0

command specifies the X axis as the imaginary axis, then the X axis will

not move until the G07 X1 command is executed.

Sine Interpolation

G07 can be used for a sine interpolation. For example, before the helical

interpolation, if an axis used for arc interpolation is specified as the

imaginary axis, then the helical interpolation becomes the sine

interpolation.

Attention

If you want to cancel the imaginary axis specification, you only specify

the imaginary axis as a real axis, e.g. executing G07 X1.

Example

Use G03 for programming the sine curve as below:

…

100

M3S1000

G90 G00 X-50 Y0 Z0

G07 X0 G91

G03 X0 Y0 I0 J50 Z60 F800

…

5. Interpolation Functions

5.5 NURBS Spline Interpolation (NURBS)

You may conduct NURBS spline interpolation by specifying three

parameters (IP, W, K) of the NURBS curve.

Single Spline NURBS Format

NURBS P_ K_ IP_ W_ F_;

Parameter

Description

Order of NURBS curve; Only cubic spline

interpolation is supported, where the value of P is 4.

Node

Control point coordinate

Weight

Feed speed

Cancel Interpolation

NURBS indicates modal of Group 01. You may cancel the NURBS

interpolation modal by specifying G01 or G00.

Curve order

P is used to specify the order of the NURRBS curve:

P=4, indicates cubic NURBS curve;

P is modal address word, which will be valid until it is changed or other

modal commands in group 01 are specified.

Node

During NURBS interpolation, you must specify the first control point as

the start point and the last control point as the end point.

In addition, use the following format to specify the node of the first

program block:

y Single-spline:

NURBS P4 K:0,0,0,0,1: X1 Y0 Z0

y Dual-spline:

NURBSB P4 K:0,0,0,0,0.5: Q:10,0,0,38.28,0,28.28: W1F60

5. Interpolation Functions

Weight

Weight indicates the weight value of the control point specified in the

same program block. If it is not specified, the default value is 1.0.

Compensation

In the NURBS curve interpolation mode, you cannot use tool radius

compensation.

Description

Single-spline NURBS interpolation is generally used for three-axis small

line interpolation.

Dual- spline NURBS interpolation is generally used for five-axis small

line interpolation.

Example

Single-spline

interpolation

The figure below shows the single-spline NURBS interpolation for a

full-circle (R=50mm):

100

(100, 100)

-100

(100, -100)

%0001

G54

G90G17F500G64

G01x0y0z0

NURBS P4 K:0.0,0.0,0.0,0.0,0.5: X0.0Y0.0Z0.0 W1.0

K0.5

X0.0000 Y100.0 W0.3333

K0.5

X100.0 Y100.0 W0.3333

5. Interpolation Functions

5.6 Thread Cutting (G32)

The feed operation coincides with the spindle rotation, which different

kinds of threads can be processed, such as variable pitch screw,

multi-thread, etc.

Format

G32 X_ Z_ F_ P_ R_ E_

Parameter

Description

X Z

Thread end point coordinate (G90).

Relative distance of the thread end point away from

the start point (G91).

Metric thread pitch (along the long axis).

Angle of the thread start point

Specify the retreat of tailstock along the Z axis in the

incremental mode. If the tool withdrawal groove is

not required, the parameter signal cannot be specified.

Specify the retreat of tailstock along the X axis in the

incremental mode. If the tool withdrawal groove is

not required, the parameter signal cannot be specified.

Constant Pitch

Multi-Thread

You may process multi-threads by specifying the thread start angle P.

For example, you may set P to 180 degrees to process double threads.

See the figure below:

5. Interpolation Functions

Retreat of tailstock

tailstock by specifying the R (retreat along the Z axis) and E (retreat

along the X axis) parameters, of which values are specified in the

incremental mode for both absolute and incremental programming. The

positive value indicates the retreat along the positive direction of the Z/X

axis, while the negative value indicates the retreat in the negative

direction of the Z/X axis. If no R or E value is specified, there will be no

retreat function.

According to the thread standard, R is generally specified as double pitch,

while E is specified as the height of the thread.

Note: If the retreat of tailstock is specified, the thread cutting direction

must be coordinated with the R/E direction to avoid damage to the

thread. For example, if the thread cutting is towards the negative

direction of the Z axis, then the value of R must be negative; otherwise,

there may be damage to the processed thread.

You may define the retreat of

Attention

Do not change the feed rate or spindle override during thread

cutting.

It is dangerous to stop the feed of the thread cutting tool without

stopping the spindle as it may suddenly increase the cutting depth;

therefore, the function of feed hold is invalid during thread cutting.

The feed hold is valid only during the non-thread machining.

When thread cutting is conducted in the single block mode, the tool

will stop at the beginning of the first block where no threading

cutting is specified.

During thread cutting, the work mode cannot be changed from the

auto mode into manual, incremental or reference mode.

5. Interpolation Functions

Example

The figure below shows the cylindrical thread programming. Thread lead:

1.5 mm; each cut depth (diameter value): 0.8 mm, 0.6 mm, 0.4 mm, 0.16

mm.

100

%3316

N1 T0101 (Set coordinate system, and select No. 1 tool)

N2 G00 X50 Z120 (Move to the start point position)

N3 M03 S300 (Rotate the spindle at 300 r/min)

N4 G00 X29.2 Z101.5 (Move to the start point, acceleration stage: 1.5

mm, cut depth: 0.8 mm)

N5 G32 Z19 F1.5 (Thread cutting to the end point, deceleration stage: 1

mm)

N6 G00 X40 (Quick retreat along the X axis)

N7 Z101.5 (Quick retreat to the start point along the Z axis)

N8 X28.6 (Fast forward to the start point along the X axis, cut depth: 0.6

mm)

N9 G32 Z19 F1.5 (Cut thread to the end point)

N10 G00 X40 (Quick retreat along the X axis)

N11 Z101.5 (Quick retreat to the start point along the Z axis)

N12 X28.2 (Fast forward to the start point along the X axis, cut depth:

0.4 mm)

N13 G32 Z19 F1.5 (Cut thread to the end point)

5. Interpolation Functions

N14 G00 X40 (Quick retreat along

the X axis)

N16 U-11.96 (Fast forward to the start point along the X axis, cut depth:

N15 Z101.5

(Quick retreat to the

0.16 mm)

start point along the Z axis)

N17 G32 W-82.5 F1.5 (Cut thread to the end point)

N18 G00 X40 (Quick retreat along the X axis)

N19 X50 Z120 (Back to the tool setting position)

N20 M05 (Stop the spindle)

N21 M30 (End the main program and reset)

5. Interpolation Functions

5.7 HSPLINE Spline Interpolation (HSPLINE)

HSPLINE is the abbreviation of Hermite SPLINE. The Hermite

interpolation function can also improve the machining results of small

lines, making the surface fairing. Different from the NURBS curves, the

Hermite curve passes through the control point. The CNC system may

conduct spline interpolation by specifying the control point and vectors

of the Hermite curve.

Format

HSPLINE P_ X_ Y_ Z_ I_ J_ K_ F_

Parameter

Description

X Y Z

Control point coordinates.

Note: The coordinate position must be the same as

the end point position of the previous line.

I J K

Vector of the control point

Hermite curve order

Cancel Interpolation

HSPLINE indicates modal of Group 01. You may cancel the HSPLINE

interpolation modal by specifying G01 or G00.

Curve order

P is used to specify the order of the HSPLINE curve: P must be set to 3.

Compensation

Tool radius compensation cannot be used for HSPLINE interpolation.

Example

Use cubic Hermite spline interpolation for the curve as below:

HNC-818. User Manual - page 2