CNC Turning Program Walkthrough

Read the setup assumptions before the first block

Illustrative; check your control's manual. This is a reading example in a common Fanuc-style lathe dialect, not a machine-ready file. Read CNC Program Structure for blocks and modes, CNC Turning Setup and Offsets for offsets, and CNC Turning Spindle and Feed Modes for S and F. The mill simulator in G-code and Toolpaths cannot validate this lathe program.

The invented part is 20 mm in diameter and 25 mm long, with a 1 mm × 45° front chamfer. The chamfer runs from X18 Z0 to X20 Z−1: the 2 mm diameter change is a 1 mm radial change. Stock is 24 mm diameter with its raw face at Z+0.5. G54 has Z0 at the finished face and X0 on the spindle centreline. Stock and clearance extend beyond Z−28; workholding is farther toward negative Z.

Assume diameter programming and absolute X/Z endpoints; this dialect does not need G90 for absolute moves. T0101 selects station 1 and offset 1: a right-hand OD/facing tool with a 0.4 mm nose radius, suitable for the illustrated cuts. Its imaginary tip and radius are set, and G42 is the correct side for this setup's finish contour. T0202 selects a 2 mm wide cutoff tool and offset 2. Its Z reference is the edge toward positive Z, so Z−25 puts the blade in the interval Z−27 to Z−25. The cutoff tool is capable of the illustrated small travel past centre.

The example assumes X60 Z10 is an already-verified tool-change clearance location for both tools and the turret sweep, and starts there with spindle and coolant off. These coordinates are not a general clearance rule. All speeds, feeds and the 1800 RPM ceiling are teaching values, not material recommendations. Verify the real setup, tool calls, compensation entry/exit, centre crossing and file delimiters using CNC Programming and Prove-Out and the Safety collection.

Face the end, then leave a small allowance on the outside diameter

Every parenthesized comment explains its block. G01 remains active until G00 replaces it; X/Z values here are destinations. Facing travels slightly past the centre to account for the rounded nose. Roughing uses two explicit lengthwise passes rather than a control-specific canned-cycle format.

O2460 (IDENTIFY THIS EXAMPLE PROGRAM)
G18 G21 G40 G80 G99 (XZ PLANE, MM, COMP OFF, CYCLES OFF, MM/REV)
G54 (SELECT THE PRESET PART WORK OFFSET)
T0101 (SELECT OD TOOL 1 WITH OFFSET 1 AT VERIFIED CLEARANCE)
G50 S1800 (SET THE EXAMPLE MAXIMUM SPINDLE RPM)
G97 S600 M03 (FIXED 600 RPM, START SPINDLE IN SETUP DIRECTION)
G00 X26.0 (APPROACH OUTSIDE THE 24 MM STOCK AT Z10)
G00 Z0.0 (MOVE TO FINISHED FACE PLANE WHILE OUTSIDE STOCK)
M08 (TURN ON THE ASSUMED FLOOD COOLANT SYSTEM)
G96 S90 (SELECT 90 M/MIN CSS WITH THE RPM CEILING ACTIVE)
G01 X-0.8 F0.10 (FACE THROUGH CENTRE: 0.4 MM RADIAL OVERTRAVEL)
G00 Z2.0 (RETRACT AXIALLY BEYOND THE FACED END)
G00 X22.0 (POSITION FOR THE FIRST OD ROUGHING PASS IN AIR)
G01 Z-28.0 F0.20 (ROUGH LENGTHWISE TO 22 MM DIAMETER)
G00 X26.0 (RETRACT RADIALLY OUTSIDE THE ORIGINAL STOCK)
G00 Z2.0 (RETURN TO THE FRONT AT CLEAR X)
G00 X20.6 (POSITION FOR THE SECOND OD ROUGHING PASS)
G01 Z-28.0 F0.20 (LEAVE 0.6 MM ON DIAMETER FOR FINISHING)
G00 X26.0 (RETRACT OUTSIDE STOCK AGAIN)
G00 Z2.0 (RETURN AHEAD OF THE FACE FOR FINISHING)

Compensate the chamfer and finish, then cut off at fixed RPM

The finish contour uses the same tool at a smaller feed. Nose compensation is active for the chamfer and OD; it is entered ahead of the face and cancelled after departing the finished contour. See CNC Turning Profiles and Cycles for why a sharp-point assumption would give the wrong chamfer.

G00 X16.0 (POSITION AHEAD OF THE FACE FOR THE COMPENSATED ENTRY)
G01 G42 X18.0 Z0.0 F0.10 (ENGAGE RIGHT COMP ON THE FACE APPROACH)
G01 X20.0 Z-1.0 (CUT THE 1 MM RADIAL BY 1 MM AXIAL CHAMFER)
G01 Z-26.0 (FINISH THE 20 MM OD PAST THE CUTOFF FACE)
G01 X22.0 Z-27.0 (FEED OUT FROM THE OD BEHIND THE FINISHED PART)
G01 G40 X26.0 (CANCEL COMPENSATION ON THE OUTWARD DEPARTURE)
G97 S600 (CANCEL CSS AND REQUEST FIXED 600 RPM)
G00 X60.0 (RETRACT RADIALLY TO THE ASSUMED CLEARANCE X)
G00 Z10.0 (RETURN AXIALLY TO THE VERIFIED TOOL-CHANGE LOCATION)
M09 (COOLANT OFF)
M05 (STOP THE SPINDLE BEFORE THE TOOL CHANGE)
T0202 (SELECT CUTOFF TOOL 2 AND ITS EDGE-REFERENCED OFFSET 2)
G97 S500 M03 (START AT FIXED 500 RPM FOR THIS CUTOFF EXAMPLE)
G00 X26.0 (POSITION OUTSIDE THE STOCK WITH THE NEW TOOL)
G00 Z-25.0 (LOCATE THE POSITIVE-Z BLADE EDGE AT THE REAR FACE)
M08 (COOLANT ON)
G01 X-0.2 F0.05 (PART OFF WITH THE ASSUMED 0.1 MM RADIAL OVERTRAVEL)
G00 X60.0 (WITHDRAW RADIALLY FROM THE CUTOFF SLOT)
G00 Z10.0 (RETURN TO THE ASSUMED CLEARANCE Z)
M09 (COOLANT OFF)
M05 (SPINDLE STOP)
M30 (END AND RESET THE PROGRAM; NO RETURN MOVE IS IMPLIED)

File-start/end percent delimiters, tool-call behavior and supported startup codes must be supplied or adapted as required by the target control. No bar-feeder or parts-catcher sequence is implied.