Transcript Chapter 6 Numerical Control Programming

Numerical Control
Programming
6.1 NC PART PROGRAMMING

Introduction
• Coordinate Systems
• NC Words
6.1.1
Coordinate System
Z AXIS Z // rotating spindle
 workpiece-rotating machine:
Z is parallel to the spindle
 tool-rotating machine:
Z is parallel to the tool axis
Z
Z
Z
6.1.1
Coordinate System
X AXIS
X // table
 workpiece-rotating machine:
X is the direction of tool movement

X
Z
horizontal milling machine :
X axis is parallel to the table

vertical machine :
+X axis points to the right
when the programmer
is facing the machine.
X
Z
X
Z
6.1.5
NC Words

N, G, X, Y Z, A, B, C, I, J, K, F, S, T, R, M

N: specify the sequence number

G: preparatory word
to prepare for control functions (the motion of each axis,
coordinate system, coordinate plane, cutter radius
compensation, tool length offset……)

M: miscellaneous word
to control miscellaneous functions (spindle on/off,
start/stop the machine, turn on/off the coolant, change the
tool, and rewind the program tape)
6.1.5
NC Words
6.1.5
NC Words
M CODES
M00
Program stop
M06
Tool change
M01
Optional stop
M07
Flood coolant on
M02
End of program
M08
Mist coolant on
M03
Spindle CW
M09
Coolant off
M04
Spindle CCW
M30
End of tape
6.1.5

NC Words
Modal codes and non modal codes/
• modal functions
Modal functions stay active until some other command
changes it. Modal commands are arranged in sets called
“modal groups”, and only one member of a modal group
may be in forces at any given time.
• non-modal functions
Non-modal functions have effect only on the lines on
which they occur.
6.1.5
NC Words
modal groups
6.1.5
NC Words
M CODES
modal groups
M00
Program stop
M06
Tool change
M01
Optional stop
M07
Flood coolant on
M02
End of program
M08
Mist coolant on
M03
Spindle CW
M09
Coolant off
M04
Spindle CCW
M30
End of tape
6.1.5
NC Words
N, G, X, Y , Z, A, B, C, I, J, K, F, S, T, R, M

F: feed rate of the tool motion
S: cutting-speed

T: tool number

6.1.5
NC Words
N, G, X, Y , Z, A, B, C, I, J, K, F, S, T, R, M

X, Y, Z, A, B, C: provide the coordinate positions of
the tool. X, Y, and Z define the three translational
(Cartesian) axes of a machine. A, B and C are used
for the three rotational axes about the X, Y, and Z
axes.

I, J, K: specify the center for circular motion
6.1.5
NC Words
N, G, X, Y, Z, A, B, C, I, J, K, F, S, T, R, M

R: specify the clearance height
in canned-cycle
N0010 G81 X1.000 Y2.000 Z0.000 R1.300
Operations in drill cycle G81 :
1. Rapid to location (1,2,2).
2. Rapid down to the R plane:(1,2,1.3)
3. Feed to the Z point, the bottom of the hole:(1,2,0)
4. Operation at the bottom of the hole .
5. Rapid or feed to either the R plane or the initial height.
NC Words
G codes



Unit selection:
•
G70 (inch), G71(metric)
Coordinates selection:
•
G90(absolute), G91(incremental)
Working plane selection:
•
G17(X-Y), G18(Z-X), G19(Y-Z)
Set up working coordinate


Z
Machine zero
•
is unchangeable and usually is set up with the machine
23
Working coordinate
(is decided by the offset from the machine zero)
• G92
• Be defined in program
G55
G56
G57
X
25.2
G92 X25.2 Z23.0
G58
G59
G54
Machine zero
Rapid traverse: G00

G00:
• to make the machine move at maximum speed.
• It is used for positioning motion.
G90 G00 X20.0 Y10.0
End
G90:
absolute
coordinate
s
Start
(20,10)
(10,10)
(0,0)
Linear interpolation: G01

G01:
• linear interpolation at feed speed.
G91 G0l X200.0 Y100.0 F200.0
G91:
incremental
coordinates
Y
End
100.0
Start
200.0
X
Circular interpolation: G02, G03

G02, G03:
• For circular interpolation, the tool destination and the circle
center are programmed in one block
• G02 is clockwise interpolation, G03 is counterclockwise
interpolation
G 02
 R
G17
 X __ Y __
G 03
 I __

 F __;
J __
G 02
 R

G18
X
__
Z
__


 F __;
G 03
 I __ K __
G 02
 R

G19
Y
__
Z
__


 F __;
G 03
 J __ K __
End point Circle center, radius
Circular interpolation: G02, G03
Y

End
Specify Center with I, J, K
•
X
Start
j
Center
i
•
I, J, K are the
incremental distance
from the start of the arc;
Viewing the start of arc
as the origin, I, J, K
have positive or
negative signs.
Circular interpolation: G02, G03
N0010 G92 X200.0 Y40.0 Z0；
N0020 G90 G03 X140.0 Y100.0 R60.0 F300；
N0030 G02 X120.0 Y60.0 R50.0；
G92:
To define working
coordinate
G90:
absolute
coordinates
Y
100
60
40
R50
R60
X
O
90 120 140
200
Circular interpolation: G02, G03
Annotation for Circular Interpolation
• I0.0, J0.0, and K0.0 can be omitted.
• If X,Y,Z are all omitted in the program, that means
start and end of arc are same points.
N0020 G02 I20.0 (a full circle)
• If I, J, K, and R all appears in circular interpolation
instruction, R is valid and I, J, and K are invalid
Return to Machine Zero: G28
G28
 The machine passes by the specified point, and then
move to the machine zero.
G91: incremental
G91 G28 X_, Y_, Z_


coordinates
X,Y,Z are the coordinate of specified point that is saved in
memory of machine.
Usually this instruction is used in the beginning and end of
program.
Machine
Zero
A
Specified
point
Return to the Specified point : G29
G29
 The machine passes from the machine zero by
the point that is specified in G28, and then move
to the new specified point.
G29 X_, Y_, Z_


X, Y, Z are the coordinate of new specified point
G28,G29 are usually used to change tool
Specified point
in G28
Machine
Zero
A
New specified point
in G29
M code


miscellaneous word
miscellaneous functions:
•
•
•
•
•
turn the spindle on/off
start/stop the machine
turn on/off the coolant
change the tool
rewind the program (tape)
M code
M00
Program stop
M06
Tool change
M01
Optional stop
M07
Flood coolant on
M02
End of program
M08
Mist coolant on
M03
Spindle CW
M09
Coolant off
M04
Spindle CCW
M30
End of tape
modal groups
M code: M00, M01


M00 and M01 both stop the machine in the
middle of a program.
M01 is effective only when the optional stop
button on the control panel is depressed. The
program can be resumed through the control
panel.
M code: M03, M04, M05



M03 turns on the spindle clockwise.
M04 turns the spindle on counterclockwise.
(The spindle rpm must be specified in the
same line or in a previous line. )
M05 turns off the spindle.
M code: M07, M08, M09

M07 and M08 turn on different modes of
coolant.
•
•

M07: flood coolant on
M08: mist coolant on
M09 turns off the coolant.
M code: M06


M06 signals the tool-change operation.
On a machine equipped with an automatic
tool changer, it stops the spindle, retracts the
spindle to the tool-change position, and then
changes the tool to the one specified in the
T-code.
M code: M02, M30


M02 marks the end of the program.
M30 marks the end of the tape. It stops the
spindle and rewinds the program (tape)
Example

A 2.0-in 2.0-in. square is to be milled using a 1/2-in. end
milling cutter (end mill). Write an NC part program to
make the square.
Example
Part program
Explanation
N0010 G41 S1000 F5 M03
Begin compensation（left）, set feed and
speed, spindle on （CW）
Move to lower left corner
Plunge down the tool
Cut to upper left corner
Cut to upper right corner with external curve
Cut to lower right corner with external curve
Cut to lower left corner with external curve
Lift the tool
End the composition, stop the machine
N0020 G00 X6.000 Y6.000
N0030 G01 Z-1.000
N0040 G01 Y8.000
N0050 G01 X8.000 M96
N0060 G01 Y6.000 M96
N0070 G01 X6.000 M96
N0080 G01 Z1.000
N0090 G40 M30
G codes with animations
http://www.cncezpro.com/gcodes.cfm
Manual Part Programming Example
5”
2.5”
p3
p2
p4
p5
1”
5”
45°
Tool size = 0.25 inch,
Feed rate = 6 inch per minute,
Cutting speed = 300 rpm,
Tool start position: 2.0, 2.0
Programming in inches
(4, 4)
p1
p0 (2, 2)
Motion of tool:
p0  p1  p2  p3  p4  p5  p1  p0
1. Set up the programming parameters
5”
2.5”
p3
p2
p4
p5
1”
Programming in inches
5”
Use absolute coordinates
Feed in ipm
45°
N010 G70 G90 G94 G97 M04
(4, 4)
p1
p0 (2, 2)
Spindle speed in rpm
Spindle CCW
2. Set up the machining conditions
5”
2.5”
p3
p2
p4
p5
1”
Machine moves in XY-plane
Use full-circle interpolation
5”
Feed rate
Spindle speed
45°
N020 G17 G75 F6.0 S300 T1001 M08
(4, 4)
p1
p0 (2, 2)
Tool no.
Flood coolant ON
3. Move tool from p0 to p1 in straight line
5”
2.5”
p3
p2
1”
p4
p5
Linear interpolation
target coordinates
N030 G01 X3.875 Y3.698
5”
45°
(4, 4)
p1
p0 (2, 2)
4. Cut profile from p1 to p2
5”
2.5”
p3
p2
p4
p5
1”
Linear interpolation
5”
target coordinates
N040 G01 X3.875 Y9.125
45°
or
(4, 4)
p1
N040 G01 Y9.125
p0 (2, 2)
X-coordinate does not change  no need to program it
5. Cut profile from p2 to p3
5”
2.5”
p3
p2
p4
p5
Linear interpolation
target coordinates
1”
N050 G01 X5.634 Y9.125
5”
y = 9 + 0.125 = 9.125
(6.5 - x)2 + 0.1252 = (1 - 0.125)2
x = 5.634
45°
p3
(x, y)
(4, 4)
p1
(6.5, 9)
.125
p0 (2, 2)
1”
6. Cut along circle from p3 to p4
5”
2.5”
p3
p2
p4
p5
1”
circular interpolation, CCW motion
5”
target coordinates
45°
(4, 4)
N060 G03 X7.366 Y9.125 I6.5 J9.0
coordinates of center of circle
p1
p0 (2, 2)
N060 G03 X7.366 Y9.125 I0.866 J-0.125
7. Cut from p4 to p5
5”
2.5”
p3
p2
p4
p5
1”
5”
Linear interpolation
45°
(4, 4)
p1
p0 (2, 2)
target coordinates (Y is unchanged)
N070 G01 X9.302
8. Cut from p5 to p1
5”
2.5”
p3
p2
p4
p5
1”
5”
Linear interpolation
target coordinates (see step 3)
45°
N080 G01 X3.875 Y3.698
(4, 4)
p1
p0 (2, 2)
9. Return to home position, stop program
5”
2.5”
p3
p2
p4
p5
1”
Linear interpolation
target coordinates (see step 3)
5”
N090 G01 X2.0 Y2.0 M30
45°
(4, 4)
p1
p0 (2, 2)
end of data
N100 M00
program stop
10. Complete RS-274 program
N010 G70 G90 G94 G97 M04
N020 G17 G75 F6.0 S300 T1001 M08
N030 G01 X3.875 Y3.698
N040 G01 X3.875 Y9.125
N050 G01 X5.634 Y9.125
N060 G03 X7.366 Y9.125 I0.866 J-0.125
N070 G01 X9.302
N080 G01 X3.875 Y3.698
N090 G01 X2.0 Y2.0 M30
Automatic Part Programming
Software programs can automatic generation of CNC data
Define Tool
CNC data
Make 3D model
Simulate
cutting
Automatic part programming and DNC
Very complex part shapes  very large NC program
NC controller memory may not handle HUGE part program
computer feeds few blocks of
NC program to controller
When almost all blocks executed,
controller requests more blocks
Assignment



(Learn this software)
CNC Simulator
Download from
http://cncsimulator.com/download/get.php?f=C
ncSetup453.exe
Direct Numerical Control (DNC):

A system in which a central computer
downloads the NC programs block by
block to many NC machine tools
simultaneously is called Direct Numerical
Control (DNC) system.
2004
49
DNC
 Direct numerical control (DNC) – control of multiple
machine tools by a single (mainframe) computer
through direct connection and in real time
 1960s technology
 Two way communication
 Distributed numerical control (DNC) – network
consisting of central computer connected to machine
tool MCUs, which are CNC
 Present technology
 Two way communication
Direct Numerical Control (DNC):

This system used to work with the early NC
machine tools which can not read more
than a block of information at a time. The
central computer feed the program
information one block at a time. When the
machine execute the information, the next
block of information would be fed.
2004
51
Distributed Numerical Control (DNC):

Distributed NC is known by the same
acronym as Direct Numerical Control
(DNC). After the introduction of CNC, the
machine tools have had the capability of
storing large amount of information.
Therefore, there have been no need to have
drip feed information system, like, Direct
Numerical Control. Instead, Distributed
Numerical Control is introduced. In such a
system, a host computer communicate with
many CNC machine tools via networks and
download or upload programs.
2004
52
Distributed Numerical Control (DNC):


With Distributed Numerical Control
systems, it is possible to monitor the
activities in individual CNC machine tools
on host computer.
Therefore, better shop floor control can be
achieved.
2004
53
TYPES of CNC CONTROL
SYSTEMS


2004
Open-loop control
Closed-loop control
54
OPEN-LOOP CONTROL SYSTEM






In open-loop control system step motors are
used
Step motors are driven by electric pulses
Every pulse rotates the motor spindle through a
certain amount
By counting the pulses, the amount of motion
can be controlled
No feedback signal for error correction
Lower positioning accuracy
2004
55
CLOSED-LOOP CONTROL
SYSTEMS





In closed-loop control systems DC or AC
motors are used
Position transducers are used to generate
position feedback signals for error
correction
Better accuracy can be achieved
More expensive
Suitable for large size machine tools
2004
56