9. part program

CAD/CAM
Department of Mechatronics Engineering
CHUNGNAM NATIONAL UNIVERSITY
©2008-2015 Young-Woo Park
NC Part ProgrammingNC Part Programming
Professor Young-Woo Park, Ph.D.
Lecture 9

CAD/CAM
 Definition
 the procedure by which the sequence of processing steps to
be performed on a CNC machine tool is planned & documented.
 Ways
 manual programming
 tailoring to a particular controller
 trigonometric computations are required.
 computer-aided programming
 programming using English-like commands
 not tailoring to a particular controller
 CAD/CAM
IntroductionIntroduction

CAD/CAM
 Definition
 a program format for arranging information so to be suitable for
input to a CNC controller
 Comparison
English language CNC programming language
English characters Program characters
English word Program word
English sentence Program block
Period End of block
Word Address ProgrammingWord Address Programming

CAD/CAM
 Program Language Terminology
 program character
 an alphanumeric character or punctuation mark
 ex: N, G, ;
 address
 a letter that describes the meaning of the numerical value
following the address
 ex: G 00
address number
X -3.75

CAD/CAM
 words
 are composed of two parts: an address followed by a number.
 are used to describe such important information as machine motions &
dimensions in programs.
 ex: N0020 G90
 block
 a complete line of information to a CNC machine tool
 is composed of one word or an arrangement of words.
 ex: N0020 G90 ;
 program
 a sequence of blocks to manufacture a part
 the MCU executes a program block by block.

CAD/CAM
 Syntax
 O: program number
 programs are stored in the MCU memory by program number.
 O0001 to O9999
 N: sequence number
 an optional tag that can be coded at the beginning of a block if needed
 N0001 to N9999
 ex: O0519 program number
N0010 G91G80G49G40G00T01
N0020 T02M01
… sequence number

CAD/CAM
 G: preparatory function
 G code is a command in the program specifying the mode
in which a CNC machine moves along programming axes.
 the # following the G address indicates the mode of movement.
 two categories of G codes
Category Effect
modal the G code specification will remain effective for all subsequent blocks
unless replaced by another modal G code.
nonmodal the G code specification will only affect the block in which it appears.

CAD/CAM
 Examples
G code Mode Specification
G00 modal Rapid positioning mode. The tool is to be moved to its
programmed XYZ location at maximum feedrate.
G01 modal Linear interpolation mode. The tool is to be moved along
a straight-line path at the progammed feedrate.
G21 modal Specifies metric (mm) mode for all units.
G28 nonmodal Return tool to reference point.
G43 modal Specifies tool length offset (positive direction).
G49 modal Cancels the tool length offset.
G98 modal Specifies a return to the initial point in a machining cycle
that had been created by a modal G code.

CAD/CAM
 M: Miscellaneous machine functions
 Specify CNC machine functions not related to axes or
dimensional movements.
 Direct the controller to immediately execute the machine function
indicated.
 two groups of M codes
Category Effect
A those executed with the start of axis movements in a block.
B
those executed after the completion of axis movements in a block.

CAD/CAM
 Examples
M code Type Specification
M00 B Cause a program stop.
M02 B Cause a program end. An M02 code must be the last
command in a program. If used, do not use M30.
M03 (M04) A Turns spindle on clockwise (counterclockwise).
M05 B Turns spindle off. Usually used prior to a tool change &
at the end of a program.
M06 B Stops the program & calls for an automatic tool change.
M07 (M08) A Turns the coolant tap oil (the external coolant) on.
M08 A Turns the external coolant on.
M30 B Directs the system to end program processing, reset
the memory unit. This code must be the last command
in a program. If used, do not use M02.

CAD/CAM
 dimensional words
 are used to specify the movement of the programming axes.
 X, Y, Z; linear axes
 A, B, C: rotary axes
 U, V, W: axes parallel to X, Y, Z axes
 I, J, K: axes used as auxiliary of X, Y, Z axes
 R, Q: axes used as auxiliary of Z axis
 ex: N0030 G00 X.5Y.5
move tool at rapid speed/tool moves to X.5 Y.5.

CAD/CAM
 F: feedrate
 the rate at which the spindle moves along a programming axis
 F10 = 0.001 ipm; F10. = 10 ipm
 S: spindle function
 S codes control the speed at which the spindle rotates.
 a numerical value up to 4 digits maximum
 modal code
 replaced by a new S code or cancelled by a spindle off (M05)
 spindle rotation should be specified prior to entering blocks
containing cutting command.
 T: tool function

CAD/CAM
 Three planes in the Cartesian coordinate system
 XY plane
conventional standard
 YZ plane
 XZ plane
 reference points
 MRZ
a point on the actual machine
 PRZ = part reference zero
a point on the actual part
lower left-hand top corner
CNC Milling FundamentalsCNC Milling Fundamentals

CAD/CAM

CAD/CAM
 three major phases of a CNC program
 program setup
always start with the program start flag (% sign)
line two: a program number
line three: the first that is actually numbered
 increments of 1, 5 or 10
 absolute units, inch programming, etc.
 material removal: actual cutting
 system shutdown
spindle off, coolant off, end of program

CAD/CAM
 preparing to program
 develop an order of operations
 before writing your program, plan it from start to finish considering
all operations that must be performed.
do all the necessary math and complete a coordinate sheet.
choose your tooling and calculate the speeds and feeds.
 decide on which tools are going to use & ensure the tools
available that will perform the required tasks.
 calculate the required speeds and feeds.

CAD/CAM
 safety rules for G00
 If the Z value represents a negative move, the X- and Y-axes
should be executed first.
 If the Z value represents a positive move, the X- and Y-axes
should be executed last.
 If the basic rules are not followed, an accident can result.

CAD/CAM
1. The computer interprets the instructions in the program into
computer-usable form.
2. The computer performs the necessary geometry and trigonometry
calculations required to generate the part surface.
3. The part-programmer specifies the part outline as the tool path.
Since the tool path is at the periphery of the cutter that machining
actually takes place, it must be offset by the radius of the cutter.
4. The cutter offset computations in contour part-programming are
performed by the computer.
5. Part-programming languages are general-purpose languages.
Since NC machine tool systems have different features and
capabilities, the computer must take the general instructions and
make them specific to a particular machine tool system. This
function is called post processing

CAD/CAM
6. After converting all instructions into a detailed set of machine tool
motion commands, they are downloaded to the specific NC
machine.
7. Graphic proofing techniques provide a visual representation of the
cutting tool path.
8. This representation may be a simple two-dimensional plot of the
cutter path or a dynamic display of tool motion using computer
generated animation.
9. If necessary, part-programs are also verified on the NC station
using substitute materials such as light metals, plastics, foams,
wood, laminates, and other castable low cost materials used for NC
proofing.

CAD/CAM
 Syntax: G01 Zn Fn
X1 Y1
X2 Y2
…
 Example
G01 Z-0.125 F5
X3 Y2
Linear Interpolation, G01Linear Interpolation, G01

CAD/CAM

CAD/CAM
 coordinate sheet
Position X Y
②
③
④
⑤
⑥
⑦
⑧

CAD/CAM
Position X Y
② -0.35 4.25
③ 2.25 4.25
④ 2.25 1.25
⑤ 5.25 1.25
⑥ 5.25 -0.25
⑦ -0.25 -0.25
⑧ -0.25 4.25

CAD/CAM
 Direction
Circular Interpolation, G02, G03Circular Interpolation, G02, G03

CAD/CAM
 Plane Specification
Circular Interpolation, G02, G03Circular Interpolation, G02, G03

CAD/CAM
 I, J, K
the DISTANCE from the ARC START POINT
to the CENTER POINT of the arc
 G17 – Use I and J
 G18 – Use I and K
 G19 – Use J and K
Circular Interpolation : I, J, K MethodCircular Interpolation : I, J, K Method

CAD/CAM
 Syntax: G02 Xn Yn In Jn (XY plane) (G17 G90 G02)
XY plane
absolute coordinate
G03 Xn Yn In Jn (XY plane) (G17 G90 G03)

CAD/CAM
 Syntax: G02 Xn Yn In Jn (XY plane) (G17 G91 G02)
XY plane
incremental coordinate
G03 Xn Yn In Jn (XY plane) (G17 G91 G03)

CAD/CAM
 Exercise
Ref: http://www.manufacturinget.org/2011/12/cnc-g-code-g02-and-g03/

CAD/CAM
 Exercise
G01Y1.0 F8.0;
G02 X1.2803 Y1.5303 I.750;

CAD/CAM
 Syntax: G02(G03) Xn Yn Rn (XY plane)
Circular Interpolation : R MethhodCircular Interpolation : R Methhod

CAD/CAM
 Exercise

CAD/CAM
 Exercise
G01Y1.0 F8.0;
G02 X1.2803 Y1.5303 R-.750;

CAD/CAM
Linear & Circular InterpolationLinear & Circular Interpolation

CAD/CAM
 All of CNC MTs require some form(s) of compensation.
 Examples of Compensation in Daily Life
 airplane pilot
 for wind velocity & direction as a heading is set.
 race car driver
 for weather & track conditions as a turn is negotiated.
 bowler
 for spin of the bowling ball as the ball rolls down the valley.
 marksman firing a rifle
 for the distance to the target.
CompensationCompensation

CAD/CAM
 Way of Compensation
 initial compensation  fine tuning
 example: marksman
 adjust the sight on the rifle to allow for a distance.
 fine tune to adjust for minor imperfections within the initial
adjustment after the first firing.

CAD/CAM
 Offsets
 All forms of compensation work with offsets.
 Offsets are storage locations into which numerical values can
be placed in the CNC control.
 Reasons for Offsets
 To specify each tool's length
 At the time of setup, the setup person measures the length of
each tool & inputs the length value into the corresponding offset.
 To specify the radius of the cutting tool
 The cutter radius compensation allows the programmer to ignore
the cutter size as the program is written. So, the setup person
inputs the cutter size into its corresponding tool offset.

CAD/CAM
 Types of Compensation
 tool length compensation
 cutter diameter compensation
 dimensional tool (wear) offsets for turning center
 tool nose radius compensation for turning center

CAD/CAM
 Definition
 a process in which the machine controller automatically
moves the cutter so that the edge cuts the programmed
movement, rather than the center of the cutter following the
programmed movement.
 Reasons for CDC
 Program coordinates are easier to calculate
 Range of cutter sizes
 Easy sizing
 Roughing and finishing
Cutter Diameter Compensation (CDC)Cutter Diameter Compensation (CDC)

CAD/CAM
 Comparison
Cutter Diameter CompensationCutter Diameter Compensation

CAD/CAM
 Understanding
 With a little imagination, you can see all the possibilities for
tweaking your part, or getting your part made with any size endmill.

CAD/CAM
 How to turn CDC on
 to zero your part & program a move away from the part in the
X & Y direction equal to the tool radius.
 Then move back to 0,0, and then continue cutting your profile.

CAD/CAM
 How to turn CDC “ON”
 A CDC G code must be followed by an X, Y linear motion code.
 It signals the controller to initiate (ramp on) or cancel (ramp off) CDC.
 G02 & G03 blocks must be programmed after the initial linear
motion blocks.
 The 1st
X, Y linear tool movement following a CDC block must be
equal to or greater than
the radius of the cutter being
used.

CAD/CAM
 The MCU will apply compensation by offsetting the cutter in the
direction perpendicular to the next X, Y axis tool movement.
 The offset will be equal to the cutter radius
previously entered at setup.

CAD/CAM
 The 1st
move for an inside cut should be to a location away from
an inside corner.
 This will prevent the cutter from notching the part.

CAD/CAM
 How to turn CDC “OFF”
 send the tool off in the X & Y direction a distance equal to the
tool radius.
 after reaching 0,0 turn off cutter compensation and ramp off to
A.

CAD/CAM
 Syntax: G41 Xn Yn Dn
 G41
 directs the controller to offset
(ramp on) the tool to the left
side of upward tool motion.
 Dn
 specifies the address in
memory where the cutter
radius offset value is stored.
n = register number

CAD/CAM
 Syntax: G42 Xn Yn Dn
 G41
 directs the controller to offset
(ramp on) the tool to the right
side of upward tool motion.
 G40
 cancels G41 or G42.

CAD/CAM
G01 X1.0 Y-1.0
G41 X1.0 Y0.0 D1
Y1.0
X0.0
Y0.0
G01 G40 X1.0 Y-1.0

CAD/CAM
 Example

CAD/CAM
 Solution
G90 G00 X-11.0 Y6.0 S800 Rapid to position .②
G01 Z-.5 M03
G41 X-10.5 D21 Ramp on to left of upward tool
motion on next move to .③
G01 X10.0 F10.0 Cut to ④ at feedrate 10.
Y-6.0 Cut to .⑤
X-10.0 Cut to .⑥
Y6.5 Cut to .⑦
G00 G40 Y7.0 Ramp off on the next move to
.⑧

CAD/CAM
 Definition
 a canned cycle is a single line of code which, in effect,
says "Start cutting here, finish cutting there, remove the material
with cuts that are so deep and use this cutting feed rate".
 Hole operation
 Modal command
 These cycles are used when NC code is created
manually.
Canned CycleCanned Cycle

CAD/CAM
 Five operations in a canned cycle
 Positioning of the X and Y axes
 Rapid traverse to the R plane
 Drilling, boring and tapping
 Operation at the bottom of hole
 Retract to the R plane

CAD/CAM
 Codes
 G80, G81, G82, G83, G84, G98, G99
 G80: Cancel canned cycle
 G81: Drill
 F, L, P, R, X, Y & Z
 L; # of repeats
 R; Reference plane
 G82: Center Drill
 F, L, P, R, X, Y & Z
 P; Dwell operation time in seconds

CAD/CAM
 G83: Peck drill
 F, L, Q, R, X, Y & X
 Q; Peck Depth
 If the depth of hole is 1”, Q.25 will peck 4 times.
 G84: Tapping
 Same as G81 but be careful with F.
 G98: Initial point return
 G99: Reference plane return

CAD/CAM
 G83: Pack drill
 F, L, Q, R, X, Y & X
 Q; Peck Depth
 If the depth of hole is 1”, Q.25 will peck 4 times.
 G84: Tapping
 Same as G81 but be careful with F.
 G98: Initial point return
 G99: Reference plane return

CAD/CAM
 G98 and G99

9. part program

More Related Content

What's hot (20)

Viewers also liked (20)

Similar to 9. part program (20)

Recently uploaded (20)

9. part program