Content      ..      1       2         ..

HNC-818. User Manual - page 1

1. Overview

1 Overview

This documentation describes the following CNC systems:

CNC System

Abbreviation

HNC-818A Turning Unit (with

HNC-818A-TU-H

handheld unit)

HNC-818A Turning Unit (without

HNC-818A-TU-X

HNC-818

handheld unit)

HNC-818B Turning Unit

HNC-818B-TU

HNC-818A Milling Unit

HNC-818A-MU

HNC-818B Milling Unit

HNC-818B-MU

2

1. Overview

1.1 CNC Machine Programming

CNC machines conduct workpiece machining based on programming.

The programming has a direct impact on the quality of machining,

productivity, and lifecycle of cutting tools. A good programmer should

have the abilities to master and flexibly use the CNC machine

programming.

Programming means that a programmer, by referring to the workpiece

machining blueprint and craft, creates program codes and instructions for

the workpiece cutting process, machining path, auxiliary operations

during the machining such as tool change, cooling, clamp, and clockwise

(CW) and counter clockwise (CCW) rotation of spindle, etc. Then the

programmer inputs all the programs into the CNC system to run the CNC

machine for the workpiece machining. The CNC programming indicates

the process to create CNC codes and instructions based on the blueprint

and craft, and input them to the CNC system.

The figure below shows the general programming methods and

procedure:

Edit

6

1. Overview

1.2

Machine Coordinate System

Machine coordinate system is a geometric coordinate system and a fixed

coordinate on the machine, which is established to determine the position

of the workpiece on the machine, the special position and motion scope

of the motion parts. In the machine coordinate system, the workpiece is

believed stationary and the tool is in motion. This allows programmers to

determine the machining process based on the blueprint without

considering the movement of the workpiece and the tool.

Standard machine coordinate system adopts the right hand Cartesian

coordinate system. The coordinate is named X, Y, Z which is often

referred to as the basic coordinate system shown in the figure below. It

follows the right-hand rule: stretching out the right hand thumb,

forefinger and middle finger, and keeping them mutually perpendicular;

then the thumb points in the positive direction of the X axis (+X), the

index finger points in the positive direction of the Y axis (+Y), and the

middle finger points in the positive direction of the Z axis (+Z).

+Y

+B

+X

+C

+Y

+A

+X, +Y, +Z

+Z

+A, +B, +C

+X

+Z

The letters A, B, and C are used to define the circumferential feed

coordinate which rotates around X, Y, and Z or the axis parallel to the X,

Y, and Z. According to the right-hand screw rule, if the thumb points in

the direction of +X, +Y, or +Z, the rotation direction of the remaining

four fingers point in the direction of +A, +B and +C.

• Define the Z axis

The axis parallel to the spindle is the Z axis. For the machine

without a spindle, Z axis is perpendicular to the workpiece

clamping surface. The positive direction of Z (+Z) is the direction

where the tool moves away from the workpiece.

7

1. Overview

•

•

Define the X axis

On the machine where the tool rotates, such as milling machine,

drilling machine, or boring machine, if the Z axis is horizontal, the

X axis is positive in the right direction when looking from the tool

(spindle) to the workpiece; If the Z axis is vertical, X axis is

positive in the right direction when looking from the spindle to the

column. The above are based on the motion of tool relative to

workpiece.These directions are relative directions of the tool to the

motion workpiece.

On the machine where the tool rotates, such as turning machine or

grinding machine, the X axis motion is in the radial direction of the

workpiece and parallel to the cross carriage. The direction where

the tool moves away from the workpiece rotation center is the

positive direction of the X axis.

•

Define the Y axis

After defining the positive directions of X and Z axis, you may

define the positive direction of the Y axis based on the right-handed

rectangular Cartesian coordinate system. That is, within the ZX

plane, rotate from + Z to + X, and the right hand-screw should

advance along the + Y direction.

This may differ based on the machine types. The figure below

shows the coordinate system of a six-axis machining center:

•

8

1. Overview

1.3 Machine Origin

The Machine Origin is a fixed point on the machine, which is defined by

the machine manufacturer. It is a benchmark of workpiece coordinate

system, programming coordinate system and reference point. The

Milling Machine Origin may differ for different machine manufacturers.

Some are defined at the center of the machine work table, and some are

defined at the end of the feed travel.

M:machine origin; R: reference point

The origin of the machine is called

Machine Origin (X=0, Y=0, Z=0).

9

1. Overview

1.4 Reference Point of Machine

The machine reference point is exactly defined by the machine

manufacturer in each feed axis with limit switch. The coordinate values

are input into the numerical control system, which are fixed by the

mechanical block along each axis. You may return the tool or the work

table to the reference point by pressing the Reference key on the control

panel. Usually in the CNC milling machines and machining centers, the

machine reference point is coincident with the machine origin. See the

figure below:

Y

Z

R: Reference Point

W: Workpiece Origin

M: Machine Origin

X

10

1. Overview

1.5

Workpiece Coordinate System and Workpiece Origin

The workpiece coordinate system is used to define the position of the

workpiece geometry elements (points, straight lines and arcs). The origin

of the workpiece coordinate system is the workpiece zero. When you

select the workpiece zero, it is recommended to define it in the position

where the dimension of the blueprint can be easily converted into

coordinate values. For the workpiece zero of milling machines, it is

generally defined on one corner of the outer contour of the workpiece;

the zero point in the cutting depth direction is mostly defined on the

surface of the workpiece.

During processing, after the workpiece is installed on the machine with

the clamper, measure the distance between the workpiece origin and the

machine origin (defined by measuring the distance between certain base

level/lines). This distance is called the workpiece origin offset

(the

absolute coordinate value of the machine origin in the workpiece

coordinate system). See the figure below. Before machining, pre-input

the offset value in the CNC system, then during machining, the

workpiece origin offset value is automatically attached to the workpiece

coordinate system, to ensure accurate axis movement on the CNC

machine; therefore, programmers can directly create programs based on

blueprint dimensions, without considering the installation position of the

workpiece on the machine.

Y

Y

O_w Workpiece coordinate system

X

Workpiece origin offset

Y

Machine coordinate system

11

1. Overview

1.6 Programming Origin

Generally, for simple workpiece, the workpiece origin is the

programming origin. For the workpiece with complex shapes, you need

to create several programs or subprograms. To facilitate programming

and reduce coordinate value calculation, the programming origin will not

be necessarily the workpiece origin, but be defined in a position for easy

programming.

The figure below shows the coordinate systems and relative points.

M: Machine origin

R: Machine reference point

W: Workpiece origin

P: Programming origin

12

1. Overview

1.7

Absolute and Relative Coordinate Systems

There are two modes to describe the amount of movement in the CNC

system: the absolute coordinate system and the relative coordinate

system.

-

The absolute coordinate system refers to the coordinate system

where all coordinate points are measured based on a fixed origin.

-

The relative coordinate system refers to the coordinate system

where the end point coordinates of the motion path are measured

based on the starting point.

As shown in the figure below, A, B are two coordinate points. In the

absolute coordinate system, the coordinate value of the two points (A, B)

are

(

x

,

)=(

40,40)

and

(

x

,

)=(

15,20)

respectively; but in

A y

A

B y

B

the relative coordinate system with the origin of point A, the coordinate

value of the point B is

(

x

,

)=(

−

25,−20)

B y

B

Y

Y

A

X

B

O

15

25

X

40

13

2. Preparation

2.1 G-Codes (T)

Attention

After the system is powered on, the G-code marked with the "[ ]" symbol

indicates the initial modal of the same group, while the "『 』" symbol

indicates the equivalent macro name of the G-code.

G

Group

Function

Code

No.

G00

Quick location

[G01]

Linear interpolation

Clockwise (CW) circular interpolation/CW

G02

01

cylindrical helical interpolation

Counter clockwise (CCW) circular interpolation/

G03

CCW cylindrical helical interpolation

G04

00

Pause

G07

Specify the imaginary axis

G08

00

Close look-ahead function

G09

Exact stop verification

G10

Programmable data input

07

[G11]

Cancel programmable data input

G17

XY plane selection

G18

02

ZX plane selection

[G19]

YZ plane selection

G20

Inch input

08

[G21]

Metric input

G28

Return to the reference point

G29

00

Return from the reference point

G30

Return to the reference point 2, 3, 4, and 5

G32

01

Thread cutting

[G36]

Diameter programming

17

G37

Radius programming

[G40]

Cancel tool radius compensation

G41

09

Left cutter compensation

G42

Right cutter compensation

G52

Local coordinate system settings

00

G53

Direct machine coordinate system programming

G54.x

Extended workpiece coordinate system selection

[G54]

Select workpiece coordinate system 1

G55

Select workpiece coordinate system 2

11

G56

Select workpiece coordinate system 3

G57

Select workpiece coordinate system 4

G58

Select workpiece coordinate system 5

15

2. Preparation

G59

11

Select workpiece coordinate system 6

G60

00

Single-orientation

[G61]

Precise stop mode

12

G64

Cutting mode

G65

00

Macro non-modal calling

Inner (outer) diameter roughing compound

G71

cycle

G72

End-face roughing compound cycle

G73

Closed contour compound cycle

G76

Thread cutting compound cycle

G80

Inner (outer) diameter cutting cycle

G81

End-face cutting cycle

06

G82

Thread cutting cycle

G74

End-face deep-hole drilling cycle

G75

Outer diameter grooving cycle

G83

Axial drilling cycle

G87

Radial drilling cycle

G84

Axially rigid tapping cycle

G88

Radial rigid tapping cycle

[G90]

Absolute programming mode

13

G91

Incremental programming mode

G92

00

Workpiece coordinate system settings

G93

Inverse-time feed

[G94]

14

Feed per minute

G95

Feed per revolution

[G97]

Disable constant linear velocity control

19

G96

Enable constant linear velocity control

G101

Axis release

G102

Axis acquisition

G103

Command channel loader

G103.1

Run the command channel loader

G104

Channel synchronization

G108

00

Change the spindle to the C-axis

『STOC』

G109

Change the C-axis to spindle

『CTOS』

G110

Alarm

G115

Redefine the rotary axis angular resolution

16

2. Preparation

2.2 G-Codes (M)

Attention

After the system is powered on, the G-code marked with the "[ ]" symbol

indicates the initial modal of the same group, while the "『 』" symbol

indicates the macro name of the G-code.

G

Group

Function

Code

No.

G00

Quick location

[G01]

Linear interpolation

CW circular interpolation/ CW cylindrical helical

G02

01

interpolation

CCW circular interpolation/ CCW cylindrical

G03

helical interpolation

G04

00

Pause

G05.1

27

High-speed high-precision mode

G07

Specifies the imaginary axis

G07.1

Cylindrical surface interpolation

00

G08

Close look-ahead function

G09

Exact stop verification

G10

Programmable data input

07

[G11]

Cancel programmable data input

G12

Enable polar coordinate interpolation

18

[G13]

Disable polar coordinate interpolation

[G15]

Disable polar coordinate programming

16

G16

Enable polar coordinate programming

[G17]

XY plane selection

G18

02

ZX plane selection

G19

YZ plane selection

G20

Inch input

08

[G21]

Metric input

G24

Enable Mirror function

03

[G25]

Disable Mirror function

G28

Return to the reference point

G29

00

Return from the reference point

G30

Return to the reference points 2, 3, 4, and 5

[G40]

Cancel tool radius compensation

G41

09

Left cutter compensation

G42

Right cutter compensation

G43

Positive tool length compensation

G44

10

Negative tool length compensation

[G49]

Cancel tool length compensation

17

2. Preparation

[G50]

Disable the Zoom function

04

G51

Enable the Zoom function

G52

Local coordinate system setting

00

Direct machine coordinate system

G53

programming

Extended workpiece coordinate system

G54.x

selection

[G54]

Select workpiece coordinate system 1

G55

Select workpiece coordinate system 2

11

G56

Select workpiece coordinate system 3

G57

Select workpiece coordinate system 4

G58

Select workpiece coordinate system 5

G59

Select workpiece coordinate system 6

G60

00

Single-orientation

[G61]

12

Precise stop mode

G64

Cutting mode

G65

00

Macro non-modal calling

G68

Start rotation transformation

05

[G69]

Cancel rotation transformation

G73

Deep-hole drilling cycle

G74

Reverse-tapping cycle

G76

Fine-boring cycle

[G80]

Cancel fixed cycle

G81

Centre-drilling cycle

G82

Drilling cycle with pause

G83

Deep-hole drilling cycle

G84

Tapping cycle

G85

Boring cycle

G86

Boring cycle

G87

06

Anti-boring cycle

G88

Boring cycle (hand boring)

G89

Boring cycle

G181

Arc groove cycle (Type 1)

G182

Arc groove cycle (Type 2)

G183

Circumference groove milling cycle

G184

Rectangular groove cycle

G185

Circular groove cycle

G186

End-face milling cycle

G188

Rectangular boss cycle

G189

Circular boss cycle

[G90]

Absolute programming mode

13

G91

Incremental programming mode

G92

00

Define workpiece coordinate system

18

2. Preparation

G93

Inverse-time feed

[G94]

14

Feed per minute

G95

Feed per revolution

[G98]

Fixed cycle returning to the starting point

15

Fixed cycle returning to the reference

G99

point

G101

Axis release

G102

Axis acquisition

G103

Command channel loader

G103.1

Run the command channel loader

G104

Channel synchronization

G108

00

Change the spindle to the C-axis

『STOC』

G109

Change the C-axis to spindle

『CTOS』

G115

Redefine the rotary axis angular resolution

NURBS

NURBS spline interpolation

HSPLINE

HSPLINE spline interpolation

19

3. Program Structure

3 Program Structure

A program is a set of commands and data transferred to the CNC system.

A program consists of a number of program blocks which follow a

certain structure, syntax and format rules. Each block consists of a

number of commands. See the figure below:

Program

%1000

N01 G91 G00 X50 Y60

N10 G01 X100 Y500 F150 S300 M03

Block

N

N200

M02

Command

20

3. Program Structure

3.2 Program Block Format

A program block specifies the commands executed by a numerical

control device.

The block format specifies the syntax of the functional words of each

program block. See the figure below:

Block

N..

G..

X..

F..

M..

S..

Spindle Function

Auxiliary Function

Feed Function

Dimension word

Preparatory function

Block number

22

3. Program Structure

3.6 Sub-Programs

When a fixed machining operation is repeated in a program, you may set

it as a sub-program and input it into the program to simplify the

programming.

Execution Process

Main program

Sub-program 1001

Sub-program 1002

%1001;

%1002;

……

……

……

M98P1001;

M98P1002;

……

……

M99;

……

M99;

M98P2001;

……

Sub-program 2001

M98P1001;

%2001;

……

……

……

M30;

M99;

Call Sub-program

You may call a sub-program with M98 or G65. For the method of calling

a sub-program with M98, see the description of M98 in section 4. For the

method of calling a sub-program with G65, see section 13.

26

Content      ..      1       2         ..

//////////////////////