Computer integrated manufacturing slides

Computer integrated manufacturing

1. CNC – Computer Numerical Control Word Address Programming Character: an alphanumeric character or punctuation mark Address: a letter describing the meaning of a number following the letter Word: an address followed by a number, used to describe machine motions and dimensions Block: a complete command to the CNC machine (one or more words, depending on the information needed to command a CNC operation) Program: a sequence of blocks describing the motions of a CNC machine to manufacture a part N G ; G 00 X -3.75 G00 X-3.75 N010 G00 X-3.75 Y2.5 N010 G00 X-3.75 Y2.5 N020 G00 Z1. . . . . N0100 M30

2. CNC – Computer Numerical Control Word Address Programming General Syntax (arrangement of addresses in a block): O – program number (optional), used to identify programs in the MCU memory. Ex: O 0001, O 9999 N – sequence number (optional). MCU executes a program block by block regardless of the sequence number entered. Ex: N 0001, N 9999 G – preparatory functions , usually placed at the beginning of a block and used to prepare the CNC controller to act in a particular mode when processing the other words in a block. The mode is indicated by the numerical value following the G address. Ex: G 00 ( Rapid positioning at maximum feedrate ), G 01 ( linear interpolation at a programmed feedrate ) G 20 ( inch mode ) G 28 ( return to reference point ) G 90 ( absolute positioning ) G 91 ( incremental positioning )

3. CNC – Computer Numerical Control Word Address Programming G code categories: Modal : the G code specification will remain in effect for all subsequent blocks unless replaced by another associated modal G code. Nonmodal : the G code specification will only affect the block in which it appears . Ex: N0010 G91G01X1.0F10.0 N0020 X2.0 N0030 Y2.0 N0040 G90G00Y0 N0050 G28 X , Y , Z , … – dimension words , used to specify the movement of the programming axes (Cartesian coordinate system). G91, G01, G90 and G00 are modal G28 is non-modal

4. CNC – Computer Numerical Control Word Address Programming F – feed rate , the rate at which the spindle moves along a programming axis. F is modal English system: in/min Metric system: mm/min Ex: F10. – a feedrate of 10 in/min, F10 – a feedrate of 0.001 in/min ( Fanuc controllers ) S – spindle speed , the speed at which the spindle rotates (rpm) Spindle rotation should be specified prior to axis movement M – miscellaneous machine function , used to specify machine functions other than dimensional or axis movements Ex: M 03 (spindle on, clockwise) M 05 (spindle off) M 08 (coolant on) M 09 (coolant off) M 30 (program end)

5. CNC – Computer Numerical Control

6. CNC – Computer Numerical Control Linear Interpolation Machine a rectangular block 3”  2”  0.5”. Cutter ½” end mill. Part zero: X 0 & Y 0 at lower left-hand corner. Z 0 at top of the part.

7. CNC – Computer Numerical Control Linear Interpolation Machine a rectangular block 3”  2”  0.5”. X0 & Y0 at lower left-hand corner. Z0 at top of the part. Cutter ½” end mill. O0001 N0010 G20 G90 N0020 G92 N0030 T01 M06 N0040 M03 S800 N0050 G00 X-.5 Y-.5 N0060 G00 Z.25 N0070 G01 Z-.55 F5.0 N0080 G01 X-.25 Y-.25 N0090 Y2.25 N0100 X3.25 N0110 Y-.25 N0120 X-.5 N0130 Z.25 N0140 G00 Z 1.0 N0150 M05 N 0160 G28 N0170 M30 X=-0.5 Y=-0.5 Z=.25 Y X Z X=M.HOME Y=M.HOME Z=M.HOME X=-0.5 Y=-0.5 Z=-0.55 X=-0.5 Y=-0.5 Z=M.HOME X=-0.25 Y=-0.25 Z=-0.55 X=-0.25 Y=2.25 Z=-0.55 X=3.25 Y=2.25 Z=-0.55 X=3.25 Y=-0.25 Z=-0.55 X=-0.5 Y=-0.25 Z=-0.55 X=-0.5 Y=-0.25 Z=.25 X=-0.5 Y=-0.25 Z=1.0 X=-0.5 Y=-0.25 Z=1.0

8. CNC – Computer Numerical Control Circular Interpolation Circular Interpolation commands G02 & G03 – for cutting a circular contour It moves the tool along a circular path from the initial (current) position to the final position at a programmed feedrate Note:(1) Circular interpolation is executed on a plane . Plane selection (modal commands): G17 – XY (default), G18 – XZ, G19 – YZ (2) Tool motion direction: G02 – clockwise ; G03 – counterclockwise (3) Absolute or Incremental coordinates are being used General Syntax: G02 (G03) Xn Yn (Zn) In Jn ( Kn ) (Fn)

9. CNC – Computer Numerical Control Circular Interpolation Example: N010 G90 (Absolute) N020 G17 (XY Plane) N040 G01 X3.0 Y.25 F10.0 N040 G02 X4.125 Y-3.9486 I0. J-2.25 Calculation: End Position: X=3+2.25cos(60) Y=-2-2.25sin(60) I and J: (center-initial) I=3-3 J=-2-0.25 Y X 2 3 X Y 60  R 2 J Initial position of ½” tool End position

10. CNC – Computer Numerical Control Circular Interpolation Circular Interpolation via Radius Specification – coding the radius (R) of the circular arc instead of I, J, and K General Syntax: G02 (G03) Xn Yn (Zn) Rn (Fn)

11. CNC – Computer Numerical Control G-code for Turning DEF WORK PS LC, [0,0], [96,90] END DRAW G00 X500 Z500 G50 S2500 NLAP1 G81 G00 G42 X50 Z98 G01 X60 Z88 F0.15 Z80 G02 X70 Z75 L5 G03 X80 Z70 L5 G01 Z60 G02 X80 Z35 L40 G01 Z25 X90 Z20 X95 G40 G80 G00 X95 Z100 S670 T010101 M03 M08

12. CNC – Computer Numerical Control G-code for Turning DEF WORK PS LC, [0,0], [96,90] END DRAW G00 X500 Z500 G50 S2500 NLAP1 G81 G00 G42 X50 Z98 G01 X60 Z88 F0.15 Z80 G02 X70 Z75 L5 G03 X80 Z70 L5 G01 Z60 G02 X80 Z35 L40 G01 Z25 X90 Z20 X95 G40 G80 G00 X95 Z100 S670 T010101 M03 M08 ---------------- ROUGH CUT -------------------- NT1 G96 S130 G85 NLAP1 D3 F0.3 U1.0 W0.1 G00 X95 Z100 G97 X500 Z250 S930 M01 X95 Z100 T020202 ---------------- FINISH CUT ------------------- NT2 G96 S180 G87 NLAP1 G00 X95 Z100 M05 M09 M02