TOOLBOX · CNC & MACHINING · VISUAL TOOLPATH
Use this free lathe backplotter and CNC program checker to paste or write G-code and visualise the X/Z toolpath before running it on the machine. X is interpreted as a diameter value; Z is the spindle-length axis.
✓ No basic parser warnings found.
G00 RAPIDG01 LINEARG02 CW ARCG03 CCW ARCG20 INCHG21 METRICG90 ABSOLUTEG91 INCREMENTALG94 PER MING95 PER REVU/W INCREMENTALR + I/K ARCSCommon N, O, T, S, F and M words plus parenthetical and semicolon comments are handled without creating false motion. G18 is the assumed XZ plane.
G71 ROUGHINGG72 FACINGG74 PECKG75 GROOVINGG76 THREADINGThese blocks are skipped and reported by line instead of displaying a guessed toolpath. Expand cycles into explicit moves for a visual preview.
PRACTICAL PROGRAM CHECKING
This free browser-based tool turns common two-axis turning moves into an immediate visual check. It is designed to help machinists and CNC programmers understand programmed motion before moving to the control, not to replace the machine’s own graphics and prove-out process.
Paste a lathe program into the editor and the simulator reads supported X and Z moves, plots the path and shows the active block, tool position, motion mode and feed information. Use playback, single-step controls or the complete toolpath view to inspect the sequence.
The display treats X as the diameter or radial axis and Z as the spindle-length axis. The stock outline and X0 Z0 reference make it easier to spot a move on the wrong side of the component, an unexpected retract or an incorrect sign.
G00 rapid moves appear as dashed grey lines. G01 linear feed moves are orange, while G02 and G03 arcs use a lighter orange path. This visual separation helps reveal where the tool approaches, cuts and retracts.
The current simulator handles G00, G01, G02 and G03 motion; G20 and G21 units; G90 and G91 positioning; G94 and G95 feed modes; U/W incremental moves; and supported R or I/K arc definitions. N, O, T, S, F and common M words can remain in the program without creating false movement.
CHECKING WORKFLOW
Paste the program. Keep the original line numbers and comments so warnings are easy to trace.
Set the stock. Enter a practical diameter and length so the path has useful scale and context.
Read the warnings. Review unsupported cycles, mixed units and incomplete or unusual blocks.
Step through motion. Check rapids, feed direction, approach moves, retracts, arcs and the final safe position.
Verify at the control. Confirm offsets, compensation, tooling and clearances, then use machine graphics, single block, feed override and a safe dry run.
EXAMPLE CNC LATHE PROGRAMS
Use the built-in example buttons above to load these programs directly into the simulator. Explicit G00, G01, G02 and G03 moves are the clearest way to review motion online.
Metric absolute positioning with facing, an outside profile and a safe retract.
(EHQ LATHE SIM EXAMPLE)
G21
G90
G0 X52 Z5
G0 Z1
G1 Z0 F0.2
G1 X0
G0 X52 Z2
G1 X50 Z0
G1 Z-30
G1 X40 Z-35
G1 Z-50
G0 X60 Z10
M30G02 centre-offset arc motion in the standard G18 X/Z plane.
%
(ENGINEERS HQ ARC PROFILE DEMO)
G21 G18 G90 G95
G50 S2500
T0101
G97 S1200 M3
G0 X42 Z3
G96 S180
G1 Z0 F0.20
G1 X-1.0
G0 X38 Z2
G1 Z0 F0.18
G1 X40 Z-1
G1 Z-18
G2 X34 Z-21 I-3 K0
G1 X30 Z-21
G1 Z-35
G0 X60 Z10
M5
M30
%