HNC8 Series CNC Controller. Programming Manual (V2.4)

%0330

N1 T0101; Set coordinate system, select No.1 tool

N2 G00 X80 Z80; Move to starting point of program

N3 M03 S400; Spindle rotates CW at 400r/min

N4 G00 X60 Z5; Move to starting point of cycle

N5 G73U3W0.9R3P6Q13X0.6Z0.1F120; Closed roughing cycle

N6 G00 X0 Z3; Contour finishing starts, move to extension line of chamfer

N7 G01 U10 Z-2 F80;

2×45°chamfer finishing

N8 Z-20; Φ10 outer circle finishing

N9 G02 U10 W-5 R5; R5 arc finishing

N10 G01 Z-35; Φ20 outer circle finishing

N11 G03 U14 W-7 R7; R7 arc finishing

N12 G01 Z-52; Φ34 outer circle finishing

N13 U10 W-10; Cone finishing

N14 U10; Exit machined surface, contour finishing end

N15 G00 X80 Z80; Return to starting point of program

N16 M30; Spindle stop, main program end and reset

Note

(1) The rough turning cycle is realized by the G73 command with addresses P and Q. The F, S

and T functions specified in the motion command are invalid. But the F, S and T functions

specified in the G72 block or the previous block are valid.

320

(2) When the constant speed limit is used for cutting speed control, the G96 or G97 specified in

the movement command between "ns" and "nf" is invalid. It is valid to specify G96 or G97 in the

G73 block or the previous block. The blocks between the sequence numbers na and nf cannot call

subprogram.

(3) G72 cannot be the same line with M code.

(4) In the any line with scanning mode, the blocks between ns and nf cannot be specified.

(5) The number of divisions R can only be given as an integer value. If the specified value is a

decimal, it will be rounded up.

17.4

Thread Cutting Multiple Repetitive Cycle (G76)

Function and Purpose



Threading is a forming processing, and the cutting amount per cut cannot be too large, so

processing a threaded part often requires multiple processing to complete.

This command can use a cycle command to realize multiple reciprocating motions and finally

complete the processing of threaded parts. It includes multiple roughing and at least one finishing.

Command Format

G76 C(c) R(r) E(e) A(a) X(x) Z(z) I(i) K(k) U(d) V(dmin) Q(d) P(p) F

Parameter

Meaning

Number of finishing (c=1 to 99), modal value

Undercut length on Z (The positive or negative R value determines the direction

of undercut on Z axis), modal value

Undercut length on X (The positive or negative E value determines the direction

of undercut on X axis), modal value

Tool nose angle (A value is a two-digit integer), modal value; the value is larger

than 10° and smaller than 80°

X Z

Coordinate of the effective thread end point C in absolute programming;

directional distance from the end point C of thread to starting point A of cycle

in incremental programming

Radius difference between the starting point and the end point of thread cutting

(The positive or negative I value determines the direction of taper); I=0 for

straight thread, and I is negative for normal tapered thread

Thread cutting height (K is the radius, and is generally the thread tooth height)

Finishing allowance (d is the radius)

321

Min. cutting depth

(dmin is the radius); when the n^th cutting depth

d

nd

n 1 is smaller than dmin, the cutting depth is set to dmin

The first cutting depth (d is the radius)

Spindle rotation angle from the spindle reference pulse to the cutting start point

Thread lead (same as G32), F is in metric

Description



 For machining path of G76 thread multiple repetitive cycle, see the figure below,

There are 4 paths for each reciprocation,

1^st path A→B, R rapid traverse feed

2^nd path B→C, F speed thread feed

3^rd path C→D, R rapid traverse feed (including E, R undercut path)

4^th path D→A, R rapid traverse feed

 Cutting depth setting for thread multiple repetitive cycle, see the figure below,

322

Example

Example 1: Use the thread cutting multiple repetitive cycle G76 for programming. The thread to

be processed is ZM60×2, the workpiece size is shown in the figure below, and the size in brackets

is obtained according to the standard. (Tan1.79=0.03125).

%3331

N1 T0101; Select No. 1 tool, and determine the coordinate system

N2 G00 X100 Z100; Move to the starting point of program or tool change position

N3 M03 S400; Spindle rotates CW at 400r/min

N4 G00 X90 Z4; Move to the starting point of simple cycle

N5 G80 X61.125 Z-30 I-1.063 F80; Machine the outer surface of tapered thread

N6 G00 X100 Z100 M05; Move to the starting point of program or tool change

position

N7 T0202; Change to No. 2 tool, and determine the coordinate system

N8 M03 S300; Spindle rotates at 300r/min

N9 G00 X90 Z4; Move to the starting point of thread

N10 G76C2R-3E1.3A60X58.15Z-24I-0.875K1.299U0.1V0.1Q0.45F2

N11 G00 X100 Z100; Return to the end point of program or tool change position

N12 M05; Spindle stop

N13 M30; Main program end and reset

Note

(1) The cycle processing is realized based on the X(x) and Z(z) commands in the G76 block. In

323

incremental programming, note the sign of u and w (determined by the direction of the tool path

AC and CD);

(2) G76 is used to perform the single-side cutting, which reduces the force on the tool tip. The

cutting depth for the first cut is

 d, the total cutting depth for the nth cut is

d

n_{, and the}

（



1

）

amount of cutting depth in each cycle is d

;

(3) In the single-side cutting diagram, the cutting speed from point B to C is specified by the

thread cutting speed, and other paths are the rapid traverse feed.

(4) During thread cutting, the feed hold and reset bottons are invalid;

(5) During thread cutting, feed override is invalid;

(6) To avoid tool interference, the starting point of the thread cutting cycle should be set above

the apex of the thread pitch;

(7) When the tapered thread cutting is executed, the thread pitch is calculated in the way of axis,

and the actual processing speed is calculated in the way of generatrix.

18 Programming Simplifying Function (M)

18.1

Mirroring Function（G24，G25）

Function and Purpose



When editing a symmetrical shape processing program, user only needs to program any one side

of the shape for the processing of the other side of the shape, which can save the time required

for programming. At this time, the most effective function is the mirroring function.

For example, as shown in the figure below, when there is a program for processing the shape A

on the left, the shape B that is symmetrical to the A can be completed on the right by mirroring

the program.

324

Mirroring axis

Command Format

G24 IP_; Establish mirroring

…… Tool path programming commands

G25 IP0; Cancel mirroring

Parameter

Meaning

Mirroring axis position

Description



(1) In G24, the mirroring axis and mirroring enter coordinates are specified in absolute or

incremental programming.

(2) In G24, user can specify axisymmetric mirroring and point-symmetric mirroring.

a) Axisymmetric mirroring

(G17/G18/G19) G24 α_/β_;

…… ;

d) G25;

Parameter

Meaning

Plane selection for mirroring, this plane should include programmed tool

G17/G18/G19：

path

Symmetry axis of mirroring. Only one of α_ and β_ can be specified. α

G24 α_/β_：

represents the first axis of the selected plane, and β represents the second

axis of the selected plane. If an axis on a non-selected plane is specified, the

325

system alarms.

……：

Programmed tool path commands

Cancel mirroring. When running the program, only write G25, or α and β

G25α0/β0：

after G25 are specified as any values, the mirroring function can be

cancelled.

Point symmetry mirroring

(G17/G18/G19) G24 α_ β_;

…… ;

G25;

Parameter

Meaning

Plane selection for mirroring, this plane should include the programmed tool

G17/G18/G19：

path

Symmetry axis of mirroring. When α_ or β_ is omitted, the current tool

G24 α_β_：

position is defaulted. If an axis on a non-selected plane is specified, the

system alarms.

……：

Programmed tool path commands

Cancel mirroring. When running the program, only write G25, or α and β after

G25 α0 β0：

G25 are specified as any values, the mirroring function can be cancelled.

The diagram of axisymmetric and point-symmetric mirroring is as follows:

Mirroring path 1

Programmed path

Mirroring path 2

Mirroring path 3

A mirror image path 1 and the programmed path are axisymmetrical, the axis of

symmetry is α=50;

B mirror image path 2 and the programmed path are point-symmetrical, and the

326

symmetrical point is (50, 60);

C mirror image path 3 and the programmed path are axisymmetric, and the

symmetry axis is β=60;

(3) By specifying G24 α_, the β-axis symmetry mirror can be established.

(4) When the β-axis mirror image is established, specify G25 α0 to cancel the β-axis mirror image.

For example, when G24 X0 Y0 is specified to establish the point-symmetric mirroring, user can

cancel the Y-axis symmetrical mirroring and only specify the X-axis symmetrical mirroring by

specifying G25 X0.

(5) When only mirroring is specified on the first axis of the specified plane, the rotation direction

and compensation direction in arc, tool radius compensation, and coordinate rotation are all

reversed.

(6) The mirror image center of the local coordinate system will move due to the preset coordinate

system and the change of the workpiece coordinate.

(7) G24 block and G25 block must be specified seperately.

(8) G24 is a modal command, can be canceled by G25 after mirroring function is finished.

(9) When no axis follows G25, all mirroring is canceled.

(10) When the reference point return command (G28, G30) is executed in mirror image, the mirror

image is valid in the motion before the intermediate point is reached, so the mirror image is not

executed in the motion from the intermediate point to the reference point.

Mirrored

intermediate point

Intermediate point

Mirroring path

Programmed path

Mirroring axis

(11) When the return from origin command (G29) is specified in the mirroring, the mirroring is

performed to the intermediate point.

(12) The mirror image is not executed to G53.

(13) The mirror image is processed after the tool radius compensation (G41, G42) is executed, so

the cutting path as shown in the figure below is performed.

327

Programmed path

Path when only the tool compensation is executed

Path when only the mirroring is executed

Path when both mirroring and tool compensation

are executed

Example

Use the mirror image function to program the contour as shown in the figure: set the starting point

of the tool to be 100mm from the upper surface of the workpiece, and the depth of cut is 5mm.

%3331

；Main program

G92 X0 Y0 Z100

G91 G17 M03 S600

M98 P100

；Machining ①

G24 X0

；Y-axis mirror image, the mirroring position is X=0

M98 P100

；Machining ②

G24 Y0

；X, Y axis mirror image, the mirroring position is (0, 0)

M98 P100

；Machining ③

G25 X0

；X-axis mirroring continues to be effective, cancel Y-axis mirroring

M98 P100

；Machining ④

G25 X0 Y0

；Cancel mirroring

328

18.2

Scaling Function（G50，G51）

Function and Purpose



When executing the scaling function, the programmed path is enlarged or reduced based on the

given scaling factor.

Command Format

G51 IP_ P_ ； Scaling starts

……

G50

； Cancel scaling

Parameter

Meaning

Specify the coordinates of the scaling center point. If it is not specified,

specify the current point as the scaling center point.

This command always specifies the absolute position of the scaling

center in the workpiece coordinate system.

Specify the scaling factor of each axis.

All axes are scaled by this factor.

Description



(1) Designation of scaling axis, scaling center and magnification

After issuing the G51 command, the scaling mode is entered. The G51 command only specifies

the scaling axis, scaling center and magnification and doesn’t specify the movement.

Although executing the G51 command will enter the scaling mode, in fact the effective axis for

scaling is only the axis for which the scaling center is set.

(a) Scaling center

The center of the scaling is specified based on the absolute/incremental mode (G90/G91). In the

G51 block, whether it is in incremental or absolute mode, the center of the scaling refers to the

absolute position in the workpiece coordinate system.

Even if the current position is the center, it must be specified.

The effective axis for scaling is limited to the axis for which the scaling center is specified.

(b) Scaling magnification

The scaling magnification is specified with the address P.

The magnification for scaling only can be specified after G51.

330

Scaling magnification ranges from 0.000001 to 99999999999

When the scaling magnification is not specified, 1 is specified by default.

The scaling magnification exceeds the upper limit of the magnification command range.

(2) Scaling is cancelled. After specifying G50, the scaling is cancelled.

Example

Example 1: Use the scaling function to create the program with 1/2 scaling and the program

without scaling in the figure below.

Scaling center

Programmed path after 1/2 scaling

Programmed path without scaling

%1234

G92 X0 Y0 Z0；

G90 G51 X-100. Y-100. P0.5；

G00 G43 Z-200. H02；

G41 X-50. Y-50. D01；

G01 Z-250. F1000；

Y-150. F200；

X-150.；

G02 Y-50. J50.；

G01 X-50.；

331

G00 G49 Z0；

G40 G50 X0 Y0；

G90 G51 X-100. Y-100. P1；

G00 G43 Z-200. H02；

G41 X-50. Y-50. D01；

G01 Z-250. F1000；

Y-150. F200；

X-150.；

G02 Y-50. J50.；

G01 X-50.；

G00 G49 Z0；

G40 G50 X0 Y0；

M30;

Example 2: Use the scaling function to create the program of the contour as shown in the figure

below: The vertices of the triangle ABC are A (10, 30), B (90, 30), C (50, 110), and the triangle

A'B'C 'is the zoomed one, where the scaling center is D (50, 50), the scaling factor is 0.5 times,

and the starting point of the tool is 50mm from the upper surface of the workpiece.

332

%3332

；Main program

G92 X0 Y0 Z60

G17 M03 S600 F300

G43 G00 Z14 H01

X110 Y0

#51=0

M98 P100

；Machine triangle ABC

#51=6

G51 X50 Y50 P0.5

；Scaling center (50,50), scaling factor 0.5

M98 P100

；Machine triangle A'B'C'

G50

；Cancel scaling

G49 Z60

G00 X0 Y0

M30

%100

；Subprogram (the processing programi of triangle ABC)

N100 G41 G00 Y30 D01

N120 Z[#51]

N150 G01 X10

N160 X50 Y110

N170 G91 X40 Y-80

N180 G90 Z[#51]

N200 G40 G00 X110 Y0

N210 M99

Note

(1) When there is tool compensation, perform scaling first, and then tool radius compensation and

tool length compensation. The scaling does not change the tool radius compensation value and

tool length compensation value.

(2) Scaling is only valid for traverse commands in auto mode. It is invalid for the traverse in JOG.

When the movement is in JOG mode, the breakpoint must be returned first.

(3) Scaling is valid to the axes of which X, Y, Z are specified, and invalid to the axes of which X,

Y, Z are not specified.

(4) The G51 block must be specified separately.

333

(5) If M02 or M03 command is specified in scaling mode, or NC reset is executed, the scaling is

canceled.

(6) When the coordinate system is offset (G92, G52 commands) or switched in the scaling mode,

then the scaling center will be offset based on the coordinate system offset amount.

(7) When G28, G30, or G29 command is secified in scaling mode, the scaling is not canceled.

(8) When the G51 command is issued in the scaling mode, the axis of the newly-specified center

becomes the effective scaling axis. The magnification is based on the newly specified G51.

(9) When G60 (unidirectional positioning) is issued in scaling mode, neither the final positioning

point nor the crawling amount is scaled.

(10) When the graphics rotation is specified in the scaling mode, the graphics rotation center and

the radius will be scaled.

(11) If the scaling command is issued in the graphics rotation subprogram, the radius of the

graphics rotation is not scaled, but only the shape determined by the subprogram is scaled.

18.3

Rotation Transformation（G68，G69）

Function and Purpose



The rotation transformation is used to rotate the programmed processing path around the rotation

center by a specified angle. If the shape of the workpiece is composed of many identical graphics,

the graphics unit can be compiled into a subprogram which is then called by the rotation

transformation command of the main program.

Command Format

G17/G18/G19； Select a rotation plane

G68 IP_ P_； Establish rotation transformation

……

G69；

Cancel rotation transformation

Parameter

Meaning

To specify coordinates of the rotation center. If it is not specified, it is the

current point of the tool.

The absolute position in the workpiece coordinate system whether it is in

absolute or incremental mode

Rotation angle (unit: degree), counterclockwise rotation indicates a positive

value, clockwise rotation indicates a negative value

334

Description



(1) The coordinate of the rotation center are always specified as an absolute value. Even if it is

specified as an incremental address, it will not be treated as an incremental value. Regardless of

the rotation angle specified in G90 or G91, P is always the absolute value of the angle of the first

axis in positive direction in the specified reference plane.

(2) If the coordinate of the rotation center is omitted, the position where the G68 command is

located will become the rotation center.

(3) The value of rotation angle P ranges from

-360 to

360. The value is positive for

counterclockwise direction, and negative for clockwise direction. When the angle command

exceeds 360 degrees, the system will issue that the parameter is illegal.

(4) The rotation angle P is a modal value and will not change until a new angle is specified next

time. The rotation angle can be omitted. If the rotation angle is omitted when G68 is specified for

the first time, P will be regarded as 0. If the rotation angle is omitted when G68 is not specified

for the first time, P will inherit the previous rotation angle.

(5) Use G69 to cancel it after the rotation transformation is completed. If M02 or M30 is specified

in the coordinate rotation mode or the reset button is pressed, the coordinate rotation will be

cancelled.

(6) In coordinate rotation mode, G68 is not displayed on the modal information screen, and G69

is not displayed after the mode is cancelled.

(7) The coordinate rotation function is valid in both auto and single-block working modes.

Example

Use the rotation function to program the contour as shown in the figure: the starting point of the

tool is 50mm from the upper surface of the workpiece, and the depth of cut is 5mm.

335

%3333

；Main program

N10 G92 X0 Y0 Z50

N15 G90 G17 M03 S600

N20 G43 Z-5 H02

N25 M98 P200

；Machine ①

N30 G68 X0 Y0 P45

；Rotate 45°

N40 M98 P200

；Machine ②

N60 G68 X0 Y0 P90

；Rotate 90°

N70 M98 P200

；Machine ③

N20 G49 Z50

N80 G69 M05 M30

；Cancel rotation

%200

；Subprogram (Program of graphic

①)

G41 G01 X20 Y-5 D02 F300

N105 Y0

N110 G02 X40 I10

N120 X30 I-5

N130 G03 X20 I-5

N140 G00 Y-6

N145 G40 X0 Y0

N150 M99

Note

(1) The traverse command following G68 and G69 must be an absolute value command.

(2) In coordinate rotation mode, G codes related to the reference point (G28, G29, G30, etc.) and

commands used to change the coordinate system (G52, G54 to G59, G54X, G92, etc.) cannot be

specified. Otherwise, the coordinate rotation command needs to be cancelled first.

(3) G68 and G69 are specified in the tool radius compensation mode, and the rotation plane must

be consistent with the tool radius compensation plane.

(4) If the coordinate rotation command is designated without the coordinate rotation specifications,

it will be executed according to the detailed instructions (2) and (3).

(5) The G68 block must be specified separately.

(6) Tool radius compensation, tool length compensation, tool offset and other compensation

operations are operated after the coordinate rotation is performed. When rotation and scaling are

needed, user should enable the rotation function first and then the scaling function, otherwise

system will prompt "nesting order change error".

336

19 User Macro and Subprogram Calling

19.1

User Macro Program

Function and Purpose



A user macro program is a program with specific control functions created by variables, logic

operations, and control commands.

User macro program is a programming method similar to high-level language, which allows users

to use variables, logic operations and conditional transfer and other control commands, makeing

it more convenient to create the same program than traditional methods. At the same time, some

same processing operations can be programmed into general programs with macro programs for

users to call in cycles, as shown in the figure below for bolt hole processing.

After storing the bolt hole machining program in the above figure created by the macro program

in the CNC, user can call this program to machine the bolt hole at any time, and just fill in the

bolt hole attributes such as the number of holes and deviation angle when calling. This is as if a

bolt hole function has been added to the CNC.

19.1.1 Variable

Function and Purpose



A certain address in the program is not directly specified with a numerical value, but with a

variable. When the program is running, the variable is assigned based on a predetermined situation

to improve the generality of the program.

In the macro program, user can use variables in the parameters of the axis movement distance,

such as G01 X[#54]F1000, at this time #54 is the variable, and user can perform some operations

such as assignment before calling.

337

Command Format

#○○○=□□□□

#○○○=[ Expression]

Variable

Description

Example

representation

A is composed of numbers from 0 to 9

#21

Value A

#23

Expression Operation command Expression

#1+#2

#B（expression）

Function [expression]

COS[#3]

Note

It is not allowed to use variable names directly in user macro programs. Variables are designated

by the variable symbol (#) and the following variable number.

Description



Variable types

According to the purpose of variables, variables can be divided into local variables, global

variables, and system variables. In addition, the access attributes of different variables are also

different. Some variables are read-only, and some are readable and writable.

Constant

Some constants with constant values are defined in the system for users to use. The attributes of

these constants are read-only.

PI：Pi π

TRUE： True, used for conditional judgment, indicating that the condition is ture

FALSE： False, used for conditional judgment, indicating that the condition is not ture

Note

When the constant PI is used, due to the calculation error, it needs to be dealt with at the time of

ending conditions, otherwise an abnormal situation will occur.

Local Variable

Local variables refer to the variables used in the macro program. The local variable #i (i is a value,

such as #10) used in macro program A is called in the current state, which is different with the #i

used in macro program A called in other states. Therefore, when multiple levels of macros are

called, such as calling macro B from macro A, if the local variable used in macro A is incorrectly

used in macro B, the value will be destroyed.

338

The system provides #0 to #49 as current local variables, and their access attributes are readable

and writable.

The system provides 6 levels of nesting. The corresponding local variables of each level are as

follows. The access attributes of these local variables are readable:



#200～#249 Level 0 local variable



#250～#299 Level 1 local variable



#300～#349 Level 2 local variable



#350～#399 Level 3 local variable



#400～#449 Level 4 local variable



#450～#499 Level 5 local variable

Global variable

Different from local variables, global variables are commonly used between subprograms and

macro programs, and their values remain unchanged. That is, #i used in one macro is the same as

#i used in other macros. In addition, the public variable #i calculated by a certain macro can be

used in other macros.

The system provides #50 to #199 as global variables, and their access attributes are readable and

writable.

System variable

System variables are variables whose purposes are fixed in the system. There are 3 types of

attributes for the system variables: read-only, write-only, and read/write. The attributes varies with

system variables.

Undefined variable

The value of variables not defined in the system defaults to 0

Example：%1234

G54

G90G01 X10Y10F1000

X[#1]Y40

; The coordinate value of the workpiece coordinate system is (0, 40)

M30

User-defined variable

User-defined variable：500 to 999

50000 to 54999

#500 - #999

R/W

Global variable

#50000 - #54999

R/W

Global variable

Note

339

When machine user parameter 010091 "#500 - #999 user macro variable enable" is 1, #500 - #999

are valid user-defined variables. User-defined variables are saved after power off.

"USERMACCFG.XML" needs to be configured (configured based on usage requirements, too

many variables configured will occupy too much system storage space), and the configured file

is correctly imported into the system in the "Data Management-User Macro Variable Name"

interface.

USERMACCFG.XML（the file comes from the internal CNC system

：

<?xml version="1.0" encoding="GB2312"?><USERMACCFG version="1.0">

</USERMACCFG>

Note

The numeric format in type needs to be configured correctly (FLOAT represents the data type of

floating point, and INT represents the data type of integer), otherwise the macro program cannot

run normally.

Channel-related variables

Variable number

Attribute

Description

Channel parameter

Channel 00：(00000 to 03999)

#0～#49

R/W

Current local variable

#50～#199

Reserved

#200～#249

Level 0 local variable

#250～299

Level 1 local variable

#300～#349

Level 2 local variable

#350～#399

Level 3 local variable

340

#400～#449

Level 4 local variable

#450～#499

Level 5 local variable

#1000～#1008

Machine position of current channel axis

(9-axis)

#1009

Diameter programming of lathe

#1010～#1018

Programmed machine position of current

channel axis (9-axis)

#1019

Reserved

#1020～#1028

Programmed workpiece position of current

channel axis (9-axis)

#1029

Reserved

#1030～#1038

Workpiece origin of current channel axis

(9-axis)

#1039

Coordinate system

#1040～#1048

R/W

G54 origin of current channel axis (9-axis)

#1049

G54 axis mask

#1050～#1058

R/W

G55 origin of current channel axis (9-axis)

#1059

G55 axis mask

#1060～#1068

R/W

G56 origin of current channel axis (9-axis)

#1069

G56 axis mask

#1070～#1078

R/W

G57 origin of current channel axis (9-axis)

#1079

G57 axis mask

#1080～#1088

R/W

G58 origin of current channel axis (9-axis)

#1089

G58 axis mask

#1090～#1098

R/W

G59 origin of current channel axis (9-axis)

#1099

G59 axis mask

#1100～#1108

G92 origin of current channel axis (9-axis)

#1109

G92 axis mask

#1110～#1118

Break-off position of current channel axis

(9-axis)

#1119

Break point axis mark

#1120～#1149

R/W

Modal variable of canned cycle

#1150～#1189

Groups 0 to 39 modal of G code

#1190

User-defined input

#1191

User-defined output

#1192～#1199

Reserved

#1200～#1209

AD input

#1210～#1219

DA output

#1220

M3/4/5

#1221

G94 F value

#1222

Tapping F value

#1223~#1226

Tapping spindle speed

#1227

Valid radius compensation D number

341

#1228

Valid length compensation H number

#1229

cmd_feed

#1300～#1308

Relative zero of current channel axis (9-

axis)

#1309

Reserved

#1310～1318

Programmed machine position of current

channel axis (9-axis)

#1319

Reserved

#1320～#1328

G28 intermediate point

#1329

G28 axis mask

#1330～#1338

G52 origin

#1339

Reserved

#1340~#1349

G31 measurement machine command

#1350~#1359

Reserved

#1360~#1369

G31 measurement machine actual

#1370~#1399

Reserved

#1400~#1408

R/W

G54 offset

#1409

Reserved

#1410~#1418

R/W

G55 offset

#1419

Reserved

#1420~#1428

R/W

G56 offset

#1429

Reserved

#1430~#1438

R/W

G57 offset

#1439

Reserved

#1440~#1448

R/W

G58 offset

#1449

Reserved

#1450~#1458

R/W

G59 offset

#1459~#3999

Reserved

Note

The variables corresponding to the origin and offset of the workpiece coordinate system G54 -

G59 in the current channel are both readable and writable, and are saved after power off.

Variables related to the extended coordinate system

Variable number

Attribute

Description

Channel variable

Channel 00：(40100 to 40639)

#40100～#40108

R/W

G54.1P1

#40109～#40117

R/W

G54.1P2

#40118～#40126

R/W

G54.1P3

#40127～#40135

R/W

G54.1P4

#40136～#40144

R/W

G54.1P5

#40145～#40153

R/W

G54.1P6

342

#40154～#40162

R/W

G54.1P7

#40163～#40151

R/W

G54.1P8

#40172～#40180

R/W

G54.1P9

#40181～#40189

R/W

G54.1P10

#40190～#40198

R/W

G54.1P11

#40199～#40207

R/W

G54.1P12

#40208～#40216

R/W

G54.1P13

#40217～#40225

R/W

G54.1P14

#40226～#40234

R/W

G54.1P15

#40235～#40243

R/W

G54.1P16

#40244～#40252

R/W

G54.1P17

#40253～#40251

R/W

G54.1P18

#40262～#40270

R/W

G54.1P19

#40271～#40279

R/W

G54.1P20

#40280～#40288

R/W

G54.1P21

#40289～#40297

R/W

G54.1P22

#40298～#40306

R/W

G54.1P23

#40307～#40315

R/W

G54.1P24

#40316～#40324

R/W

G54.1P25

#40325～#40333

R/W

G54.1P26

#40334～#40342

R/W

G54.1P27

#40343～#40351

R/W

G54.1P28

#40352～#40360

R/W

G54.1P29

#40361～#40369

R/W

G54.1P30

#40370～#40378

R/W

G54.1P31

#40379～#40387

R/W

G54.1P32

#40388～#40396

R/W

G54.1P33

#40397～#40405

R/W

G54.1P34

#40406～#40414

R/W

G54.1P35

#40415～#40423

R/W

G54.1P36

#40424～#40432

R/W

G54.1P37

#40433～#40441

R/W

G54.1P38

#40442～#40450

R/W

G54.1P39

#40451～#40459

R/W

G54.1P40

#40460～#40468

R/W

G54.1P41

#40469～#40477

R/W

G54.1P42

#40478～#40486

R/W

G54.1P43

#40487～#40495

R/W

G54.1P44

#40496～#40504

R/W

G54.1P45

#40505～#40513

R/W

G54.1P46

#40514～#40522

R/W

G54.1P47

#40523～#40531

R/W

G54.1P48

#40532～#40540

R/W

G54.1P49

343

#40541～#40549

R/W

G54.1P50

#40550～#40558

R/W

G54.1P51

#40559～#40567

R/W

G54.1P52

#40568～#40576

R/W

G54.1P53

#40577～#40585

R/W

G54.1P54

#40586～#40594

R/W

G54.1P55

#40595～#40603

R/W

G54.1P56

#40604～#40612

R/W

G54.1P57

#40613～#40621

R/W

G54.1P58

#40622～#40630

R/W

G54.1P59

#40631～#40639

R/W

G54.1P60

Note

The variables corresponding to the origin and offset of the workpiece coordinate system G54~G59

in the current channel are both readable and writable, and are saved after power off.

Variables related to tool

Tool data：#70000 to #89999

Each tool occupies 200 numbers, a total of 100 tools, a total of 20,000

numbers

Relative coding range of No. 0 tool：000 to 199

Relative coding range of No. 1 tool：200 to 399

Relative coding range of No. 99 tool：18000 to 19999

#70005

Lathe tool nose direction

#70006

R/W

Tool length of milling cutter or X offset

value of lathe tool

#70007

Y offset of lathe tool

#70008

Z offset of lathe tool

#70009

Reserved

#70010

Reserved

#70011

R/W

Tool radius of milling cutter or tool nose

radius of lathe tool

#70012~#70028

Reserved

#70029

R/W

Length wear of milling cutter or Z offset

wear of lathe tool

#70030

Y offset wear of lathe tool

#70034

R/W

Radius wear of milling cutter or X offset

wear of lathe tool

#70035~#70100

Reserved

#70101

Tool life monitoring type

#70104

Max. life of cutting time

#70105

Life of pre-warning cutting time

#70106

Life of current cutting time

344

#70107

Life of max. cutting times

#70108

Life of pre-warning cutting times

#70109

Life of actual cutting times

Note

The variables corresponding to the tool radius compensation value, length compensation value,

and wear value can be read and written, and can be saved after power off.

（F） Class A command (T)

#50000

X coordinate of tool measuring

#50003

Z coordinate of tool measuring

instrument calibration

#[50006+N]

Avarage measured value of No.

Average measured value of No. N

#[51006+N]

N tool on Z

tool on X

#54005

Tool retraction amount

#54006

Tool nose angle A

#54007

Finishing times

#54008

(FUNAC) Q value

#54009

（F）R value

#54010

Undercut angle

#54011

Thread chamfer amount

#54012

G83 Axial drilling cycle

H1/H2 Retraction mode

#54013

G83 Retraction amount

#54014

G84 Tapping axis selection

#54015

G84 H1/H2 Retraction mode

#54016

G84 Retraction amount

#54017

G88 Tapping axis selection

#54990

Measuring

instrument

center

position X

#54992

Measuring instrument center

position Z

Note

The (F) Class A command (T) function in the CNC system occupies the above-mentioned user-

defined macro variables. Please do not use the above-mentioned user-defined macro variables.

Workpiece measurement F

Variable

Description

Variab

Description

number

numbe

#600

Distance from actual center to trigger

#630

Center position value in X plane or

point in X positive direction

X direction

#601

Distance from actual center to trigger

#631

Center position value in Y plane of

point in X negative direction

Y direction

#602

Distance from actual center to trigger

#632

Z plane position value

point in Y negative direction

#603

Distance from actual center to trigger

#633

Position offset value in X direction

point in Y positive direction

#604

Probe length value

#634

Position offset value in Y direction

#605

Eccentricity of probe in X direction

#635

Position offset value in Z direction

345

#606

Eccentricity of probe in Y direction

#636

Dimension value: width/diameter

#607

Trigger radius of probe in X direction

#637

Dimension offset vlaue

#608

Trigger radius of probe in Y direction

#638

Angle value (unit: degree)

#609

Second measurement speed of probe

Note

The workpiece measurement function in the CNC system occupies the above-mentioned user-

defined macro variables. If the debugger uses other user-defined macro variables when debugging

the workpiece measurement function, instead of the user-defined macro variables listed in the

above table, the debugger will replace or add them to the table, and inform and provide it to the

user. Please do not use the above user-defined macro variables.

Tool measurement

Variable

Description

Variable

Description

number

#642

Laser beam width of tool setter

#649

2nd measurement speed in tool

setting

#643

Tool setter laser on X

#650

Center position of tool setter on

#644

Tool setter on Y

#651

Center position of tool setter

on Y

#645

Height difference

1 (laser height-

#652

Absolute safety height of tool

base height)

setter

#646

Height difference

2 (base height-

#653

Max. allowable value for tool

workpiece height)

break detection

#647

Rapid traverse speed in tool setting

#654

Tool number of datum tool

#648

1st measurement speed in tool

#660

Datum tool length—relative

setting

tool setter surface

#661~#676

1~16 号刀，刀长相对对刀仪

表面 No.1 to 16 tools,

Note

The workpiece measurement function in the CNC system occupies the above-mentioned

user-defined macro variables. If the debugger uses other user-defined macro variables when

debugging the workpiece measurement function, instead of the user-defined macro variables

listed in the above table, the debugger will replace or add them to the table, and inform and

provide it to the user. Please do not use the above user-defined macro variables.

19.1.2 Operation Command

Function and Purpose



Arithmetic operators, functions and other operations can be flexibly used in macro programs,

which is very convenient to realize complex programming requirements. As shown in the table

346

below.

Operation

Meaning

type

command

#i = #i + #j

Addition, #i plus #j

Arithmetic

#i = #i - #j

Subtraction, #i minus #j

operation

#i = #i * #j

Multiplication, #1 times #j

#i = #i / #j

Division, #i divided by #j

#i EQ #j

（=）Equal to

#i NE #j

（≠）Not equal to

Conditional

#i GT #j

（>）Larger than

operation

#i GE #j

（≥）Larger than or equal to

#i LT #j

（<）Smaller than

#i LE #j

（≤）Smaller than or equal to

#i = #i & #j

Logic and

Logic

#i = #i | #j

Logic or

operation

#i = ~#i

Logic not

#i= SIN[#i]

Sine (unit: radians)

#i=ASIN[#i]

Arc sine

#i=COS[#i]

Cosine (unit: radians)

#i=ACOS[#i]

Arc cosine

#i=TAN[#i]

Tangent (unit: radians)

#i=ATAN[#i]

Arc tangent

#i=ABS[#i]

Absolute value

#i=INT[#i]

Round (round down)

#i=SIGN[#i]

Sign

#i=SQRT[#i]

Square root

Function

#i=#A POW[#i]

#A to the #i power

#i=LOG[#i]

Log

#i=PTM[#i]

Pulse revolutions mm

#i=PTD[#i]

Pulse revolution degree

#i=RECIP[#i]

Reciprocal

Exponent, an exponent

based

#i=EXP[#i]

(2.718)

#i=ROUND[#i]

Rounding

#i=FIX[#i]

Round down

#i=FUP[#i]

Round up

Note

When using trigonometric functions, pay attention to check "000349 trigonometric function

selection, 0: radian, 1: angle", and adjust the calculation during programming based on the

parameters.

347

19.1.3 Macro Statement

Function and Purpose



The following blocks are macro statements:

1) Blocks containing variables and operation commands;

2) Blocks containing conditional judgment statements or cycle statements;

3) Blocks containing macro program calling commands.

Description



Expression

Any calculation formulas including signs such as "+", "-", "*", "/", "[", "]", SIN, etc. are referred

to as expressions. Shown as follows

-#4

SIN[#4+#5]*COS[[#4+#5]/#6]

Note

The priority in [] is higher than +-*/, for example [[#4+#5]/#6], first calculate [#4+#5], then

calculate

/#6. For expressions, in order to ensure the correctness of calculations, it is

recommended to use [] for expressions, such as [-#5]. The usage such as -[#5] is not recommended.

Assignment statement

Transferring the value of a constant or an expression to a macro variable is referred to as an

assignment, and this statement is referred to as an assignment statement, as follows:

#5 = 145 / SQRT[3] * COS[40*PI/180]

#6 = 123

Conditional judgement statement

Two kinds of conditional judgement statements are supported:

IF [Conditional expression];

Type 1

……

ENDIF

IF [Conditional expression];

Type 2

……

ELSE

……

ENDIF

349

For the conditional expressions in the IF statement, user can use simple conditional expressions

or compound conditional expressions, as shown in the following example:

When #4 is equal to #5, assign 1 to #6

IF [#4 EQ #5]

#6 = 1

ENDIF

When #4 is equal to #5, and #6 is equal to #7, assign 2 to #6

IF [#4 EQ #5] AND [#6 EQ #7]

#6 = 2

ENDIF

When #4 is equal to #5, or #6 is equal to #7, assign 1 to #6, otherwise assign 2 to #6

IF [#4 EQ #5] OR [#6 EQ #7]

#6 =1

ELSE

#6 = 2

ENDIF

Cycle statement

The conditional expression is specified after WHILE. When the specified conditional expression

is satisfied, execute the program from WHILE to ENDW, and execute the cycle until the

conditional expression is not satisfied. When the specified conditional expression is not met, exit

the WHILE cycle and execute the program blocks after ENDW.

The calling format is as follows,

WHILE [Conditional expression]

……

ENDW

Infinite cycle

When the conditional expression in WHILE is always true, an infinite cycle can be realized. For

example,

WHILE [TRUE];or WHILE [1]

……

ENDW

Jump statement

GOTO _

Use GOTO to jump to the specified label

350

GOTO is followed by a number. For example, with GOTO 5, the system jumps to the N5 block

(N5 must be written at the beginning of the block).

Nesting

For IF statements or WHILE statements, the system allows nested statements, but with certain

restrictions, as follows:

IF statement supports up to 6 levels of nested calls, and the system will issue an error if 6 levels

are exceeded;

The WHILE statement supports up to 6 levels of nested calls, and the system will issue an error

if 6 levels are exceeded;

The system supports mixed use of IF statement and WHILE statement, but the matching

relationship between IF-ENDIF and WHILE-ENDW must be met.

Example

Edit the ellipse processing program (ellipse expression: X=A×COSα; Y=B×SINα).

%0001

#0=5

； Define the tool radius R value

#1=20

； Define A value

#2=10

； Define B value

#3=0

； Define the initial value of the step angle α, unit: degree

G92 X0 Y0 Z10

M3S1000

G00 X[2*#0+#1] Y[2*#0+#2]

G01 Z0

G41 X[#1]D01F200

WHILE #3 GE [-360]

G01 X[#1*COS[#3*PI/180]] Y[#2*SIN[#3*PI/180]]

#3=#3-5

351

19.2

Macro Program Calling

Function and Purpose



The system supports the following three ways to call the macro program:

(1) Non-modal call: G65

(2) Call macro program with G code

(3) Call macro program with M command

19.2.1 Argument Specification Rules

Function and Purpose



Argument specification rules

In the user macro program, when the argument needs to be transmitted as a local variable, the

actual argument value must be specified after the address.

When the user calls the macro program, the system will copy the content of the arguments (A to

Z) in the current block to the corresponding local variables #0 - #25 of the current layer of the

corresponding user macro program, and also copy the absolute position of the nine axes

(XYZABCUVW) of the workpiece coordinate system in the current channel to the local variables

#30 - #38 in the current channel.

Macro

Argument

Macro

Argument

Macro

Argument

variable

name

variable

name

variable

name

#10

#11

#12

#13

#14

#15

#16

#17

#18

#19

空

#20

#21

#22

#23

#24

#25

#26

Reserved

#27

Reserved

#28

Reserved

#29

Reserved

X axis

Y axis

Z axis

#30

#31

#32

position

A axis

B axis

C axis

#33

#34

#35

position

U axis

V axis

W axis

#36

#37

#38

position

353

Example

Macro variable is defined and determined

Format: AR[#Variable number]

Return value: 0: Indicates that the variable is not defined;

90: Indicates that the variable is defined as absolute mode G90;

91: Indicates that the variable is defined as incremental mode G91

Note: The system macro AR[] is used to determine whether the macro variable is defined and

defined as incremental or absolute mode;

Example

%1234

G92X0Y0Z0

M98P9990X20Y30Z40

M30

%9990

IF [AR[#23] EQ 0] OR [AR[#24] EQ 0] OR [AR[#25] EQ 0]； If the X, Y or Z value is not

defined, it returns.

M99

ENDIF

IF AR[#23] EQ 90

；If X value is in absolute mode G90

#23=#23-#30

；X value is converted to be in incremental mode, #30 is the absolute

coordinate of X

ENDIF

……

M99

19.2.2 Non-modal Call (G65)

Function and Purpose



When G65 is specified, the user macro program specified by the parameter P is called, and at the

same time, the arguments and the variables needed by the user macro program are transferred to

the user macro program.

Command Format

G65 P_ L_ [Argument address word]；

Parameter

Meaning

Program number required to be called

Number of repeated calls

354

Argument address

Data that the user needs to transfer to the

word

macro program

Note

（1）G65 is a non-modal command. User needs to specify G65 in this line every time the macro

program is called;

Example

%0032

G54G0X0Y0Z100

M3S1000

G65P100L5X50Y50Z-30R5F200

G00X50Z10

M30

%100

G01X[#23]Y[#25]F[#5]

G81Z[#25]R[#17]F[#5]

G0Z50

M30

19.2.3 Calling Macro Program with G Code

Function and Purpose



In addition to calling macro program with non-modal code (G65), user can also call the macro

program in the form of G code. Currently, the macro program in the form of G code canned cycle

can only be called for canned cycle. For the specific code, please refer to the drilling and milling

chapter and this chapter 17.2.3.

Function

Call the user-defined subprogram in user canned cycle with G command.

Command Format

G_：

Parameter

Meaning

The number of the called subroutine in USERDEF.CYC

(Arabic numerals)

Note:

1) The system provides G1000 to G1999 to call the user-defined subprogram in the canned cycle

355

with G command.

2）G1000 to G1999 respectively correspond to the called subprogram number (in Arabic

numerals) %1000 to %1999 in USERDEF.CYC, for example, G1010 corresponds to the called

subprogram number %1010 in USERDEF.CYC.

Example

Add user canned cycle %1010 in USERDEF.CYC

%1010;

G01 X30 Y0 F3000

#0 = 0.0

#1 = 30.0

#2 = 2.1

#3 = 3.4

WHILE [#0 LE 360]

G1 X[ #1 * COS[#0*PI/180]]Y[ #1 * SIN[#0*PI/180]]F3000

#0 = #0 + 0.1

ENDW

G01X30Y0F3000

G80

M99

%1244 Main program

G92X0Y0Z50

G01X30Y-20F3000

M3S3000

Z0F1000

G1010 (Call user-defined canned cycle)

G01Y20F3000

G00Z50

M30

19.2.4 Calling Macro Program with M Command

Function and Purpose



Calling macro program with M command is realized by calling a custom subprogram with an M

code.

There are two forms as described in the "Command Format" below. For the macro program calling

with M98, when M98 is executed, first call the subprogram number of the internal subprogram.

If there is no such subprogram number, search for the number of the external subprogram. If there

is no such subprogram in both, an error will be reported; for calling macro program with M code,

356

can the user-defined subprogram in the canned cycle can be called.

The corresponding M code parameter settings of user-defined subprogram in canned cycle are

shown in the following figure. The user-defined parameters 010360 to 010373 respectively

correspond to the %1007 to %1020 subprogram in USERDEF.CYC.

Command Format

M98 P_；

Parameter

Meaning

The program number to be called in the program

Note: when M98 is specified, the user macro program following P parameter is called.

M_；

Parameter

Meaning

The input value of user-defined parameter

Example

The parameter 010360 M Code Corresponding to User Canned Cycle G1007 is set as 13, that is,

the %1007 program in USERDEF.CYC can be called by the M13 command in the processing

program.

%1007; Add user-defined subprogram 1007 in the USERDEF.CYC file

G59

G64G01 X30 Y0 F3000

#0 = 0.0

#1 = 30.0

WHILE [#0 LE 360]

G1 X[ #1 * COS[#0*PI/180]]Y[ #1 * SIN[#0*PI/180]]F3000

#0 = #0 + 0.1

ENDW

G01X30Y0F3000

G80

M99

%1234; Main program

G54

G1X0Y0Z50

G01X30Y-20F3000

M3S3000

Z0F1000

M13; Call the matching 1007 subprogram with M13

357

G01Y20F3000

G00Z50

M30

Parameter type

Paramet

Parameter name

Value

Activation

010360

M code corresponding to

Save

user canned cycle G1007

010361

M code corresponding to

Save

user canned cycle G1008

010362

M code corresponding to

Save

user canned cycle G1009

010363

M code corresponding to

Save

user canned cycle G1010

010364

M code corresponding to

Save

user canned cycle G1011

010365

M code corresponding to

Save

user canned cycle G1012

010366

M code corresponding to

Save

Machine user

user canned cycle G1013

parameter

010367

M code corresponding to

Save

user canned cycle G1014

010368

M code corresponding to

Save

user canned cycle G1015

010369

M code corresponding to

Save

user canned cycle G1016

010370

M code corresponding to

Save

user canned cycle G1017

010371

M code corresponding to

Save

user canned cycle G1018

010372

M code corresponding to

Save

user canned cycle G1019

010373

M code corresponding to

Save

user canned cycle G1020

Note

(1) The above canned cycle, rotation/mirroring/scaling and G91 cannot be used at the same time.

(2) When using the M command to call a subprogram, it is necessary to add G80 before M99 at

the end of the program.

358

19.2.5 Classification of Subprogram

Function and Purpose



Internal subprogram

The called program which is in the same file with the main program is referred to as internal

subprogram.

External subprogram

The called program is stored separately in another file, which is referred to as external subprogram.

The file name of the external subprogram must start with the letter O.

Example

Example for internal subprogram

The G code file name is OTEST, and %111 is an internal subprogram, which is in the same file

as the main program %1001 and is called by M98 in the main program.

%1001; Main program

G92 X0 Y0 Z50

G91 G01 Z10 F400

M98 P111; Call subprogram 111

G4X1

M30

%111; Subprogram

G01X10Y10Z10

…

G80

M99

Example for external subprogram

The G code file name is OTEST, and the subprogram file name is O123.

Main program

Subprogram 0123

%1001

%1234;

G92 X0 Y0 Z50

G01X10Y10Z10

G91 G01 Z10 F400

…

M98 P123; Call subprogram 0123

G80

G4X1

M99

M30

359

HNC8 Series CNC Controller. Programming Manual (V2.4) - page 9