Mill Toolpath Codes: Rapid, Linear Feed, and Circular Interpolation
Objective. Students write and simulate G00 rapid, G01 linear, G02/G03 circular interpolation blocks with correct I/J/K or R arc parameters to produce a defined 2D profile on a CNC mill simulator.
This lesson, its worked examples and its practice questions has not yet been verified by a licensed engineer or certified journey-level tradesperson or by a certification or approval body. It is a study draft and may contain errors. Do not use it as instructions for work on a job site or on live equipment. Always follow your instructor, your supervising professional, and current official references and regulations.
VoTechWorks program approval and accreditation are still in progress. Credentials are issued only by the certifying bodies named in each program, after their own exams.
Mill Toolpath Codes: Rapid, Linear Feed, and Circular Interpolation
Why These Three Codes Matter
Every CNC milling program you will ever write relies on three motion codes: G00 for rapid positioning, G01 for straight-line cutting, and G02/G03 for arc cutting. Master these and you can describe any 2D profile a drawing can specify. NIMS Machining Level 1 and 2 standards test your ability to write and verify exactly these blocks, so accuracy here pays off on the credential exam and on the shop floor.
Safety Before the Machine Moves
Before you run any program — even in simulation — build the habit of checking:
- Clearance plane. Your rapid moves must begin and end at a Z height that clears all clamps, fixtures, and workpiece features. A common choice is Z0.100 above the part top.
- Spindle state. In a real machine, the spindle must be running at the correct RPM before any cutting move (G01, G02, G03). A rapid move (G00) with a spinning tool that clips a clamp can break tooling or cause serious injury.
- Feed rate present. G01, G02, and G03 all require an active F-word. If you omit it, the control either alarms out or uses the last programmed feed — which may be dangerously fast.
- Lockout/tagout (LOTO). When you set up a physical machine — loading a tool, adjusting a work stop — the machine must be locked and tagged out per OSHA requirements. Simulation does not require LOTO, but the habit starts now.
- PPE. Safety glasses are required in the lab at all times. When observing a live machine, add hearing protection if the environment exceeds safe noise levels.
G00 — Rapid Positioning
G00 moves the tool from one point to another at the machine's maximum traverse rate. It is not a cutting move. Use it to position above the work before a cut and to retract after.
```
G00 G90 X1.500 Y0.750 Z0.100
```
- G90 sets absolute mode (coordinates measured from part zero).
- The tool moves simultaneously in X, Y, and Z. On most machines the axes do not move in a true straight line — they reach their target independently, so the path may be diagonal or angled. Never rapid into a part.
- Program rapid retracts to your clearance plane before any X/Y repositioning.
G01 — Linear Interpolation (Straight-Line Feed)
G01 moves in a precise straight line at the feed rate you specify with the F-word (inches per minute for milling in the US).
```
G01 X3.000 Y0.750 F10.0
```
The control calculates how fast each axis must move so they all arrive at the endpoint together, producing a true straight line. Change the F-word to change cutting speed — the path geometry does not change.
G02 and G03 — Circular Interpolation
G02 cuts a clockwise arc; G03 cuts a counterclockwise arc, both viewed from above (positive Z looking down at the XY plane).
You define the arc endpoint and either:
Method 1 — I/J offsets (recommended for precision):
```
G02 X2.500 Y1.000 I0.000 J0.500 F8.0
```
I and J are the distance from the arc start point to the arc center, measured in X and Y respectively. They are signed values (positive or negative). K is used instead of J when the arc is in the XZ or YZ plane.
Method 2 — R word (radius):
```
G02 X2.500 Y1.000 R0.500 F8.0
```
R is convenient for arcs less than 180°, but controls may interpret R differently for arcs greater than 180°, which can cause unexpected toolpath errors. I/J is safer for complex profiles.
Calculating I and J Values
Given:
- Arc start point: (2.000, 0.500)
- Arc center: (2.000, 1.000)
I = center X − start X = 2.000 − 2.000 = 0.000
J = center Y − start Y = 1.000 − 0.500 = +0.500
Always verify these values by hand before running a simulation. An incorrect I or J produces a spiral or alarm.
Building a Block Sequence
A complete motion sequence for a radiused corner looks like this:
```
N010 G00 G90 X1.000 Y0.000 Z0.100 (rapid to start position)
N020 G01 Z-0.250 F5.0 (plunge to depth)
N030 G01 X3.000 Y0.000 F10.0 (straight cut along X)
N040 G02 X3.500 Y0.500 I0.000 J0.500 F8.0 (CW arc, radius 0.500)
N050 G01 X3.500 Y2.000 F10.0 (straight cut up Y)
N060 G00 Z0.100 (retract)
```
Notice: the feed rate drops slightly for the arc (F8.0) — this is good practice to maintain surface finish on curves.
Verifying in CNCSimulator Pro
1. Enter your program and press Simulate.
2. Compare the on-screen toolpath against your printed 2D profile drawing.
3. Use the coordinate display to spot-check endpoint positions.
4. Overlay graph paper on the screen or print the simulation and trace it — this is exactly what the peer-review activity requires.
5. If a segment is wrong, go back to your I/J calculation before changing the code. Fix the math first, then fix the code.
Common Mistakes to Avoid
- Forgetting to cancel cutter compensation (G40) before arcs if compensation was active.
- Using G02 when the arc direction is actually counterclockwise (use G03).
- Leaving I and J at zero when they should not be — this commands a full circle on some controls.
- Mixing absolute and incremental mode without intention.
Key terms8
Worked examples4
- Identify the formula: I = Arc Center X − Arc Start X; J = Arc Center Y − Arc Start Y.
- Calculate I: 1.500 − 1.000 = +0.500.
- Calculate J: 2.000 − 2.000 = 0.000.
- Write the block: G02 X1.500 Y2.500 I0.500 J0.000 F8.0
- Calculate I: Arc Center X − Arc Start X = 0.500 − 0.500 = 0.000.
- Calculate J: Arc Center Y − Arc Start Y = 0.500 − 0.000 = +0.500.
- Verify radius: distance from center (0.500, 0.500) to start (0.500, 0.000) = sqrt((0.500−0.500)² + (0.500−0.000)²) = sqrt(0 + 0.25) = 0.500 in. ✓
- Write the block: G03 X0.000 Y0.500 I0.000 J0.500 F8.0
- Arc Center X = Start X + I = 4.000 + (−0.750) = 3.250.
- Arc Center Y = Start Y + J = 1.250 + 0.000 = 1.250.
- Arc Center = (3.250, 1.250).
- Radius = distance from center to start = sqrt((4.000−3.250)² + (1.250−1.250)²) = sqrt(0.5625 + 0) = 0.750 in.
- Verify using endpoint: distance from center (3.250, 1.250) to end (4.000, 2.000) = sqrt((4.000−3.250)² + (2.000−1.250)²) = sqrt(0.5625 + 0.5625) = sqrt(1.125) ≈ 1.061 in. This does NOT equal 0.750 in., indicating the endpoint is inconsistent with the I/J values — the program contains an error and would alarm on the control.
- Identify geometry: start = (2.500, 1.500), end = (3.000, 1.500), radius = 0.500 in., CW arc curving upward.
- Find arc center: midpoint of chord in X = (2.500 + 3.000)/2 = 2.750. Since radius = 0.500 and half-chord = 0.250, height from chord midpoint to center = sqrt(0.500² − 0.250²) = sqrt(0.25 − 0.0625) = sqrt(0.1875) ≈ 0.433 in. For a CW arc curving upward, center Y = 1.500 + 0.433 = 1.933 in. Center = (2.750, 1.933).
- Calculate I: 2.750 − 2.500 = +0.250.
- Calculate J: 1.933 − 1.500 = +0.433.
- Write I/J block: G02 X3.000 Y1.500 I0.250 J0.433 F8.0
The math in this lesson2
Materials: CNCSimulator Pro (PC lab); graph paper; arc-calculation worksheet; Smid CNC Programming Handbook Chapters 5–6; printed 2D profile drawing
Check: Simulated toolpath must match the 2D profile drawing within 0.005 in. on all features; arc center coordinates verified mathematically by instructor before simulation run; ≥80% of segments correct on peer-review overlay.
Practice check8
Answer each question, then check it. Nothing is recorded; this is your own practice.
