1. The Cartesian Coordinate System
Basis for plotting all machine table positions Y+ Y-
The left/right axis is X (East/West) Z+
The front/back axis is Y (North/South) I IV
III II
Consists of four quadrants
+,-
-,-
+,+
-,+ X+ X-
Points are plotted as (X,Y) Pairs
(0,0)
Negative numbers have (-) prefix Z-
Positive numbers have no prefix
Where the X and Y axes cross is the (0,0) point
The up/down axis is Z and controls the tool height

2. The Home Position Default zero position of the X Y plane
After power up the machine must be Homed
The spindle is located at the Machine Zero position after Homing
The machine may now be programmed with reference to Machine Zero

3. Absolute Positioning
All points used for movement are plotted using their absolute position from the (0,0) point or Active Origin
CNC programming uses G codes to execute commands
G codes consist of a G followed by a number - like G90
G90 is the command to Enable Absolute Positioning relative to the active origin
G90 is Modal as well as a Default command
Modal commands stay active until they are intentionally cancelled or replaced by another command.
Non-Modal commands are automatically cancelled or replaced as soon as they are completed.
Default commands become active when the machine is powered up, the reset button is pushed, or after an M30 command.

4. Absolute Coordinates A (6,7) C (-7,-1) (-5,8) D (2,-2) B
Drawing C.1 9 7 6 5 3 4 8 2 1 A B C D A
(6,7) C
(-7,-1)
(-5,8) D
(2,-2) B
(X value, Y value)

5. Absolute Coordinates C Write the Absolute X,Y locations
Drawing C.2 9 8 7 6 5 4 3 2 1 1 2 3 4 5 6 7 8 9 C 9 9 8 8
Write the Absolute X,Y locations 7 7 6 6
in the chart below 5 A 5 4 D 4 3 B 3 A
(7,5) I
(-9,-5)
III 2 2 E 1 1
(1,3) I
(-2,-2)
III 1 F H 1 B F 2 2 3 E 3
(-2,9) II
(1,-7) IV C G 4 4 5 G 5
(-9,2) II
(8,-1) IV 6 6 D H 7 7 8 8 9 9 9 8 7 6 5 4 3 2 1 1 2 3 4 5 6 7 8 9

6. Exercise C.3
Label the points of the part
using Absolute Coordinates
Part 1
Part 2 20 30 A B C D A
X Y 0 B
X Y 0 B
X Y 30 C
X Y 0 C
X Y 30 D
X Y -30 D
X Y 0 A
X Y -30
Part 3
Part 4 C
X Y 0 D
X Y 0
In each of the parts the origin is placed in a different corner.
Fill in the X and Y values for each point with regards to the part origin D
X Y -30 A
X Y 0 A
X Y -30 B
X Y 30 B
X Y 0 C
X Y 30
In each of these parts the origin has been placed in a different corner.
Fill in the X and Y values for each point with regards to the part origin.

7. Linear Movement
G00 Enables rapid movement of the machine. Rapid positioning is never used for cutting. It is modal and default.
G01 Enables linear movement using a specified feed rate. The feed rate specified with an F followed by a number representing units per minute. The feed rate is modal and stays active until replaced by another feed rate or the machine is reset.
Examples:
G01 F30 - Specifies linear movement with a feed rate of 30 units per minute
G01 F10 - Specifies linear movement with a feed rate of 10 units per minute

8. Exercise C.7
Label the points of the part using the type
of motion required for G90 20 30
A (0,0) B C D
FAST!
10 IPM
12 IPM
12IPM
A-B
B-C
C-D
D-A
G 90
Point
Motion X Y
Feedrate
Note: G00 is never used for cutting. It is used in this example to show movement options only.
G01
X Y30
F10
G00
X Y30
G01
X Y0
F12
G01
X Y0
F12

9. Drawing C.8
5.0
6.0
9.0
10.0
15.0 A. B. C. D. E.
Fast!
12 IPM
Fast!
11 IPM
10 IPM
(0,0)
A-B
Point
Motion X
X______
Y______ Y
Feedrate
B-C
C-D
D-E
E-A
______
F______
G90
G01 10
Note: G00 is never used for cutting. It is used in this example to show movement options only.
G01 6 11
G01 5 15 12
G00 10 15
G00 10

10. Arc Motion G02 & G03 End G03 G02 Counter Clockwise Start
Cutting arcs and circles requires the simultaneous movement along two axes. This is called Interpolation.
G02 - Is the command for Clockwise Interpolation
G03 - Is the command for Counter Clockwise Interpolation
Both G02 and G03 will use the active feedrate or they can be assigned a new feedrate.
End
G03
Counter
Clockwise
G02
Start

11. Specify Motion Codes: G01, G02, G031. 2. 3. 4. 5. 6. 7. 8. 9.
10.
11.
12.
Drawing D.2
G02
G01
G03
G03
G01
G02
G03
G02
G03
G01
G02
G01

12. The Radius Method is used to cut arcs.
It incorporates the Direction (G02 or G03), the Endpoint (X,Y), the Radius (R) of the arc, and the Feedrate (F) of the desired cut into the command line.
G03 X-10 Y10 R10 F200.
Start (0,0)
End (-10,10)
mm/m
R10

13. Origins
User created Cartesian Coordinate Systems may be located anywhere on the machine table.
The (0,0) points of these systems are called origins
The machine table coordinates of these origins are stored in the controller’s memory
The Fanuc Controller can create and save up to 5 origins
These origins are saved in a data table referred to as the Origin Table
When an origin is made active all subsequent G90 positions are plotted in reference to the active origin.
The Z0 position after an origin command is usually at the top of the CNC worktable

14. Origins G54 – Machine zero origin – Cannot be used for parts
G55 – G59 Workpiece origins 1 through 5 are used for parts
By activating a workpiece origin any previously called origin is deactivated
G52 - Creates an offset from the active origin
Example:
G55 G52 X-.3 Y-.3 Z2 Offsets origin 1 by -.3 on the X axis, by -.3 on the Y axis, and by 2 on the Z axis.

15. Z 0 Position C B A A. Z 0 with Origin 1 Activated. Example: G55
CMS
Router
Spindle A B C
A. Z 0 with Origin 1 Activated.
Example: G55
B. Z 0 with Origin 1 Activated and Part offset activated.
Example: G55 G52 Z1.181
C. Z 0 with Origin 1 Activated and Part offset and Tool length compensation.
G43 H7 Z0

16. G53 –Programming in Reference to Machine Zero
Default (0,0) point for (X, Y) coordinates are located at the center of the main spindle
Zero for the Z axis is at the top of the Z stroke
Straight line moves only, no arcs or circles
Movements may be performed in either Rapid or Feed speeds (G00 / G01)
Is Non-modal
Used for moving the machine to safety positions

17. G53 Programming G 5 3 X 7 6 Y 1 C M S W o r k t a b l e R u s p i n d5 3 X 7 6 Y 1 C M S W o r k t a b l e R u s p i n d h m .
Drawing C.9

18. M06 Tool Change
Tools may be automatically loaded from the tool holder or manually inserted by hand using the M06 code
Tools are designated by a T followed by the tool holder number of the tool
Example:
T5 M06 loads tool number 5
To empty the spindle, use T0 M06.
Try not to interrupt a tool change. (See tool change errors)

19. Controlling Spindle Rotation
May spin either clockwise or counter clockwise
M3 is the code for clockwise rotation
M5 is the code for spindle stop
M8 is the code to turn on internal and external coolant
The speed is always in Rotations per Minute (RPM)
An S code after the M command sets the RPMs
Examples:
M3 S4500 – Clockwise rotation at 4500 RPM

20. Tool Length Offsets – G43 H_ Z_
The tool length and tool diameter are manually entered in the offset table and stored in the controller’s memory
When a tool is changed the offset information is read from the offset table location corresponding to the H number
The tool tip is then moved to the Z distance above the part
The offset table can store over 300 offset combinations
Examples:
G43 H01 Z3= Tool length offset is activated from offset table location 1 and the tool tip is moved to 3 inches above the part
G49 H0 = Tool length offset is deactivated
G53 Z0 Moves spindle to top of Z stroke
G49 H0 Deactivate tool length offset
(Note: G53 Z0 is required prior to deactivating a tool length offset)

21. Tool Diameter Offset – G42 D_
The tool length and tool diameter are manually entered in the offset table and stored in the controller’s memory
When a tool is changed the offset information is read from the offset table location corresponding to the D number
The tool center is now offset from the tool path the value of the radius of the tool.
G42 Specifies the tool center is offset to the right of the tool path
Examples:
G42 D01 Tool diameter offset is activated from offset table location 1
G40 D0 Cancels tool diameter offset

22. Drawing H.1 Tool Cone Tool Cone in Router Spindle Tool Length =
Spindle Nose to
Tool Tip
Tool Æ
Tool Æ

23. Ending the Part Program
M30 is at the end of of all programs
M30 resets the machine to defaults
M30 rewinds the program
M30 deactivates any active origins

24. Programming
O0001 (PART PROGRAM NAME = SQUARE 15” X 15”)
(1/2” DIAMETER STRAIGHT TOOL)
N1 G91 G17 X0 Y0
N2 G00 G90 G53 Z0
N3 G55
N4 G52 Z.75
N5 T5 M06
N6M08
N7 M03 S5000
N8 X0 Y-1
N9 G43 H5 Z4
N10 Z1.
N11 G01 Z-.78 F10
N12 G42 X0 Y0 D5
N13 Y15
N14 X-15
N15 Y0
N16 X0
N17 G40 X1 Y0 D0
N18 G00 Z1
N19 G53 Z0
N20 G53 X141 Y78
N21 G49 H0
N22 M05 S0
N23 M30
15.0
1.0
Part thickness: .75"
Requires a half inch mill bit from tool holder position 5. This tool runs clockwise with coolant at 4500 RPM at 10 IPM. The length and diameter values are stored in offset table position 5. The part thickness is 0.75 inches.

25. CODE EXPLAINATION
O0001 (PART PROGRAM NAME = SQUARE 15” X 15”)
(1/2” DIAMETER STRAIGHT TOOL) First 2 lines: Program name and comments
N1 G91 G17 X0 Y0 Set Plane of interpolation
N2 G00 G90 G53 Z0 Safety move to top of Z stroke
N3 G55 Activate Origin 1
N4 G52 Z.75 Offset in Z direction for mat’l thickness
N5 T5 M06 Get tool
N6M08 Activate cooling
N7 M03 S5000 Spindle CW rotation on
N8 X0 Y-1 Move close to part
N9 G43 H5 Z4 Activate tool offset
N10 Z1. Move tool tip to 1 inch over part
N11 G01 Z-.78 F10 Move tool tip to just under part
N12 G42 X0 Y0 D5 TSR active diameter offset move to part
N13 Y15 Move to upper right corner
N14 X-15 Move to upper left corner
N15 Y0 Move to lower left corner
N16 X0 Move to lower right corner
N17 G40 X1 Y0 D0 Deactivate diameter offset move from part
N18 G00 Z1 Move tool tip 1 inch above part
N19 G53 Z0 Safety move to top of Z stroke
N20 G53 X141 Y78 Safety move away from part
N21 G49 H0 Cancel tool length comp
N22 M05 S0 Deactivate spindle
N23 M30 End Program

26. Program Sections O0001 (PART PROGRAM NAME = SQUARE 15” X 15”)
(1/2” DIAMETER STRAIGHT TOOL)
N1 G91 G17 X0 Y0
N2 G00 G90 G53 Z0
N3 G55
N4 G52 Z.75
N5 T5 M06
N6M08
N7 M03 S5000
N8 X0 Y-1
N9 G43 H5 Z4
N10 Z1

27. Program Sections N11 G01 Z-.78 F10 N12 G42 X0 Y0 D5 N13 Y15 N14 X-15
N21 G49 H0
N22 M05 S0
N23 M30

28. Exercise L.1
Write a Full Part Program to cut the part shown below. Use Origin 2. This part requires one tool. A 1/2” Straight Cutter. This tool is stored in the Automatic Tool Changer, position number Two. The length and diameter of this tool is being stored in the offset table, also position number Two. This tool cuts at 4500 RPM and a feed rate of 10 IPM. The part is 0.5” thick.
20.0
4.0
8.0
16.0
R0.5
1.0
Drawing L.1
(0,0)

29. Exercise L.1 Code (Exercise L.1 - Fanuc) (1/2 INCH STRAIGHT CUTTER)
G91 G17 X0 Y0
G00 G90 G53 Z0
G55
G52 Z.5
T2 M6 M8
M3 S4500
X0 Y-1
G43 H2 Z4 Z1
G01 Z-.53 F10
G42 D2 X0
Y16
X-20
Y12
X-16.5
G02 X-16 Y11.5 R.5
G01 Y8.5
G02 X-16.5 Y8 R.5
G01 X-20 Y0 X0
G40 X1 D0
G00 Z1
G53 Z0
G53 X-141 Y78
G49 H0
M05 S0
M30

30. Exercise L.2
Write a Full Part Program to cut the part shown below. Use Origin 1. This part requires one tool. A 1” diameter straight cutter. This tool is stored in the Automatic Tool Changer, position number Eight. The length and diameter of this tool is being stored in the offset table, position number One. This tool runs at 4500 RPM with a feed rate of 10 IPM. The part is 1.5” thick.
10.0
1.0
R5.0
R2.0
(0,0)
Drawing L.2
4.0

31. Exercise L.2 Code (Exercise L.2 - Fanuc) (1 INCH STRAIGHT CUTTER)
G91 G17 X0 Y0
G00 G90 G53 Z0
G57
G52 Z1.5
T8 M6 M8
M3 S4500
X0 Y-1
G43 H1 Z4 Z1
G01 Z-1.53 F10
G42 X0 D1
Y10
X-4
G02 X-8 R2
G01 X-18
G03 Y0 R5
G01 X-8
G02 X-4 R2
G01 X0
G40 X1 D0
G00 Z1
G53 Z0
G53 X141 Y78
G49 H0
M05 S0
M30

32. Exercise L.4
Write a program to cut the part shown below. Use Origin 1. This part requires one tool, a 3/8” straight cutter that is stored in the Automatic Tool Changer position number three. This tool runs at 4500 RPM with a feed rate of 10 IPM. The length and diameter of this tool is being stored in the offset table position number three. The part is 3/8” thick.
(0,0)
18.0
9.0
R3.0
3.0
Four places
R1.0
1.0

33. Exercise L.4 Code (Exercise L.4 - Fanuc) (3/8 INCH STRAIGHT CUTTER)
G91 G17 X0 Y0
G00 G90 G53 Z0
G56
G52 Z.375
T03 M06
M08
M03 S5000
X0 Y-1
G43 H3 Z4 Z1
G01 Z-.41 F10
G42 X0 Y0 D3
G02 X3 Y3 R3
G01 Y12
G02 X0 Y15 R3
G01 X-18
G02 X-21 Y12 R3
G01 Y3
G02 X-18 Y0 R3
G01 X0
G02 X1 Y-1 R1
G40 D0
G00 Z1
G53 Z0
G53 X-141 Y78
G49 H0
M05 S0
M30