amada AMNC-F Programming Manual

CNC LASER MACHINE

(AMNC-F)

PROGRAMMING MANUAL

LASER-AMNC-F PRO-E01-200406

PREFACE This manual describes the programming procedures for the laser machine. To increase the cutting efficiency of the laser machine, read the manual carefully before creating programs.

(For operating the laser machine, refer to the separate Operator’s Manual.)

Programming Manual:

CNC Laser Machine (AMNC-F) © 2004 by AMADA CO., LTD.

No part of this publication may be photocopied or otherwise reproduced without the prior written permission of AMADA CO., LTD.

ii	Printed in Japan

CONTENTS

Part I	GENERAL MACHINE COMMANDS
	G-Code listing ............................................................................			I-4
	M-Code listing............................................................................			I-6
	Machine layout...........................................................................			I-7
	Coordinates and dimensions .....................................................			I-7
	G20		Select INCH coordinates..........................................	I-7
	G21		Select METRIC coordinates.....................................	I-8
	G90		Absolute programming .............................................	I-8
	G91		Incremental programming ........................................	I-8
	G92		Establishing coordinate system................................	I-8
	G93		Origin point offset .....................................................	I-9
	G120 Measurement probe (for LC-θ)...............................			I-9
	Motion instructions....................................................................			I-10
	G00		Rapid traverse .........................................................	I-10
	G01		Straight line motion..................................................	I-11
	G02		Circular arc CW .......................................................	I-12
	G03		Circular arc CCW ....................................................	I-14
	G09		Exact stop................................................................	I-16
	G61		Exact stop check mode ...........................................	I-16
	G64		Contour cutting mode..............................................	I-16
	G160 Space arc interpolation (for LC-θ) .........................			I-17
	General .....................................................................................			I-18
	O	Program numbers........................................................		I-18
	F	Feedrate code..............................................................		I-18
	D	Offset code ..................................................................		I-18
	N	Sequence numbers .....................................................		I-18
	;	End of block ..................................................................		I-18
	/	Block skip ......................................................................		I-19
	(Comments) .......................................................................			I-19
	G04		Dwell........................................................................	I-19
	G25, G27 Programmed repositioning (for LC-α) ............			I-20
	G31		Assist gas selection.................................................	I-20
	G50		Home return ............................................................	I-21
	G77		Measurement probe coordinate rotation (for LC-θ).....	I-21
	Laser beam compensation .......................................................			I-22
	G40		Laser beam compensation-cancel ..........................	I-22

(Continued on next page.)

iii

G41	Laser beam compensation-left................................		I-22
G42	Laser beam compensation-right .............................		I-23
Laser control .............................................................................			I-24
G24	Piercing mode .........................................................		I-24
M100	Laser mode ON.....................................................		I-24
M101	Laser mode OFF...................................................		I-24
M102	Material designation..............................................		I-25
M103	Start cutting mode.................................................		I-25
M104	Cutting mode cancel .............................................		I-25
M722, M723, M727 Tracking sensor calibration.............			I-25
M758	Beam ON ..............................................................		I-26
E1...E10 Cut condition select..........................................			I-26
E101...	E103	Pierce condition select ...............................	I-26
E201...	E205	Edge condition select.................................	I-26
Cutting parameter database..............................................			I-28
U, V, W macro functions ...........................................................			I-29
Macro number usage.........................................................			I-29
Macro memory (U, V) ........................................................			I-29
Macro recall (W) ................................................................			I-30
Nested macros ..................................................................			I-31
Multiple part processing............................................................			I-33
G98	Multiple part setup...................................................		I-33
To cancel G98....................................................................			I-34
G75, G76 Multiple macro recall ......................................			I-35
Multiple part example ........................................................			I-37
Multiple part processing on subcarriage side
of FO machine ...................................................................			I-39
General M-codes ......................................................................			I-42
M00	Program stop ..........................................................		I-42
M02	Program end ...........................................................		I-42
M30 Program end, return to start of program .................			I-42
M80, M81 Work chute open/close (for LC-α)..................			I-42
M96	Call subprogram......................................................		I-43
M97	End of subprogram .................................................		I-43
M99 End of subprogram (for FO)....................................			I-43
M150, M151, M152 Queue code (for FO).......................			I-44
M180 Cycle work chute (for LC-α)..................................			I-44
Special ......................................................................................			I-45
G32, G33 Z-axis tracking sensor ....................................			I-45
G65 Subprogram call (for FO) ........................................			I-45
G95 Call program with parameters.................................			I-45

iv

	G96	Modal program call..................................................		I-46
	G97 Modal program call cancel ......................................			I-46
	G107	Pipe Interpolation ..................................................		I-46
	G121, G122 HS-Edge detection .....................................			I-46
	G130	Axes retract ...........................................................		I-47
	G140, G141, G149		OVS .................................................	I-47
	G150	Scaling/Coordinate rotation...................................		I-48
	G161, G162 Space corner radius insertion (for LC-θ) ....			I-49
	G163 3D coordinate conversion (for LC-θ) .....................			I-49
	G164 3D coordinate conversion cancel (for LC-θ)..........			I-49
	G165 3D conversion (for LC-θ) .......................................			I-49
	G166 3D conversion cancel (for LC-θ)............................			I-49
	G173 U-axis length compensation (for LC-θ) ................			I-49
	M720, M721 Sensor ON/OFF (for LC-θ).........................			I-50
	Loader control ...........................................................................			I-51
	G10 Pallet unload (for LC-β) ...........................................			I-51
	M10, M11 Workpiece clamp/release (for LC-α) ..............			I-51
	M20 – M29 Detectable material thickenss (for LC-α) .....			I-51
	M33 Pallet load (for LC-β, FO)
		/Workpiece load (for LC-α) .....................................		I-51
	M34 Pallet unload (for LC-β)...........................................			I-51
	M55 Cancel mirror image (for LC-β) ...............................			I-52
	M65 Stock function (for LC-α).........................................			I-52
	M707, M772 – M774		Pallet change ................................	I-52
	M790, M791 Pallet set (for LC-β, FO).............................			I-52
	M792, M793 Pallet set pin (for LC-β, FO) .......................			I-52
Part II	HOLES AND PATTERNS
	G-codes for holes and patterns .................................................			II-2
	Standard holes....................................................................			II-2
	Standard patterns ...............................................................			II-2
	G-codes for standard holes .......................................................			II-3
	G111	Square/Rectangle
	(with Square/Radius/Chamfered corners) ..........................			II-4
	G112	Round/Obround ......................................................		II-6
	G113	Single D/Double D ..................................................		II-8
	G114	Polygon
	(with Square/Radius/Chamfered corners) .........................			II-10
	G115 Arc slot (Radius ends) ...........................................			II-12

(Continued on next page.)

v

G116 Arc slot (Flat ends) ................................................		II-14
G-codes for standard patterns..................................................		II-16
General format of pattern call............................................		II-16
G126	Bolt hole circle.......................................................	II-17
G128	Line at angle..........................................................	II-18
G129	Arc.........................................................................	II-19
G136	Grid- X...................................................................	II-20
G137	Grid- Y...................................................................	II-21

vi

Part I

General Machine

Commands

..................................................................................G-Code listing			I-4
M-Code listing ..................................................................................			I-6
Machine layout.................................................................................			I-7
Coordinates and dimensions ...........................................................			I-7
G20		Select INCH coordinates ................................................	I-7
G21		Select METRIC coordinates...........................................	I-8
G90		Absolute programming ...................................................	I-8
G91		Incremental programming ..............................................	I-8
G92		Establishing coordinate system......................................	I-8
G93		Origin point offset ...........................................................	I-9
G120 Measurement probe (for LC-θ).....................................			I-9
Motion instructions ..........................................................................			I-10
G00		Rapid traverse ...............................................................	I-10
G01		Straight line motion........................................................	I-11
G02		Circular arc CW .............................................................	I-12
G03		Circular arc CCW ..........................................................	I-14
G09		Exact stop......................................................................	I-16
G61		Exact stop check mode .................................................	I-16
G64		Contour cutting mode ....................................................	I-16
G160 Space arc interpolation (for LC-θ) ...............................			I-17
General	...........................................................................................		I-18
O	Program numbers..............................................................		I-18
F	Feedrate code....................................................................		I-18
D	Offset code ........................................................................		I-18

(Continued on next page.)

I-1

N	Sequence numbers ...........................................................			I-18
;	End of block ........................................................................			I-18
/	Block skip............................................................................			I-19
(Comments) .............................................................................				I-19
G04		Dwell..............................................................................		I-19
G25, G27 Programmed repositioning (for LC-α) ..................				I-20
G31		Assist gas selection.......................................................		I-20
G50		Home return ..................................................................		I-21
G77		Measurement probe coordinate rotation (for LC-θ)...........		I-21
Laser beam compensation .............................................................				I-22
G40		Laser beam compensation-cancel ................................		I-22
G41		Laser beam compensation-left......................................		I-22
G42		Laser beam compensation-right....................................		I-23
Laser control ...................................................................................				I-24
G24		Piercing mode ...............................................................		I-24
M100		Laser mode ON...........................................................		I-24
M101		Laser mode OFF.........................................................		I-24
M102		Material designation....................................................		I-25
M103		Start cutting mode.......................................................		I-25
M104		Cutting mode cancel ...................................................		I-25
M722, M723, M727 Tracking sensor calibration ...................				I-25
M758		Beam ON ....................................................................		I-26
E1	...E10 Cut condition select................................................			I-26
E101...		E103	Pierce condition select .....................................	I-26
E201...		E205	Edge condition select.......................................	I-26
Cutting parameter database ....................................................				I-28
U, V, W macro functions .................................................................				I-29
Macro number usage...............................................................				I-29
Macro memory (U, V) ..............................................................				I-29
Macro recall (W) ......................................................................				I-30
Nested macros.........................................................................				I-31
Multiple part processing..................................................................				I-33
G98		Multiple part setup.........................................................		I-33
To cancel G98..........................................................................				I-34
G75, G76 Multiple macro recall ............................................				I-35
Multiple part example ..............................................................				I-37
Multiple part processing on subcarriage side
of FO machine .........................................................................				I-39
General M-codes ............................................................................				I-42
M00		Program stop ................................................................		I-42
M02		Program end .................................................................		I-42

I-2

M30	Program end, return to start of program .......................		I-42
M80, M81 Work chute open/close (for LC-α)........................			I-42
M96	Call subprogram............................................................		I-43
M97	End of subprogram........................................................		I-43
M99	End of subprogram (for FO)..........................................		I-43
M150, M151, M152		Queue code (for FO).............................	I-44
M180 Cycle work chute (for LC-α) ........................................			I-44
Special ............................................................................................			I-45
G32, G33 Z-axis tracking sensor ..........................................			I-45
G65 Subprogram call (for FO)...............................................			I-45
G95 Call program with parameters .......................................			I-45
G96	Modal program call........................................................		I-46
G97 Modal program call cancel ............................................			I-46
G107 Pipe Interpolation ........................................................			I-46
G121, G122 HS-Edge detection ...........................................			I-46
G130 Axes retract .................................................................			I-47
G140, G141, G149		OVS .......................................................	I-47
G150 Scaling/Coordinate rotation.........................................			I-48
G161, G162 Space corner radius insertion (for LC-θ) ..........			I-49
G163 3D coordinate conversion (for LC-θ) ...........................			I-49
G164 3D coordinate conversion cancel (for LC-θ)................			I-49
G165 3D conversion (for LC-θ) .............................................			I-49
G166 3D conversion cancel (for LC-θ)..................................			I-49
G173 U-axis length compensation (for LC-θ) .......................			I-49
M720, M721 Sensor ON/OFF (for LC-θ)...............................			I-50
Loader control .................................................................................			I-51
G10 Pallet unload (for LC-β) .................................................			I-51
M10, M11 Workpiece clamp/release (for LC-α) ....................			I-51
M20 – M29 Detectable material thickenss (for LC-α) ...........			I-51
M33	Pallet load (for LC-β, FO)/Workpiece load (for LC-α) ...		I-51
M34	Pallet unload (for LC-β) .................................................		I-51
M55	Cancel mirror image (for LC-β) .....................................		I-52
M65	Stock function (for LC-α)...............................................		I-52
M707, M772 – M774		Pallet change ......................................	I-52
M790, M791 Pallet set (for LC-β, FO)...................................			I-52
M792, M793 Pallet set pin (for LC-β, FO) .............................			I-52

I-3

G-CODE LISTING

The machine is controlled by various G-codes and M-codes. A listing of G-codes follows. For information about M-codes, see page I-6.

CODE PURPOSE GROUP G00 Rapid traverse Motion G01 Straight line motion Motion G02 Circular arc CW Motion G03 Circular arc CCW Motion G04 Dwell General G09 Exact stop Motion G10 Pallet unload Loader

G20, G21 Select Inch/Metric coordinates Coordinates, dimensions G24 Piercing Laser

G25, G27 (for LC-α) Programmed repositioning General G31 Assist gas select General G32 Z-axis tracking sensor ON Special G33 Z-axis tracking sensor cancel Special

G40 Laser beam path compensation cancel Laser beam compensation

G41 Laser beam path compensation

to LEFT of path Laser beam compensation

G42 Laser beam path compensation

to RIGHT of path Laser beam compensation

G50 Home return General

G53 Setting in machine coordinate system Coordinates, dimensions G61 Exact stop check mode Motion

G64 Contour cutting mode Motion

G65 (for FO) Subprogram call Special G75, G76 Multiple macro recall Multiple G77 (for LC-θ) Measurement probe coordinate rotation General

G90 Absolute programming Coordinates, dimensions

G91 Incremental programming Coordinates, dimensions

G92 Establishing coordinate system Coordinates, dimensions

G93 Origin point offset Coordinates, dimensions

G95 Call Program with parameters Special

G96 Modal program call Special

G97 Modal program call cancel Special

G98 Multiple part setup Multiple G107 Pipe interpolation (for rotary table option) Special G111 Square/Rectangle Hole G112 Round/Obround Hole

I-4

G113 Single D/Double D Hole

G114 Polygon Hole

G115 Arc slot (radius ends) Hole

G116 Arc slot (flat ends) Hole

G120 (for LC-θ) Measurement probe Coordinates, dimensions G121, G122 HS-edge detection Special

G126 Bold hole circle (BHC) Pattern

G128 Line at angle (LAA) Pattern

G129 Arc (ARC) Pattern

G130 Axes retract Special G136 Grid-X (GRD-X) Pattern G137 Grid-Y (GRD-Y) Pattern G140 OVS hole detection Special G141 OVS expand function Special G149 OVS cancel Special G150 Scaling/Rotation Special G160 (for LC-θ) Space arc interpolation Motion G161 Space corner radius insertion Special G162 Space corner radius cancel Special G163 3D coordinate conversion Special G164 3D coordinate conversion cancel Special G165 3D conversion Special G166 3D conversion cancel Special G173 U-axis length compensation Special

I-5

M-CODE LISTING

M-CODE PURPOSE GROUP

M00 Program stop General M-code

M02 Program end General M-code M10, M11 (for LC-α) Workpiece clamp/release Special

M20 – M29 (for LC-α) Detectable material thickness Special

M30 Program end, return to start of program General M-code M33 (for LC-β/LC-α) Pallet load/ Workpiece load Loader

M34 (for LC-β) Pallet unload Loader M55 (for LC-β) Cancel mirror image Loader M65 (for LC-α) Stock function Loader

M80, M81 (for LC-α) Work chute open/close General M-code M96 Call subprogram General M-code M97 End of subprogram General M-code M99 (for FO) End of subprogram General M-code M100 Laser mode ON Laser

M101 Laser mode OFF Laser

M102 Material designation Laser

M103 Pierce material, start cutting mode Laser

M104 Cancel cutting mode Laser

M150, M151, M152 (for FO) Queue code General M-code M180 (for LC-α) Cycle work chute General M-code M707, M772 – M774 Pallet change Loader

M720, M721 Sensor ON/OFF Laser M722, M723, M727 Tracking sensor calibration Laser M758 Beam ON Laser M790, M791 (for LC-β) Pallet set Loader M792, M793 (for LC-β) Pallet set pin Loader

I-6

MACHINE LAYOUT

The LC-α machine and the LC-β machine are ahybrid system, with moving the material in the X-axis and moving the laser head in the Y- axis. The LC-α machine moves the material across a ball-transfer table, while the LC-β machine moves the pallet and material in the X- axis. The LC-θ or FO machine moves the laser head in the X-axis and Y-axis.

With the axes at the reference positions, the laser head is at the X+ and Y+ corner of the working area for the LC-α, -β, and -θ machines and is at the X+ and Y– corner of the working area for the FO machine.

COORDINATES AND DIMENSIONS

The NC used on these machines accepts information within certain ranges of values. The following table lists allowable values for various uses.

Numeric formats/allowable range of values
Items	Metric	Inch
X, Y, Z	+/– 99999.9999	+/– 9999.9999
G	1 to 9999	1 to 9999
N	0 to 99999	1 to 99999
O	0 to 9999	0 to 9999
R, I, J	+/– 99999.9999	+/– 9999.9999
M	1 to 999	0 to 999
X (as parameter)	.001 to 9999.999	.001 to 9999.999
P	1 to 9999	1 to 9999

G20 Select INCH coordinates

May be used in MDI, or at the beginning of a program on a line by itself. After changing coordinate system, G92 must be re-set. This may be done by re-referencing the machine (using RETRACT mode) or by using the G92 or G130 instruction.

NOTE

OIn a program, must be followed by either a G92 statement for INCH coordinates, or a G130 instruction.

I-7

G21 Select METRIC coordinates

May be used in MDI, or at the beginning of a program on a line by itself. After changing coordinate system, G92 must be re-set. This may be done by re-referencing the machine (using RETRACT mode) or by using the G92 or G130 instruction.

NOTE

OIn a program, must be followed by either a G92 statement for METRIC coordinates, or a G130 instruction.

G90 Absolute programming

When G90 is commanded, all coordinates in the program refer to current program origin or to the absolute origin point.

G90 is MODAL and remains effective until G91 is commanded.

G91 Incremental programming

When G91 is commanded, all coordinates in the program are incremental distances from the previous coordinate.

G91 is MODAL and remains effective until G90 is commanded.

G92 Establishing coordinate system

The G92 command is optional, unless the system has been switched between INCH and METRIC. Once the machine has been powered up and referenced, the standard coordinate system is ready to use.

The G92 instruction may be used to establish an absolute origin point for programming.

The usual (default) absolute origin point for the X and Y axes corresponds to the corner of the sheet of material closest to the junction of the work clamps and the X-gauge block.

NOTE

OThe G92 command must be immediately followed by the appropriate X, Y, and Z values, all on the same block of information.

When the machine has been referenced and is at “home” reference position, the NC’s position display (FUNC+POS keys) displays values which may be used in the G92 statement for the active units system (Inch/MM).

The following charts list dimensions for some common machines. If your machine does not appear here or the numbers do not seem to “match up”, confirm with AMADA the correct values for your machine and write them in below.

I-8

Machine Type	X axis mm {in}		Y axis mm {in}		Z axis mm {in}
LC-1212 α	1270	{50.000}	1270	{50.000}	300	{11.8110}
LC-2415 α	2520	{99.2126}	1550	{61.0236}	300	{11.8110}
LC-2412 β	2520	{99.2126}	1270	{50.000}	300	{11.8110}
LC-3015 β	3070	{120.8661}	1550	{61.0236}	300	{11.8110}
LC-3015 θ	3050	{120.0787}	1530	{60.2362}	700	{27.5590}
FO2412	2520	{99.2126}	1270	{50.000}	200	{7.8740}
FO3015	3070	{120.8661}	1550	{61.0236}	200	{7.8740}

G93 Origin point offset

The G93 command establishes a reference origin point, relative to the absolute origin point, anywhere within the limits set by G92. This is done for ease of programming.

G93 X__ Y__ Z__;
X…X-offset
Y…Y-offset
Z…Z-offset	(normally zero)

Example

G93 X0.2 Y12.0 Z0;

Shifts the part-program reference point 0.2 inches in the plus-X direction and 12.0 inches in the plus-Y direction from the absolute origin point or current reference established by a G98 multiple part instruction (see page I-33).

To cancel the origin point offset: G93 X0 Y0 Z0;

NOTE

OThe G93 command must be immediately followed by the appropriate X, Y, and Z values, all on the same block of information.

OWhen programming multiple parts using G98, the G93 refers to each part origin as set by G98.

OIf G91 (incremental coordinates) is effective when G93 is commanded, it becomes an incremental offset from the previous G93. Otherwise it replaces the previous G93.

OWhen using the cutting database, the system automatically corrects for material thickness. Unless cutting formed materials or not using the cutting database, use Z0.

G120 Measurement probe (for LC-θ)

Compensates the machine coordinate system and program origin point by using the optional measurement probe. For details, refer to the Operator’s Manual.

I-9

MOTION INSTRUCTIONS

Motion instructions belong to two groups: rapid traverse, and contouring rapid traverse (G00) is strictly for positioning the material to a particular location. Contouring instructions (G01, G02, and G03) are used to move the material through a particular path under the laser head at a particular speed (feedrate).

The system defaults to absolute coordinates programming.

G00 Rapid traverse

This command is for positioning. It moves the table and laser head to the designated X, Y axis location at the current traverse speed. (default is maximum speed)

G00 X__Y__;

The Z-axis may also be positioned, but not on the same block as with X,

Y axes.

Only axes included in the command are actually moved.

NOTE

OThe laser beam is OFF when G00 is active.

OEach axis moves independently, so the material path is usually not a straight line.

OG00 forces an in-position check at the commanded end point. This may be used to force a sharp corner during processing. (Use G00 on separate line.)

OMaximum rapid traverse speed is 40 m/min (1575 ipm). The RATE buttons on the CNC control panel can reduce travel speed to 50% or 25% of this.

OG00 is MODAL: Once commanded, it stays in effect until a G01, G02, or G03 is commanded.

OAbsolute/incremental programming is available by G90/G91.

I-10

G01 Straight line motion

Moves the material from current position to commanded location via a straight line. Feedrate, assist gas selection, laser power, pulse rate, etc. are determined by the active material and table selection (M102, En) and by active operator overrides.

G01 X__ Y__;

X…X-coordinate (mm or in.)

Y…Y-axis coordinate (mm or in.)

NOTE

OG01 is MODAL: once commanded, it remains effective until a G00, G02, or G03 is commanded.

OThe machine is capable of moving all three axes at the same time, in this mode. Absolute/Incremental programming is available by G90/G91.

OA feedrate must be specified for G01, G02, G03. This is normally done by M102 and Enn, but may also be done using an Fnnnn feedrate command.

ODuring machine operation, feedrate may be overridden from 0% to 255% in 1% steps from the operator panel.

OThe feedrate of the optional subcarriage of the FO machine is set by an NC parameter.

Example
G90 G00	X11.0 Y20.0;
G91 G01	X7.0 Y4.0;

I-11

G02 Circular arc CW

Moves the material from current position to commanded location via a clockwise arc at a commanded radius and feedrate.

G02 X__ Y__ R__ (or I__ J__);

X… X-coordinate (mm or in.) Y… Y-axis coordinate (mm or in.)

R… Radius of arc (negative value creates an arc > 180°) (can use either R or I, J in instruction)

I… Distance in the X-direction from the staring point to the arc center.

J… Distance in the Y-direction from the staring point to the arc center.

Example of R format

G90 G02 X.5 Y25.0 R2.5; Example of I, J format

G90 G02 X.5 Y25.0 I.5 J2.449;

NOTE

OG02 is MODAL: once commanded, it remains effective until a G00, G01, or G03 is commanded.

OThe parameter “R” has priority over “I” and/or “J”, when used on the same line.

OThe radius R (or that computed from I, J) must be non-zero.

OAbsolute/incremental programming available by G90/G91 only affects the end point. The I, J values are always incremental from arc starting point.

OIf the angle of the arc is greater than 180 degrees, the R value must be negative.

OThe machine is capable of moving only two axes at the same time, in this mode.

OTo cut a full circle, I and J must be used, rather than R.

OA feedrate must be specified for G01, G02, G03. This is normally done by M102 and En, but may also be done using an Fnnnn feedrate command.

ODuring machine operation, feedrate may be overridden from 0% to 255% in 1% steps from the operator panel.

I-12

I-13

G03 Circular arc CCW

Moves the material from current position to commanded location via a counter-clockwise arc.

This command is used to cut material in a counter-clockwise arc at a commanded feedrate and radius. The X and Y values specified determine the endpoint of the cut. The R value specified determines the radius of the cut.

G03 X__ Y__ R__ (or I__ J__);

X… X-coordinate (mm or in.) Y… Y-axis coordinate (mm or in.)

R… Radius of arc (negative value creates an arc > 180°) (can use either R or I, J in instruction)

I… Distance in the X-direction from the starting point to the arc center.

J… Distance in the Y-direction from the starting point to the arc center.

NOTE

OG03 is MODAL: once commanded, it remains effective until a G00, G01, or G02 is commanded.

OThe parameter “R” has priority over “I” and/or “J”, when used on the same line.

OThe radius R (or that computed from I, J) must be non-zero.

OAbsolute/incremental programming available by G90/G91 only affects the end point. The I, j values are always incremental from arc starting point.

OIf the angle of the arc is greater than 180 degrees, the R value must be negative.

OThe machine is capable of moving only two axes at the same time, in this mode.

OTo cut a full circle, I and J must be used, rather than R.

OA feedrate must be specified for G01, G02, G03. This is normally done by M102 and En, but may also be done using an Fnnnn feedrate command.

ODuring machine operation, feedrate may be overridden from 0% to 255% in 1% steps from the operator panel.

I-14

I-15

G09 Exact stop

A command effective for a specified block only. Axis travel is decelerated at the ending point of the block and checked for in-position. The next block is then executed.

G09 (G01 X__ Y__);

The command in parentheses may be G02 or G03.

NOTE

OThe in-position check refers to the check made to see if the axis travel has reached the specified position (within the range set by a parameter).

G61 Exact stop check mode

This command requires the machine to stop and wait for verification of each programmed position before moving toward the next programmed position.

NOTE

OG61 must be canceled before cutting any blended radii or using any of the standard hole commands (G111 to 115) either singly or in patterns.

OOnce G61 is commanded, it will stay in effect until a G64 is commanded.

G64 Contour cutting mode

This is the default cutting mode for the machine. No position verification is required prior to movement towards the next programmed position. This mode is in effect until changed by a G61 command.

I-16

G160 Space arc interpolation (for LC-θ)

G160 Xx1 Yy1 Zz1 Va1 Ub1; Xx2 Yy2 Zz2 Va2 Ub2;

The first block indicates the center point of the arc, and the second block indicates the ending point of the arc.

G160 is MODAL and remains effective until G00, G01, G02 or G03 is commanded.

When the center point and ending point are commanded, the arc to the ending point is obtained.

When the commands for the V- and U-axes are omitted, the nozzle moves in that attitude. When the ending point is not commanded and another code (e.g., G01) is commanded, the conditions for the arc are not met. In this case, the nozzle moves with the path from the starting point to the center point straightly interpolated.

When the center point is omitted, the attitude of the nozzle is automatically controlled according to the radius of the arc from the starting point to the ending point. When another space arc interpolation is commanded, the ending point becomes the starting point of the next arc.

I-17

GENERAL

O Program numbers

Each program must be assigned a program number. This number is used to separate the 200 different programs that can be stored in memory at one time. The program number must begin with the letter “O”.

NOTE

OAny number from 0 to 8999 can be used.

OProgram 0 (zero) should be left vacant, as it can easily be overwritten during certain extended edit procedures.

OPrograms numbered 8000 to 8999 can be protected by setting a parameter.

F Feedrate code

Cutting feedrates are normally specified by using M102 to select material type and thickness, and using E1-E9 to fine-tune or select for type of contour or detail. The F-code may be used to override a standard feedrate, or for material for which an entry does not exist in the database.

NOTE

OIn Inch mode, the feedrate is in inches per minute.

OIn Metric mode, the feedrate is in millimeters per minute.

OAn F code is required only when the M102 functions are not used.

D Offset code

These codes are not used on the LC-α, β machine. Instead, laser beam offset amounts are kept in the cutting parameter database. See the section on laser beam compensation, beginning page I-22, and the section on standard holes, in Part II.

N Sequence numbers

Instruction blocks in a program may be marked or labeled using sequence numbers. When used, a sequence number must be the first address in the program block. The valid numeric range is from 1 to 99999. They do not need to be in numeric sequence.

;End of block

This symbol is used to separate one block of information from another.

I-18

/Block skip

If the block skip button is illuminated, any block of information with this symbol at its beginning will be ignored.

(Comments)

Comments may be placed in a program by enclosing them in parentheses.

If a comment is placed on the first line after the program number, it will be displayed in the program directory listing of the CNC (machine control). Comments should not be mixed into the middle of program lines. Place each comment at the end of a program line or on a separate line.

O1234 (SAMPLE COMMENT);

(THIS COMMENT IS ON A LINE BY ITSELF);

If programming off-line, make sure to use all capitals for comments and instructions.

G04 Dwell

The dwell function stops the machine for a specified period of time, in seconds.

G04 Xnnnn;

Where .001<=nnnn<=9999.999

NOTE

OCAUTION: Use of G04 between contouring motion instructions (G01, G02, G03) cancels laser beam compensation.

OWhen the time period is over, machine operation continues. Use extreme caution when using the dwell function.

OThe minimum dwell value is 0.001 second. This is equivalent to G04 with no “X” value.

I-19