(0,0) The Cartesian Coordinate System I IV III II +,- -,- +,+ -,+ Y+ Y- Z+ Z- X+ X- Basis for plotting all machine table positions The left/right axis is X (East/West) The front/back axis is Y (North/South) Consists of four quadrants Points are plotted as (X,Y) Pairs Negative numbers have (-) prefix 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

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 The Home Position

Absolute Positioning and Linear Movement 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 a Modal and 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.

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

A B C D E F G H Write the Absolute X,Y locations in the chart below Absolute Coordinates Drawing C.2

Label the points of the part using Absolute Coordinates Part 1 D A B C Part 2 Part 3 Part 4 B C D A C D A B D A B C Exercise C.3 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.

Linear Movement G00 Enables rapid movement of the machine. –Is never used for cutting. –Is modal and default. G01 Enables linear movement using a specified feed rate. –F is followed by a number (units per minute) –Is modal 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

of motion required for G90 Label the points of the part using the type Exercise C A (0,0) B C D  10 IPM 12 IPM RAPID! A-B B-C C-D D-A G 90 Point Motion X Y Feedrate ______ ______

A-B From - To Motion X X______ Y______ Y Feedrate B-C C-D D-E E-A ______ X______ Y______ X______ Y______ X______ Y______ X______ Y______ F______ Drawing C.8 Enter the motion type, the X & Y values, and the feedrates in the table below.

End G03 Counter Clockwise G02 Start End Arc Motion G02 & G03 Cutting arcs and circles requires the simultaneous movement of 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.

Specify Motion Codes: G01, G02, G03 G03 G01 G02G01 G03 G02 G03 G01 G02

The Radius Method The Radius Method is used to cut arcs. This command incorporates the Direction (G02 or G03), the Endpoint (X,Y), the Radius of the arc, and the Feedrate of the desired cut. G03 X-10 Y10 R10 F200. Start (0,0) End (-10,10) 200 MMPM R10

Origins (Osai) Cartesian Coordinate Systems may be located anywhere on the machine table. The (0,0) points or the home positions of these systems are called origins The Z 0 or home position for these systems is set at the top of the CNC worktable (vacuum pods) The machine table coordinates of these origins are stored in the controller’s memory The Osai 10 Series Controller can create and save up to 10 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.

UAO - Use Absolute Origin The UAO code is used to activate a specific origin (1-10) All G90 (Absolute) positions will be in reference to this origin Deactivates all other active origins for the declared axes Is modal Examples: (UAO, 1) = Origin number one is made active for all axes (UAO, 6, X, Y) = Origin number six is made active for the X and Y axes only (UAO, 0) = Reactivates the Machine Home position for all axes

UTO (UOT) - Use Temporary Origins Used to temporarily offset an origin along the specified axes All G90 (Absolute) positions will be in reference this active offset origin UTO Deactivates all other active origins for the declared axes Is modal Examples: (UTO, 1, X-.5, Y.5, Z2) = Activates a temporary offset for origin 1 at X-.5, Y.5, and Z2. (UTO, 5, Y-.3, Z2) = Activates a temporary offset for origin 5 at Y-.3, and Z2. (no X offset)

Z 0 Position A.Z 0 with Origin 1 Activated. Example: (UAO,1) B.Z 0 with Origin 1 Activated and Part offset activated. Example: (UTO, 1, Z1.181) C.Z 0 with Origin 1 Activated and Part offset and Tool length compensation. Example: (UTO, 1, Z1.181) h7 Z=0

G79 –Absolute Reference to Home Position 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 Generally used for moving the machine to safety positions

G79 Programming Drawing C.9

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: load tool number 5 T5 M06 G300 (In auto mode a G300 must follow a T# M06 command.) To empty the spindle, use T0 M06. After the spindle comes to the front of the machine, press the RESET button, then type T0 M26 (MDI Mode) Try not to interrupt a tool change. (See tool change errors)

Tool Offsets – h The tool length and tool diameter are both manually entered in the offset table and stored in the controller’s memory When a tool change is made the tool offset information is read from the offset table location corresponding to the h number The offset table can store over 300 offset combinations Examples: h1 = Tool length and diameter values are read from offset table location 1 h99 = Tool length and diameter values are read from offset table location 99 h0 = Tool length and diameter offset values are deactivated The h must always be typed in lowercase for this function.

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

Controlling Spindle Rotation M3 is the code for clockwise rotation M5 is the code for spindle stop The speed is always in Rotations per Minute (RPM) An S code after an M3 sets the RPMs Examples: M3 S4500 – Clockwise rotation at 4500 RPM

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

Programming 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 Part thickness:.75" ;PART PROGRAM NAME = SQUARE 15X15 ;1/2” DIAMETER STRAIGHT TOOL N1 G00 G79 Z0 N2 (UOT,1,X0,Y0,Z.75) N3 T5 M06 N4 G300 N5 h5 N6 M13 S4500 M7 N7 X0 Y-1 N8 Z1 N9 G01 Z-.78 F10 N10 G01 G42 X0 Y0 F10 N11 Y15 N12 X-15 N13 Y0 N14 X0 N15 G40 X1 N16 G00 Z1 N17 G79 Z0 N18 G79 X0 Y64 N19 h0 N20 M05 S0 N21 M30

CODE EXPLAINATION ;PART PROGRAM NAME = SQUARE 15X15Comment line for program name ;1/2” DIAMETER STRAIGHT TOOLComment line for tool description N1 G00 G79 Z0Rapid move to machine Z 0 / Safety move N2 (UOT,1,X0,Y0,Z.75)Use origin 1, set Z0 to top surface of part N3 T5 M06Tool change N4 G300Tool change sub-program N5 h5Use tooling offset table position 5 values N6 M13 S4500 M7CW 4500 RPM with int/ext coolant N7 X0 Y-1Position machine to 1 inch (Y) away from part N8 Z1Move tool end to 1 inch above part N9 G01 Z-.78 F10Move tool end to just below N10 G01 G42 X0 Y0 F10Enable TSR  comp, move to N11 Y15Move to upper right corner (0,15) N12 X-15Move to upper left corner (-15,15) N13 Y0Move to lower left corner (-15,0) N14 X0Move to lower right corner (0,0) N15 G40 X1Disable tool diameter comp N16 G00 Z1Rapid move tool tip to 1 inch above part N17 G79 Z0Move to machine Z 0 / safety move N18 G79 X0 Y64Park machine away from part N19 h0Disable tool offset compensation values N20 M05 S0Spindle Stop (Cancels M13) N21 M30End of Program – Reset / Rewind

Program Sections ;PART PROGRAM NAME = SQUARE 15X15 ;1/2” DIAMETER STRAIGHT TOOL “Comments” N1 G00 G79 Z0 N2 (UOT,1,X0,Y0,Z.75) N3 T5 M06 N4 G300 N5 h5 N6 M13 S4500 M7 N7 X0 Y-1 N8 Z1 “Start”

Program Sections N9 G01 Z-.78 F10 N10 G01 G42 X0 Y0 F10 N11 Y15 N12 X-15 N13 Y0 N14 X0 “Working” N15 G40 X1 N16 G00 Z1 N17 G79 Z0 N18 G79 X0 Y64 N19 h0 N20 M05 S0 N21 M30 “ End ”

Exercise D1 Write a similar program to cut this part in a CCW direction. Use Origin 5 and start at (0,0). This part requires a1/2” finger bit that is stored in the Automatic Tool Changer position number 2. The length and diameter of this tool are being stored in offset table location number 201. This tool cuts at 4500 RPM and has a feed rate of 10 IPM. The part is 0.5” thick.

G02 X4 Y11.5 R.5 G01 Y8.5 G02 X3.5 Y8 R.5 G01 X0 Y0 G40 Y-1 G00 Z1 G79 Z0 G79 X0 Y64 h0 M05 S0 M30 ;Exercise D1 – Osai – 0210 ;1/2 INCH STRAIGHT CUTTER G00 G79 Z0 (UTO, 5, Z.5) T2 M6 G300 h201 M13 S4500 M7 X-1 Y0 Z1 G01 Z-.53 F10 G42 X0 Y0 X20 Y16 X0 Y12 Code for D1

Exercise L.2 Write a program to cut the part shown below. Start at the plus sign and go CCW around the part. Use Origin 1. This part requires a 1” diameter router bit that is stored in the Automatic Tool Changer position number 8. The length and diameter of this tool is being stored in the offset table position number 47. This tool runs at 4500 RPM with a feed rate of 10 IPM. Use 8 IPM for lead in only. The part is 1.5” thick.

Exercise L.2 Code ;(Exercise L.2 - Osai) ;(1 INCH STRAIGHT CUTTER) G00 G79 Z0 (UTO,1,Z1.5) T8 M6 G300 h1 M13 S4500 M7 X0 Y-1 Z1 G01 Z-1.53 F10 G42 X0 Y0 Y10 X-4 G02 X-8 R2 G01 X-18 G03 Y0 R5 G01 X-8 G02 X-4 R2 G01 X0 G40 X1 G00 Z1 G79 Z0 G79 X0 Y64 h0 M05 S0 M30

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.

Exercise L.4 Code ;(Exercise L.4 - Osai) ;(3/8 INCH STRAIGHT CUTTER) G00 G79 Z0 (UTO, 1, Z.375) T03 M06 G300 h3 M13 S4500 M07 X0 Y-1 Z1 G01 Z-.41 F10 G42 X0 Y0 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 G79 Z0 G79 X0 Y64 h0 M05 S0 M30