Roland CAMM-3 PNC-3200 Operating and maintenance manual

PNC-3200
NC code
PROGRAMMER'S MANUAL
Thank you very much for purchasing the PNC-3200.
• To ensure correct and safe usage with a full understanding of this product's
performance, please be sure to read through this manual completely and store
it in a safe location.
• Unauthorized copying or transferral, in whole or in part, of this manual is
prohibited.
• The contents of this operation manual and the specifications of this product
are subject to change without notice.
• The operation manual and the product have been prepared and tested as much
as possible. If you find any misprint or error, please inform us.
• Roland DG Corp. assumes no responsibility for any direct or indirect loss or
damage which may occur through use of this product, regardless of any failure
to perform on the part of this product.
• Roland DG Corp. assumes no responsibility for any direct or indirect loss or
damage which may occur with respect to any article made using this product.

1
Table of Contents
Introduction.................................................................................................................................................................................. 2
Part 1 Programming Basics
Programming ............................................................................................................................................................................ 3
Coordinate Systems ................................................................................................................................................................ 7
Setting Coordinate Values (Amount of Movement) .......................................................................................................... 10
Setting the Measurement Unit.............................................................................................................................................. 11
Real-number Entry and Integer Entry ................................................................................................................................. 11
Program Number.................................................................................................................................................................... 12
Sequence Numbers ............................................................................................................................................................... 12
Optional Block Skip................................................................................................................................................................ 12
Positioning (G00).................................................................................................................................................................... 13
Linear Interpolation (G01)..................................................................................................................................................... 13
Circular Interpolation (G02 and G03).................................................................................................................................. 13
Cutter Compensation (G40, G41 and G42) ....................................................................................................................... 15
Feed Rate................................................................................................................................................................................ 15
Spindle Motor Control (M03 and M05)................................................................................................................................ 16
Spindle Motor Speed ............................................................................................................................................................. 16
Fixed Cycle.............................................................................................................................................................................. 16
Program-related Errors.......................................................................................................................................................... 16
Sample Program .................................................................................................................................................................... 18
Part 2 Reference
How to Read Part 2 ........................................................................................................................................................... 19
Preparatory Functions (G Functions)
G 00 Positioning ................................................................................................................................ 20
G 01 Linear Interpolation................................................................................................................... 21
G 02 and G 03 Circular Interpolation ................................................................................................................ 22
G 04 Dwell ......................................................................................................................................... 25
G10 Data Setting............................................................................................................................... 26
G 17, G 18 and G 19 Plane.......................................................................................................................................... 28
G20 and G21 Setting the Measurement Unit ................................................................................................... 28
G39 Corner-offset Circular Interpolation .........................................................................................29
G40, G41 and G42 Cutter Compensation ................................................................................................................. 30
G 50 and G 51 Scaling....................................................................................................................................... 38
G 54, G55, G56,
G57, G58 and G 59 Selects Coordinate System........................................................................................................ 39
G 80, G 81, G 82,
G 85, G86 and G 89 Fixed Cycle (Canned Cycle) ..................................................................................................... 40
G 90 and G 91 Absolute and Incremental ......................................................................................................... 44
G 92 Coordinate System .................................................................................................................... 45
G 98 Initial Level Return ................................................................................................................... 46
G 99 Point R Level Return ................................................................................................................ 46
Copyright © 1999, 2000 ROLAND DG CORPORATION

2
Introduction
What Is in This Manual
This manual explains those codes interpreted by numerical control machine tools (NC codes) which are supported by
PNC-3200. Codes and functions which are not supported are not described.
This Manual Has Two Parts.
“Part 1 — Programming Basics” describes such basic but necessary programming-related matters as programming,
coordinate systems, and how to set coordinate values (amount of movement).
“Part 2 — Reference” explains each of the codes in an encyclopedic form. Once a certain familiarity with programming
has been achieved, programming can be accomplished simply by glancing through this part.
Miscellaneous Functions (M Functions)
M 00 Program Stop ............................................................................................................................. 47
M 01 Optional Stop ............................................................................................................................ 47
M 02 End of Program .......................................................................................................................... 47
M 03 and M 05 Spindle Motor Start/Stop ........................................................................................................... 47
M 06 Tool Change .............................................................................................................................. 48
M 30 End of Program ......................................................................................................................... 48
M 98 Subprogram Call ........................................................................................................................ 49
M 99 End of Subprogram .................................................................................................................... 50
Spindle Speed Function (S Function) ......................................................................................................................... 51
Feed Function (F Function) ............................................................................................................................................ 53
Other Functions
N Sequence Number ..................................................................................................................... 54
O Program Number....................................................................................................................... 54
/ Optional Block Skip.................................................................................................................. 55
% or ER Program Start ............................................................................................................................ 55
EOB End of Block .............................................................................................................................. 56
( ) Comment ................................................................................................................................... 56
Appendices
Words Table......................................................................................................................................................... 57
Character Code Table (ISO, EIA, and ASCII).......................................................................................................... 59

3
Part 1 1Programming Basics
N
N 01
N 02
N 03
N 04
N 05
N 06
N 07
N 08
N 09
N 10
•
G
G 90
G 00
G 01
G 02
X
X ••••
X ••••
X ••••
X ••••
Y
Y ••••
Y ••••
Y ••••
Y ••••
Z
Z ••••
Z ••••
S
S 5000
F
F 300
F 150
M
M 03
%
Once the appropriate conditions and cutting sequence for the job have been determined, then before cutting is begun, the programming
steps are written down on a piece of paper like the one shown below. (This form is called a “process sheet.”) This sheet is handy for
confirming the cutting sequence and numerical values.
Programming
The Process of Programming
First, examine the drawing and determine such conditions as the workpiece material, the size of the workpiece to be prepared, the tool
diameter, the tool type, the proper turning speed, and the proper feed rate. Then determine the sequence in which to cut. The cutting
sequence is in extremely important point for carrying out cutting efficiently and safely.
In actual cutting, the moving portion may be either the workpiece or the spindle. Programming is carried out with consideration given
to how the tool moves, with no distinction made for the actual movement.
Drawing
Workpiece material
Size of workpiece to be prepared
Tool diameter
Tool type
Turning speed
Feed rate
Cutting sequence
Etc.
Determine conditions and
cutting sequence
G00X Y
G01X Y
G02X Y
Process sheet
Program
12
3
46
Cutting
5

4
N254M98P0003
N100M98P0002
N101G00X10.
M99
N255G00Y5.
M99
M99
N176M98P0004
N177G00Y2.
O0002
Call
O0003
Call
O0004
Call
..........
Main
program
(Program No. 1) Subprogram
(Program No. 2) Subprogram
(Program No. 3)
Subprogram
(Program No. 4)
* “%”for ISO or ASCII,
“ER ”for EIA
(* For details on blocks, see “About Blocks,”which is the following section.)
Conceptual view of a main program and subprograms
Program Structure and Format
Programming proceeds in accordance with the process sheet that has been prepared. The program is input using a dedicated input
device for NC codes, or with a general-purpose computer.
Input is made as shown in the figure below. Addresses such as G, M, X, I, and J are combined with numbers to specify the cutting steps
and tool movements.
Program Structure
A program can be classified as a “main program”or a “subprogram.”
Main Program
Ordinarily, the machine operates according to instructions from a main program. A subprogram, which is described next, is basically
specified within a main program.
Subprogram
If a main program can be likened to the trunk of a tree, then subprograms are branches. When a main program specifies execution of a
subprogram of a certain number, the subprogram of that number is called up and executed.
Subprograms can be convenient when writing a program where the same task is to be performed a number of times. Program modular-
ity can also be promoted by creating subprograms which have good general utility.
A subprogram can call another subprogram.
Data start
Program end
Preparatory function
Coordinate values, etc.
Feed rate
Spindle speed
Miscellaneous function
Block end
(start of the next block)
Sequence No.
Word
Address Value
Words which express dimensions,
angles, and so on are called
“dimension words.”Addresses for
dimension words include X, Y, Z, I,
J, K, and R.
Program No.

5
: A block containing only a “%”must appear at the start of the data. This notifies the machine of the start (or end) of
the data. Such a block may optionally be present at the end of the data. When it appears at the end of the data, the
data is specified automatically.
The character indicating the program start is “%”in the case of ISO or ASCII code, or “ER ”in the case of EIA.
: The EOB (end of block) indicates the conclusion of the block. In ASCII, this is the LF (line feed) code.
: This inputs the program number. A program starts with a program number, and ends with either M02, M30, or M99.
M02 or M30 signifies the end of a main program, and M99 signals the end of a subprogram.
An integer from 0001 to 9999 can be input as the program number. Care should be taken to ensure that multiple
program numbers do not appear in a single program.
Program numbers are used to call up subprograms.
: Sequence numbers are reference numbers for the program. They have absolutely no effect on the program (machine
operation).
: This is the preparatory function. The special functions are specified by the two-digit code following the “G.”
: This indicates a coordinate value or movement distance. I, J, and K are used to specify the center coordinate of a
circle (or arc).
:For positive coordinates or movement directions, it is not necessary to prefix a “+”to the value.
: This determines the feed rate.
: This determines the speed of the spindle motor.
: This is a miscellaneous function. It is used for such operations as starting and stopping the spindle motor.
: This signals the end of the program. The spindle stops.
%
EOB
O
N
G
X(I)
Y(J)
Z(K)
F
S
M
M02
About Blocks
A program is a series of instructions (written commands) for the machine, expressed as symbols and numbers. The instructions are
separated by EOB markers, with the information between two EOB markers making up one instruction. This single instruction
between two EOB markers is called a “block.”Each block, in turn, is composed of “words.”
The types of words include those valid only within a block, those also valid outside of blocks until a word of the same group is speci-
fied, those which activate a function immediately after being specified, those which activate a function at the end of the block in which
they are specified, and those which activate a function at the start of the block in which they are specified. Programming requires
knowledge of the characteristics of each word. See "APPENDICES-Words Table" or a chart of word characteristics.
<Examples of “words also valid outside of blocks until a word of the same group is specified”>
Indicates that the specified coordinate value is absolute (G90)
Linear interpolation from the current tool position to X = 100, Y = 100 (G01)
Linear interpolation from the tool position moved to by N02 to Z = -20
Movement (positioning) from the tool position moved to by N03 to Z = 20 (G00)
Movement (positioning) from the tool position moved to by N03 to X = 0, Y = 0.
%
N01 G90
N02 G01X100Y100
N03 Z-20
N04 G00Z20
N05 X0Y0

6
Data Output from the Computer
Before outputting data, make the appropriate cable connections to link the computer and the machine. Refer to the user's manuals for
each model for explanations on making connections and connection specifications.
The character code systems supported by the machine are ASCII, ISO, and EIA. ASCII is an abbreviation for the “American Standard
Code for Information Interchange.”ASCII is the most widely used code standard established for computers to handle text, and is used
by virtually all computers. Text is output as normal ASCII unless you use software which can output ISO or EIA codes to the machine,
or a program which converts ASCII to ISO or EIA.
Numerically controlled machine tools (NC machines) generally use ISO (International Organization for Standardization) or EIA
(Electronic Industry Association) as their character code system. Both of these use a data length of 8 bits, which means that ASCII, with
a length of 7 bits, cannot be used without modification. In an ISO code, the 8th bit is for parity checking, with bits 1 through 7 the same
as the corresponding ASCII code. (Refer to "AppendicesCharacter Code Table (ISO, EIA, and ASCII)" .)

7
Coordinate Systems
The machine uses the Cartesian coordinate system, which has three axes —the X axis, the Y axis, and the Z axis —each of which is
perpendicular to the other two.
+Z
+X
+Y
Machine Coordinate Systems
A machine coordinate system is a coordinate system determined mechanically with reference to the PNC-3200. The origin point in a
machine coordinate system is a point specific to the PNC-3200, and cannot be moved. The origin point in a machine coordinate system
is at the forward-left corner of the machine's maximum range of operation, and is the point to which the machine moves at powerup.
Coordinate values (or amounts of movement) specified in an actual program are coordinates in a workpiece coordinate system.
Workpiece Coordinate Systems
A workpiece coordinate system is a coordinate system for workpiece machining. The origin point of a workpiece coordinate system is
the program's origin point according to an absolute specification.
There are two methods that can be used to set a workpiece coordinate system.
1. Setting using G92
2. Setting using G54 to G59
1. Setting a workpiece coordinate system using G92
A workpiece coordinate is defined by specifying the workpiece coordinate location of the current tool location.
For example, to set a point which is 20 mm (X), 15 mm (Y), 10 mm (Z) from the point to be taken as the origin of the present tool
location, the following should be set:
G92X20.0Y15.0Z10.0
Normally, the tool is moved to a point on the loaded workpiece and G92X0Y0Z0 (the workpiece coordinate origin point) is set.
Z
X
Y
Tool
20.0
10.0 15.0
ZX
Y
Executing G92X20.0Y15.0Z10.0
sets the coordinate system taking
this as the origin point.
X
Y
Z

8
Z
X
Y
Z
X
Y
Z
X
YZ
X
YZ
X
Y
Z
X
Y
Workpiece
coordinate system 1
Workpiece
coordinate system 2
Workpiece
coordinate system 3
Workpiece
coordinate system 4
Workpiece
coordinate system 6
Workpiece
coordinate system 5
Machine coordinate
origin point
Workpiece origin
point offset amount
Z
X
Y
Z
X
Y
Z
X
YZ
X
YZ
X
Y
Z
X
Y
EXOFS
Machine coordinate
origin point
External workpiece origin
point offset amount
Workpiece
coordinate system 1
Workpiece
coordinate system 2
Workpiece
coordinate system 3
Workpiece
coordinate system 4
Workpiece
coordinate system 6
Workpiece
coordinate system 5
2. Setting a workpiece coordinate system using G54 to G59
This method is used to set up to six workpiece coordinate origin points and select a coordinate system from among these by means of
the program.
The workpiece coordinate systems 1 through 6 are set by specifying the amount of shift (the amount of workpiece origin point offset)
from the machine coordinate origin point to the workpiece coordinate origin point. Each workpiece coordinate system is set using the
PNC-3200's display. (Refer to the “User's Manual 3 Cutting Using NC-Codes”for information on making this setting.)
It is also possible to shift the six set workpiece coordinates by a desired distance at one time. Because the workpiece origin point is
offset, this is called EXOFS (external workpiece origin point offset amount). EXOFS is set with G10 or by using the PNC-3200's
display. (Refer to the “User's Manual 3 Cutting Using NC-Codes”for information on how to make the setting on the PNC-3200.)

9
Z
X
Y
Machine coordinate origin point
Z
X
Y
Workpiece
coordinate system 1
Workpiece
coordinate system 1
Workpiece origin
point offset amount
Amount of offset
by G10
Z
X
Y
Z
X
Y
Z
X
YZ
X
YZ
X
Y
Z
X
Y
Workpiece
coordinate system 1
Workpiece
coordinate system 2
Workpiece
coordinate system 3
Workpiece
coordinate system 4
Workpiece
coordinate system 6
Workpiece
coordinate system 5
Machine coordinate
origin point
Workpiece origin
point offset amount
Amount of offset
by G92
Y
X
Tool
Y
X
Tool
15.0
10.0 G92X5.0Y5.0
executed at
this position
Y
X
5.0
5.0
Amount of
offset by G92
G10 can be used to set not only the amount of shift for all workpiece coordinate systems, but also amounts of offset for each individual
workpiece coordinate system.
Selecting any of the workpiece coordinate systems from G54 to G59 and executing G92 causes the following to occur.
Because G92 sets the current tool position to a desired coordinate value, the workpiece coordinate system selected at that time comes to
have a new origin point. The distance between the origin coordinate points before and after G92 is specified (that is, the amount of shift
of the coordinate system) is added to each workpiece origin point offset amount. This causes the workpiece coordinate systems from
G54 to G59 to be shifted by the same distance.

10
Y
X
510 15 20
(mm)
0
5
10
15
y=7000
(Increase in Y)
x=15000
(Increase in X)
(4000, 5000)
(19000, 12000)
Y
X
510 15 20
(mm)
0
5
10
15
(19000, 12000)
(4000, 5000)
G90
G00X4000Y5000
G01X19000Y12000
G90
G00X4000Y5000
G91
G01X15000Y7000
Absolute Incremental
Setting Coordinate Values (Amount of Movement)
The addresses “X, Y, and Z”or “I, J, and K”are used, followed by the coordinate specification.
X, Y, and Z: These specify coordinate values for positioning (G00), linear interpolation (G01), and the like. X, Y, and Z represent the
coordinates for the X, Y, and Z axes, respectively. It is not necessary to specify all three. As an example, if you want to
leave the Y and Z axes as they are, and shift only the X axis by 10 mm, “G00X10.0”should be input.
I, J, and K: These specify the center point for circular interpolation (G02 and G03). I, J, and K represent the movement for the X, Y,
and Z axes from the current tool position, respectively. Another method of circular interpolation involves specifying the
radius. Refer to "G02 and G03 Circlar Interpolation" for details.
Absolute and Incremental
There are two types of coordinate specifications: absolute and incremental. These are toggled by G90 and G91.
The figure below shows the difference between absolute and incremental specifications on an X-Y plane. Absolute specifications
indicate the position as the distance from the workpiece coordinate origin, whereas incremental specifications indicate the amount of
movement from the current position.
Programming that specifies absolute coordinates is called “absolute programming,”and programming which specifies incremental
coordinates is termed “incremental programming.”
The settings for G90 or G91 made on the PNC-3200 remain in effect unless changed by programming.
There are no special rules for deciding when to use an absolute or incremental program. Examine the drawing and choose the one which
makes for the simplest program.

11
Amount of
movement (length)
Feed rate
Time
X10.0
X1000
F60.0
F120000
G04X10.0
G04X1000
10 mm or 10 in.*
1 mm or 0.1 in.*
60 mm/min. or 60 inch/min.*
120 mm/min. or 12 inch/min.*
10 sec. dwell
10 sec. dwell
Setting the Measurement Unit
G20 and G21 can be used to set the measurement unit used for movement, feed rate, and offset amounts.
G20: Inch input
G21: Millimeter input
Either G20 or G21 is set at the start of the program, before setting the coordinate system. G20 and G21 should not be changed during
the course of a program. If the unit is not set by programming, the setting made on the PNC-3200 is used.
The minimum units differ for inch input and millimeter input.
Real-number Entry and Integer Entry
Movement amount (length), feed rate, and time may be input using either real-number entry or integer entry.
Input of a number which contains a decimal point (for example “10.0”or “10.”) is called real-number entry, and input of a number
without a decimal point is called integer entry. A value such as “10.0”where the portion to the right of the decimal point is zero may be
abbreviated to “10.”with no change in value.
When real-number entry is used, the numerical value is interpreted as being in the measurement unit that has been set. When integer
entry is used, the numerical value is interpreted as being the minimum unit of the measurement unit that has been set. Some examples
of this are as follows.
* The measurement unit is set by G20 (inch input) or G21 (millimeter input).
* If the unit is not set by programming, the setting made on the PNC-3200 is used.
There are two types of methods for setting the speed of the spindle motor: setting as an rpm value, and setting as a numerical code. See
"Spindle Speed Function (S Function) for details.
Inch input
Millimeter input
Minimum units
0.0001 in.
0.001 mm
Movement
Feed rate
Offset amounts
Command
G00X10.0
G00X10000
F60.0
F45000
G10P01R10.0
G10P01R10000
G20
10 in.
1 in.
60 inch/min.
4.5 inch/min.
10 in.
1 in.
G21
10 mm
10 mm
60 mm/min.
45 mm/min.
10 mm
10 mm

12
A main program or subprogram calls and executes another program by specifying a program number. The program number appears at
the start of the program.
A program number is specified by appending an integer of up to four digits after the letter “O.”The range for program numbers is from
0001 to 9999 -- “0”(zero) may not be used as a program number.
The section that extends from the place where the program number is input to an M02, M30, or M99 is recognized as one program (or
subprogram). M02 or M30 is used to indicate the end of a main program, and M99 is used to signal the end of a subprogram.
Program Number
A sequence number is an integer number for a block. It is specified at the start of the block.
A sequence number may either be present or absent from any or all blocks. There is also no need for sequence numbers to be consecu-
tive, or to be arranged in order from smaller to larger numbers. However, consecutive sequence numbers are customarily used to mark
critical places within a program.
A sequence number is specified by appending an integer of up to four digits after the letter “N.”The range for program numbers is from
0001 to 9999. A sequence number cannot be substituted for a program number.
Sequence Numbers
This function makes it possible to skip over a desired block within a program. Optional block skip is specified at the start of the
program.
Enter a "/" (slash) at the start of the block.
The setting for enabling or disabling block skip is made on the PNC-3200. (Refer to "User's Manual 3 -- Cutting Using NC Codes.")
Optional Block Skip

13
This cuts a circular shape from the current position to the specified point. The words for circular interpolation are “G02”and “G03.”
Any address of the set X, Y, and Z is used to specify the destination coordinates, and any address of the set I, J, and K is used to specify
the center of the circle. I, J, and K always specify the movement distance (incremental value) to the centerpoint of the circle or arc, with
no regard for G90 or G91.
G02 and G03 do not include the function for starting the spindle motor. This means that if the spindle motor is not already turning, the
M03 word must be given beforehand to start it.
G02 and G03 interpolate in different directions —clockwise for G02 and counterclockwise for G03.
Circular interpolation can be carried out on any of the two-dimensional planes —the X-Y plane, the Z-X plane, or the Y-Z plane. The
desired plane is specified with G17 (X-Y plane), G18 (Z-X plane), or G19 (Y-Z plane). See "G17, G18 and G19 Plane" for the
details of plane specification.
This moves in a straight line at maximum speed from the current tool position to the specified point. The word for positioning is
“G00.” The addresses X, Y, and Z are used to specify the destination point. When X, Y, and Z are all specified, the three axes move
simultaneously.
If the tool path is blocked by the workpiece or another object during movement, it is necessary to take steps to prevent the tool from
striking the object, and one way to do this is to move each axis one at a time. An example of this would be to use the absolute specifica-
tion “G00Z5000” to raise the tool, followed by “G00X1000Y1000” for horizontal movement.
Positioning (G00)
Linear Interpolation (G01)
Circular Interpolation (G02 and G03)
This cuts in a straight line from the current position to the specified point. The word for linear interpolation is “G01.”The addresses X,
Y, and Z are used to specify the destination point. When X, Y, and Z are all specified, the three axes move simultaneously.
G01 does not include the function for starting the spindle motor. This means that if the spindle motor is not already turning, the M03
word must be given beforehand to start it.
In actual cutting, compensation for the tool diameter is required. Refer " G40, G41 and G42 Cutter Compensation" for more informa-
tion on compensation of the tool diameter.
Y
X
(15000, 2000)
Current position
(6000, 9000)
G00X15000Y2000
Y
X
(15000, 2000)
Current position
(6000, 9000)
G00X15000
* When the coordinates are absolute * When the coordinates are absolute
G00Y2000

14
+Z
+Y
+X
Clockwise Counterclockwise
Z
Y
X
G03
G02
G03
G02
G02
G03
Clockwise
rotation Counter
clockwise
rotation
G02 G03
Y
X
(12000, 5000)
(7000, 17000)
(0, 0)
G17G02X7000Y17000I12000J5000
G17G03X7000Y17000I12000J5000
Even when the point for the destination and the center of the circle are identical, circular interpolation is carried out as shown below
according to the direction of interpolation.
There is another method, which involves specifying the radius of the circle instead of specifying the circle’s center point. This method is
convenient because numerical values read from the drawing can be used directly.
Two circles with identical radii and passing through two points exist. This means that if the interpolation direction, radius of the circle,
and point for the destination of interpolation have been specified, there are two circles. These two circles can be differentiated by
specifying a positive value for the radius if the center angle is 180 degrees or less, and a negative radius if the center angle exceeds 180
degrees. Y
X
A(0, 0)
B(17000, -7000)
R13000
R13000
G17G02X17000Y-7000R-13000
G17G02X17000Y-7000R13000

15
Cutter Compensation (G40, G41 and G42)
The movement of the tool specified by the program is the path taken by the center of the tool. Because the tool has a certain thickness
(i.e., a certain diameter), it will over-cut by an amount equal to its radius if the coordinates on the drawing are input just as they are.
To cut a shape as specified by the drawing, the tool must be made to move at a place which shifted away by a distance equal to the tool
radius. This is called the “tool-diameter offset.”
Using this function makes it possible to input the values from the drawing as coordinate values (or amounts of movement) with no need
for modification, thus facilitating programming. Also, if cutting is to be performed with a tool that has a different tool diameter, it is
only necessary to change the amount of offset.
The words for cutter compensation are “G40,”“G41,”and “G42.”
G40: Cancel cutter compensation
G41: Cutter compensation -- left
G42: Cutter compensation -- right
Feed Rate
This determines the feed rate for the workpiece and the spindle. The F function is used to make the setting.
The feed rate generally varies according to the cutting parameters (such as the spindle speed, tool diameter, and workpiece material).
The F function is activated at the start of the block in which it is specified.
The feed rate is specified as a real or integer value following the “F.”
F100.0 Feed rate set at 100 mm/min. (when millimeter input is used)
F100000 Feed rate set at 100 mm/min. (when millimeter input is used)
Feed Rate Override
Feed rate override”refers to manually changing the feed rate specified by the program. This is mainly used to adjust the feed rate
during cutting. This function may or may not be supported, depending on the machine. Refer to the "User's Manual 3 Cutting Using
NC-Codes" for information on how to make this setting.
45 15
25
15
15
25
15 45
R15
R15
R
R15+R
R15
R15
R15-R
Workpiece
Tool
: Tool path

16
Spindle Motor Speed
Fixed Cycle
Program-related Errors
The Sfunction is used to set the speed for the spindle motor.
The Sfunction does not include the function for starting the spindle motor. It functions only when the spindle has been started with
M03, or when the spindle is already turning.
This function is activated at the end of the block in which it is specified.
The fixed cycle (or canned cycle) is a command for executing a series of pre-established operations for cutting, such as drilling.
This command can execute several blocks of cutting operations in a single block, thereby simplifying programming. This also reduces
the amount of data.
See "Fixed Cycle (Canned Cycle) G80, G81, G82, G85, G86 and G89" for details of the specifications for the fixed cycle.
An error is generated when an unsuitable value has been set for a parameter, or when the PNC-3200 cannot interpret the program. Only
error messages related to programming are described in this manual.
Errors Occurring During Program Execution
When an error occurs, operation pauses and an error message is displayed. When this happens, press the [DISPLAY] key to display the
block which contains the error.
The cutting operation can be continued as-is after an error has been displayed, but this is not recommended because operation following
the occurrence of an error may not be correct. Instead, stop program execution and correct the place where the error was generated.
Spindle Motor Control (M03 and M05)
These turn the spindle motor on or off. The M function is used for this.
M03 and M05 are used to control the spindle motor. M03 starts rotation of the spindle, and M05 stops it.
These functions are activated at the end of the block in which they are specified together.

17
Error message Description
Bad Parameter
Address Undefined
Parameter Undefined
Code Cannot Execute
Display Operations When an Error Occurs During Program Execution
The value of a parameter exceeds the allowable range, or the value of the radius for circular
interpolation or the amount of offset is not correct.
Only a parameter has been set. The code which specifies the parameter has not been set.
A parameter has not been set.
This is displayed when an attempt was made to execute an unrecognizable command, when
cutter compensation was started while in the circular interpolation mode, or when an attempt
was made to execute a command which cannot be used during tool-diameter compensation.
Program Number
Not found
Sub-Program
Nest Over
The program number specified by M98 or M99 could not be found.
An attempt was made to call a fifth-level subprogram from a fourth-level subprogram of a main
program.
Error While Registering Cutting Data
A check of subprograms is carried out when a program is saved in the buffer. Depending on the results of the check, one of the follow-
ing error messages may be displayed.
Error message Description
Sub-Program
Table Over
Duplicate
Sub-Program Number
There are more than ten subprograms. The maximum number of subprograms that can be
specified in one set of data is ten.
Stop sending data, and press the [CANCEL] key.
Correct the program and resend the data.
The program contains multiple subprograms with the same program number. The same
program number may not be set for more than one subprogram within a single set of data.
Stop sending data, and press the [CANCEL] key.
Correct the program and resend the data.
All commands in the block
containing the error are
ignored, and operation is
resumed with the next block
Program execution
is stopped
Error display
Display of the block containing the error
Pause display
O0001 O0001
G17G41H03G00X10.Y5.
Bad Parameter FEED HOLD
Hit CANCEL to Break

18
%
O0001
N01 G91
N02 G21
N03 G92X0Y0Z0
N04 G10P01R3.0
N05 G00Z5.0
N07 F300.0S6000M03
N06 G17G41D01G00X8.0Y8.0
N08 G01Z-7.0
N09 G01Y35.0
N10 X45.0
N11 G03X15.0Y-15.0I15.0
N12 G01Y-20.0
N13 X-60.0
N14 Z7.0
N15 G40G00X-8.0Y-8.0
N16 M05
M02
%
Data start
Program number
Incremental programming
Set millimeter input
Set workpiece coordinate origin point
Set 3 mm of offset for offset number 1
Move tool to position of 5 mm on Z axis (X0Y0 unchanged)
Set motor speed to 6,000 rpm and feed rate to 300 mm/min., and rotate spindle
Start cutter compensation and move tool to X-axis 8 mm and Y-axis 8 mm
Linear interpolation to -7 mm on Z axis
Linear interpolation to 35 mm on Y axis
Linear interpolation to 45 mm on X axis
Circular interpolation (counterclockwise) to position X 15 mm Y -15 mm from current tool position
Linear interpolation to -20 mm on Y axis
Linear interpolation to -60 mm on X axis
Linear interpolation to 7 mm on Z axis
Cancel cutter compensation and return to start point
Main spindle rotation halt
Program end
Data end
* The example program shown above is for when using ISO orASCII as the code.
45 15
35
15
20
60
R15
R
R15
Tool
: Tool path
Workpiece
Tool position
at start
8 mm
8 mm
R: 3 mm tool radius
X
Y
Sample Program