to Introduction CNC Machining
Design ----> Build & Prove Prototype ----> Production
The bugs are worked out in the prototype stage which is getting shorter time wise. In
fact some manufacturers are skipping the hard prototype models and going in for
computer simulations instead. Once a prototype is modified and proved out, then it goes
into the production stage of manufacturing.
Consider a large, odd-shaped part to be machined out of solid block of aluminum for a
pump assembly in an aircraft component. Very few parallel planes or 90 angles.
Think of your experience on the vertical milling machine, could you machine this
part manually?
3-axis of control (X,Y,Z) can handle about 90% of the work that you run into on a
day-to-day basis. This part does not fit those conditions.
We can write and run a computer program to drive a cutter on a vertical milling machine
to make something in 3-D space from a mechanical drawing - CAD drawing is standard
practice CAD/CAM use the same data base. Therefore, avoid reentering data.
However, CAM came first.
Computer programs allow you to generate points, lines, arcs, tool changing,
speeds, feeds without touching the machine except for loading/unloading the part
and starting/stopping the machine.
So take the handles (hand cranks) off the milling machine and replace them with a
servo-motor drive or stepper type drive motor which allows the computer to drive
the motor that will accurately position the table.
Chapter 39 (37) &
40 (38)
Week #8 - Lecture
Terms
NC Lathe Turning Center
NC Mill Machining Center
DNC Distributed NC (DNC) includes the use of a
central computer serving over a number of individual
CNC machines with onboard minicomputers
(networking). Direct numerical control in which
several machines are directly controlled step by step
by a central main frame computer. If the computer
goes down, all the machines are inoperative.
CNC Computer numerical control in which a
minicomputer or microprocessor is an integral part of
the control panel of a machine or equipment
(onboard computer).
General CNC Info
Lines of code (for tasks or functions) are sent into the computer on
board the NC machine which tells the servo-motors how far and
how fast to move.
It has memory capability so that we can load and run a proven
program out of memory. It has editing capability for adding,
deleting, and modifying lines.
Motor and leadscrew arrangement in a NC positioning system:
Fig. 39.4,
p. 891
CNC Notes
Programming format uses letters and numbers (G code). The beauty
of the NC system is once the program has been proved, the
accuracy of the machine tool is dependent upon the:
cutter dimensional stability (gets dull) that is one reason why we
use coolants and expensive carbide tooling
reproducibility of machine movement (X,Y,Z) that is why NC
machines are expensive.
(+/- 0.001 is just as easy to make as +/- 1/8)
Initially establish the origin (X,Y,Z) and set it when the machine is
turned on and at the start of any operator change. (In a hole, set
(0,0) at center of hole. Set Z = 0 as top of part.)
Program the movement of the center line of the cutter with respect
to a know position. Therefore, offset the radius of the cutter.
- is needed, but + is not required.
CNC Notes (Cont.)
In relation to the movement in X & Y, the table moves not the
cutter. The cutter moves in Z direction.
By jogging the table of the machine, tram the lower left corner
of the part with the side of the centering instrument (Edge
Finder) (NOT the center line of the mill's spindle) and offset
by the difference between its radius & the cutting tools
radius to set the X- & Y- origins.
TRAM dial indicating device, etc, to locate the (0,0) point.
Use absolute mode for Z-direction:
Any "-" moves will drive the cutter into the workpiece.
Rapid feed, G00, down to Z = 0.050" to save time.
Types of Codes
General Codes - Alphabetical Codes
Preparation Codes
G Codes - General Instructions for Executing
the Program
Event Codes
Dimensional Coordinates X-Y-Z
Misc. Codes
Like Tool Changes, like Spindle On or Off
Selected Common Codes
O
Starts the definition of the program number (Alphabetical)
N
Line of code number (for tasks or functions which tells the servo-motors how far and how fast
to move.) (N Sequence number identifies the block of information)
G
is called a preparatory code (function), e.g., you are telling the computer to prepare for the
data that follows and to interpret that data in a specific manner. (G Mode number Requests
different control functions, including preprogrammed machining subroutines. "25 commonly used "G" codes
(50-70 for more complicated NC systems).)
G90 Absolute mode: Computer references from the origin (0,0) Usually the default.
G91 Incremental mode: Computer references from where it is presently. (Delta change
with stepping from point-to-point which usually comes at the convenience of the
programmer and usually due to mechanical dimensions on drawings.)
(In this mode, if you return to the starting point, the sum of + and - movements is zero for
each direction. So check your work.)
G0 or G00 Rapid move to the X-Y-Z coordinate (point) in air with no metal cutting to
save time. Therefore, the feed rate, F, is preset very fast.
Example: G0X-.25Y-.25Z10
Why 2 lines of code for Z? Something in the
G0Z.5
way?
G1 or G01 Feed to the X-Y(1.657) or Z(0.6) coordinate (point) linear movement
Examples: G1Z-0.6F20
(G91: Z = -1.1 = -(0.5)+(-0.6)
G1Y1.657F40
(G91: Y = 1.907 = -(-.250)+(1.657)
The mode-number stays the same unless it is overridden by a new mode-number.
Do not need to repeat a coordinate command if it does not change by being overridden by a
new value.
Selected Common Codes (Cont.)
F
Feed rate (ipm) for this operation (Alphabetical)
F40 Peripheral milling
F20 Plunge milling (usually half of peripheral)
S
Spindle speed (rpm) for this operation (Alphabethical)
Example: S5000 for aluminum
T#
Tool number to use from a library or magazine (Alphabetical)
Tells the machine the location of the tool in the tool holder or tool turret.
T1 means tool #1 is found and is either automatically loaded (with verification by
the operator); or an indication light is lit on tool #1's storage caddy, and the
tool is manually loaded by the operator. To keep operator awake!
M
Miscellaneous functions (Some M codes are for the tape old system.)
M03 Spindle on clockwise
M05 Spindle off
M06 Tool change
M08 Flood coolant on
M09 Flood coolant off
M30 End of program
M50/51 Move spindle up/down
Z0
Top or bottom of the part at 0.000
Other Common Codes
G2 or G02
Feed to the X-Y coordinate (end point) in a clockwise arc
G3 or G03 Feed to the X-Y coordinate (end point) in a counter clockwise arc
I Defines incremental distance/movement from start point of the arc
(last point of the center line of the CUTTER) to the center point (NOT
the end point) of the arc in the X-direction. & gives (+/-) sign
J Defines incremental distance/movement from start point of the arc
(last point of the center line of the CUTTER) to the center point (NOT
the end point) of the arc in the Y-direction. & gives (+/-) sign
Example: G2X-.333Y1.500I-.167J.5
THE ARC WILL START AT THE LAST POINT ( X- & Y- COORDINATES)
AND WILL END AT THE NEW POINT (X=-.333 & Y=1.500
COORDINATES.)
Do not need to repeat a modal command if it does not change by being
overridden by a new mode-number.
Other Common Codes
G28
G43
G54
G90
G91
H1
- Return to reference Point
- Tool Length Compensation
- Select Tool Work Coordinate System 1
- Absolute
- Incremental
- Tool Length Offset Selection -(From Offset
Library in the Computer)
Dimensional Coordinates
X, Y, Z, a, b, c
Dimensional coordinate data: linear and angular motion
commands for the axis of the machine. (Table Movement)
Example: X2.5Y-.5Z-.3
+X
O
+Y
+Z is up from the table
Z0 Top (or bottom) of the part is at 0.000
- is needed, but + is not required.
Do not need to repeat a coordinate command if it does not change
by being overridden by a new value.
Objective
I want you to learn to write a program for an introductory
problem having a simple shape. Most of you have
written computer programs before, but you have
produced nothing but paper print outs with useful
information. From our exercise, you could make an
actual part - numerically control the machine.
Sample Milling Problem #1
Pick an origin, pick a cutting direction, and layout the
coordinates of the cutters center by offsetting from the
desired part the radius of the milling cutter.
Layout of Milling Cutter Coordinates for
Sample Milling Problem #1
X = 2.25
Y = 1.75
Programming Sample Milling Problem #1
Assume:
Should always be verified!
The origin (X,Y,Z) has been established.
Spindle is at a safe location to load new workpiece, e.g.,
X=20, Y=20, & Z=10. Haas calls this the Holding
Position.
The part is a 2-D part with the Z-plane shifted, i.e.,
drilling and edge milling movement only. No complicated
air foil sections or contours which would require real 3-D
programming.
CNC Worksheet for Sample Milling Problem #1
O500 (Program name is #500)
N1 G90 (Absolute mode)
Stays until a G91 given
N2 T1M6 (Change to tool #1)
N3 S5000M3M8 (Speed = 5,000, Spindle on
clockwise, Flood coolant on)
N4 G54 (Coordinate system E1 with origin at some
location, X , Y, & Z)
===============================
CNC Worksheet for Sample Milling Problem #1 (Cont.)
===============================
N5 G0
X-.25 Y-.25
Rapid feed to save time
N6 G0
Z.5
(1/2 above top of part)
N7 G1
Z-.6
F20
N8 G1
X-.25 Y1.657 F40
N9 G1
X1.817 Y2.651
Cutters center for starting arc
Path taken (Note: center of arc
*N10G2
X3.25 Y1.75 I.433 J-.901
(2.25,1.75) (last position))
Cutters center when arc is
N11 G1
X3.25 Y-.25
completed
N12 G1
X-.25 Y-.25
N13 G0
Z10
(Will something be in the way when going to Step N14 in a linear line?)
===============================
*N10
G2
X3.25 Y1.75 I.433 J-.901
(XArc CP Cutters center for starting arc = 2.25 - 1.817 = .433)
(YArc CP Cutters center for starting arc = 1.75 - 2.651 = -.901)
CNC Worksheet for Sample Milling Problem #1 (Cont.)
===============================
N14 M5M9 (Spindle and Coolant off)
N15 G0
X20 Y20 Z10
Or N15 G28
(Move tool to safe location to unload completed
workpiece and load new workpiece.)
N16 M30 (program end)
(Use G90) Move to Point A
(Use G91) Move to Point A
G90 Absolute
G91 Incremental
Assume the spindle starts at the T.C. (Holding Position)
location.
+Y
1.000
Not to scale.
A
1.500
2.500
+X
Set Point or
4.500
1.000
Absolute Zero
T.C.
(Use G90) Move to Point A
X1.000 Y1.500
(Use G91) Move to Point A
X-3.500 Y2.500
G90 Absolute
G91 Incremental
Assume the spindle starts at the T.C. location.
+Y
1.000
Not to scale.
A
1.500
2.500
+X
Set Point or
4.500
1.000
Absolute Zero
T.C.
A Program is Written as a set of
Instructions
Line 1 = SELECT CUTTING TOOL
Line 2 = TURN THE SPINDLE ON AND SELECT THE RPM
Line 3 = TURN THE COOLANT ON
Line 4 = RAPID TO THE STARTING POSITION OF THE PART
Line 5 = CHOOSE THE PROPER FEED RATE AND MAKE THE CUTS
Line 6 = TURN OFF THE SPINDLE AND THE COOLANT
Line 7 = RETURN TOOL TO HOLDING POSITION AND SELECT NEXT
TOOL
Guidelines for the use of G Codes
1. Codes come in Groups.
2. Except for G Codes, codes with the same alphabetical address
cannot be used more than once on the same line.
3. G Codes with the same Group Number cannot be used more
than once on the same line.
4. There are modal G codes groups which, once established,
remain in effect until replaced with another code from the same
group.
5. There are non-modal G codes groups, once called, are
effective only in the calling block, and then forgotten. Group 00
are non-model.
Program Format
The programmer needs to be consistent and efficient
in writing the code in the way it is listed and in the
order it appears in the program.
X, Y,Z is in the order of appearance
1. First line using active G Codes should be a tool
number and tool change command.
2. The second line will contain a rapid command (G0).
Absolute or incremental command (G90, G91),A
work Zero for X and Y, a spindle speed
command(Sxxx). And a spindle on clockwise
command (M03)
Program Format
3. The third line will contain a Read tool length
compensation command (G43), a tool length offset
number (H01), a z-axis positioning move (Z.1) and an
optional coolant ON command (M08).
Example:
T1 M06;
G00 G90 G54 X0 Y0 S2500 M03;
G43 H01 Z.1 M08;
To End the Program
1. Change feed to rapid(G00), Cancel cutter
compensation (G40), move cutter away from the
periferal cut, (Y-.3)
2. Retract Z (move it up away from the part), Turn off
Coolant (M09)
3. Return to reference point (G28), move to
incremental (G91), Y0 Z0.
4. End Program (M30