Part Programming Turning Applications

Steps in Part Programming Study of component drawing Deciding sequence of operations Identify machine tool Selecting cutting tool Deciding tool paths Determining Machining Parameters Preparing job and tool set-up plans Writing Part Program Testing Part Program Documentation of Part Program

Terminology used in part programming Absolute system : The co-ordinates are mentioned with respect to one reference point (datum) 2. Incremental System : The co-ordinates are mentioned with respect to the previous point (datum)

Terminology (Continued…) 3. Block and Words : Block - It is a group of words or coded instructions for the NC/CNC system to execute a particular movement Word - Each coded instruction

Terminology (Continued…) The words in the block are in following order : Sequence number (N) Preparatory functions (G) Dimensions (X,Y,Z,U,V,W and I,J,K) Feed functions (F) Spindle speed functions (S) Tool functions (T) Miscellaneous functions

Each line of program == 1 block Each block is composed of several instructions, or (words) Sequence and format of words: N3 G2 X+1.4 Y+1.4 Z+1.4 I1.4 J1.4 K1.4 F3.2 S4 T4 M2 destination coordinates dist to center of circle tool sequence no feed rate spindle speed preparatory function miscellaneous function

4. Formats Sequence of words in which information appears in a program Word address format : Each word is identified by a letter Tab sequence format : Each word is separated from the other by ‘Tab’ character The words are identified by their respective positions in the block

Commonly used ‘G’ codes G00 Rapid Positioning  Function: Moves to a new position as fast as possible.  Syntax: G00 [axis words] Example: G00 X1.2 Y0.3 ; Moves to (1.2, 0.3)

G01 Linear Interpolation Function: Moves to a new position linearly at some feed rate. Syntax: G01 [axis words] [optional feed word] Example: G01 X1.2 Y0.3 F3.0  ; Moves to (1.2,0.3) at 3 units/minute

G02 CW circular interpolation (3D) Function: Moves to a new position in a clockwise circular arc. The arc center is specified with signed offsets from the start position or implicitly by the magnitude of the radius Syntax 1: G02 [two axis words (optional third)] [interpolation parameters] [optional feed word] Syntax 2: G02 [two axis words (optional third)] [radius word] [optional feed word]

Example 1: G17 (plane XY specified for clarity) G00 X0 Y0 (get into start position) G02 X2 Y0 I1 J0 F4

Example 2: G17 (plane XY specified for clarity) G00 X0 Y1 (get into start position) G02 X1 Y0 R1 F4

Important G- Codes G00 Rapid Transverse G01 Linear Interpolation G02 Circular Interpolation, CW G03 Circular Interpolation, CCW G17 XY Plane,G18 XZ Plane,G19 YZ Plane G20/G70 Inch units G21/G71 Metric Units G40 Cutter compensation cancel G41 Cutter compensation left G42 Cutter compensation right G43 Tool length compensation (plus) G44 Tool length compensation (minus) G49 Tool length compensation cancel G80 Cancel canned cycles G81 Drilling cycle G82 Counter boring cycle G83 Deep hole drilling cycle G90 Absolute positioning G91 Incremental positioning Important G- Codes

M-codes m05 Spindle off

COORDINATE SYSTEMS • Right hand rule • Z axis align with the spindle - +Z moves away from the workpiece or the spindle. • X axis - Lathe: perpendicular to the spindle. Horizontal machine: parallel to the table. Vertical machine: +X points to the right. 2

Z axis : align with the spindle X axis : perpendicular to the spindle

Z axis : align with the spindle X axis : perpendicular to the spindle

Other Axes Designations Rotational axes (A,B,C) Secondary linear axes (U,V,W) Incremental dimensions in Circular Interpolation (I,J,K)

Zero points and Reference points Machine zero point (M)-positive end of each axis travel range (Home position) Blocking Point-Workpiece zero point (A) Program zero point (W)-starting point of workpiece or like A Start point (B)-first tool starts the machining process & is determined in program Reference point (R)-floating point (determined by measuring system)

Cutting Process Parameter Selection Cutting Speed (V) : V=DN/1000 Feed(fm) : fm= N x frev Depth of Cut (t) : t=(D1-D2)/2

Canned cycles Multiple repetitive cycles Consist of series of motions repeated no. of times e.g. drilling , boring , tapping Drilling cycle consist of: Rapid approach to workpiece Drill at feed rate Rapid return to initial position

Commonly used Canned cycles G74-Stock removal cycle G78-Multiple threading cycle G81-Drilling cycle G85-Boring cycle

General Structure of Turning Part Program N0 G90 Absolute program mode N1 G71 Metric mode N2 G93 M41 S1500 RPM range, Medium speed N3 G94 Feed rate (mm/min) N4 G28 U0 W0 Go to Home Position N5 M06 T0101 Tool change 01 with offset 01 N6 M03 S1500 Spindle ON N7 G00 X50 Z1 M08 Rapid tool positioning to (50,1) . Coolant ON .

General Structure of Turning Part Program (Continued….) N18 G00 X0 Z1 Rapid tool positioning to (0,1) N19 G28 U0 W0 Go to Home Position N20 M05 Spindle OFF N21 M09 Coolant OFF N22 M02 Program END N23 M30 END of tape and REWIND

Example 01- Step Turning Operation N7 G00 X42 Z1 M08 N8 G00 X40 Z1 N9 G74 X30 Z-60 F0.2 D1 stock removal cycle N10 G00 X32 Z1 N11 G00 X30 Z1 N12 G74 X20 Z-30 F0.2 D1 N13 G00 X22 Z1

Example 02-Clockwise Nose Turning N7 G00 X42 Z-20 M08 N8 G01 X40 Z-20 F0.2 S1500 N9 G02 X0 Z0 I-20 K0 F0.2 S1500 N10 G00 X0 Z2

Example 03-Drilling & Boring Operation N7 G00 X0 Z1 M08 N8 G00 X0 Z10 reference position of drill N9 G81 X0 Z-30 F0.1 S600 N10 G00 X0 Z1 N11 G00 X12 Z1 N12 G85 P10 Q10 U0 W0 F0.15 N13 G01 X12 Z-30 F0.15 S600 N14 G00 X0 Z-30 N15 G00 X0 Z1

Example 04-Threading Operation N7 G00 X26 Z1 M08 N8 G78 X19.09256 Z-30 I0 K2.4572 F0.2 D1 A60 N9 G00 X26 Z1 N10 G28 U0 W0

Example 03- P.U.2008 N7 G00 X60 Z1 M08 N8 G74 X40 Z-40 F0.25 D1 N9 G02 X60 Z-50 I10 K0 F0.35 N10 G00 X62 Z1 N11 G00 X20 Z0 N12 G01 X40 Z-20 F0.35 S400 N13 G00 X42 Z1

Example 03- P.U.2010 N7 G00 X92 Z1 M08 N8 G74 X80 Z-120 F0.25 D1 N9 G00 X82 Z1 N10 G74 X60 Z-70 F0.25 D1 N11 G00 X62 Z1 N12 G00 X40 Z0 N13 G01 X60 Z-20 F0.25 S1500 N14 G00 X62 Z-20 N15 G00 X60 Z-70 N16 G03 X80 Z-80 I0 K-10 F0.25 N17 G00 X82 Z-80

Part Programming Milling Applications

Milling Tools & Operations

Milling Machine Based on axis orientation : Horizontal Milling Machine Vertical Milling Machine

Z axis : align with the spindle X axis : perpendicular to the spindle

Cutting Process Parameter Selection Cutting Speed (V) : V=DN/1000 Feed(fm) : The rate with which workpiece advances under the cutter

Cutting Process Parameter Selection Three Methods : Feed per tooth (fz) : The distance workpiece advances in the time between engagement by two successive teeth (mm/tooth) Feed per cutter revolution (frev) : The distance workpiece advances in the time when the cutter turns through one complete revolution (mm/rev)

Cutting Process Parameter Selection (iii) Feed per minute (fm) : The distance workpiece advances in one minute (mm/min.) All the above methods are related by the equation : fm= N x frev = fz x Z x N where, Z=No of teeth on the cutter

Cutting Process Parameter Selection Depth of Cut (t) : The thickness of material removed in one pass of the workpiece under the cutter It is the perpendicular distance measured between original and final surface of workpiece

Common Preparatory Functions Principal Plane Selection (i) XY plane selection (G17) (ii) XZ plane selection (G18) (iii) YZ plane selection (G19) 2. Interpolations Linear Interpolations (G01) Circular Interpolations (G02 & G03) (iii) Helical Interpolations (G32 & G33)

Tool Compensations Tool Length Compensations (G43) : Tool Pre setter- tool measuring device mechanical ,electrical, optical Tool Length offset ‘H’ Tool register

Cutter Radius Compensations For Contouring Operations Need to calculate tool cutter path by offsetting the contour by an amount equal to the radius of the cutter Compensation OFF (G40) Cutter radius compensation left (G41) Cutter radius compensation right (G42)

Cutter Compensation (G41)

Cutter Compensation (G41/G42)

General Structure of Milling Part Program N0 G17 Principle XY Plane selection N1 G71 Metric mode N2 G40 CANCEL cutter radius compensation N3 G80 CANCEL canned cycle N4 G28 U0 W0 Incremental input ,Tool axis pullout N5 G91 Z0 Position to tool reference point N6 X0 Y0 N7 G92 Reset origin point N8 M06 T01 N9 G00 rapid travel to part zero N10 G90 X0 Y0 absolute programming N11 G43 Z0 M08 H01 tool length compensation N12 G00 X_ Y_ M03 S500 spindle ON N13 G01 Z_ F50 move tool downwards

General Structure of Milling Part Program . N21 G28 U0 V0 W0 TOOL AXIS PULLOUT N22 G91 Z0 N23 G28 RETURN TOOL TO HOME & SPINDLE OFF N24 G91 X0 Y0 M05 N25 G40 CANCEL CUTTER RADIUS COMPENSATION N26 G80 CANCEL CANNED CYCLE N27 G49 CANCEL TOOL LENGTH COMPENSATION N28 M09 COOLANT OFF N29 M02 N30 M30

Example: P.U. May 2007 N11 G43 Z0 M08 H01 TOOL LENGTH COMPENSATION N12 G00 X22 Y22 M03 S500 N13 G01 Z-2 F0.1 N14 G42 X25 D06 CUTTER RADIUS COMPENSATION-RIGHT N15 G01 X90 N16 Y40 N17 X75 N18 G02 X75 Y55 I00 J7.5 N19 G01 X90 N20 Y80 N21 G03 X75 Y95 I-15 J00 N22 G01 X55 N23 X25 Y75 N24 Y25 N25 G00 Z00

Example: P.U. May 2009 N11 G43 Z0 M08 H01 N12 G00 X30 Y30 M03 S500 N13 G01 Z-14 F0.1 N14 G00 Z02 M05 N15 G00 X90 Y30 M03 S500 N16 G01 Z-14 F0.1 N17 G00 Z02 M05 N18 G00 X90 Y70 M03 S500 N19 G01 Z-14 F0.1 N20 G00 Z02 M05 N21 G00 X30 Y70 M03 S500 N22 G01 Z-14 F0.1 N23 G00 Z02 M05 N24 G00 X0 Y0 M06 T02 N25 G43 Z2 M08 H01 N26 G00 X60 Y50 M03 S500 N27 G01 Z-14 F0.1 N28 G00 Z02 M05 N28 G00 Z00