G2 & G3: Circular Interpolation Explained – Mastering Arcs in CNC

G2 & G3: Circular Interpolation Explained – Mastering Arcs in CNC

In CNC programming, G2 and G3 are used to generate circular or arc movements in the currently active plane (set by G17, G18, or G19). These commands are essential for smooth contouring, circular pockets, threads, and more.

---

🌀 What Are G2 and G3?

G-Code	Motion	Direction
G2	Circular Move	Clockwise (CW)
G3	Circular Move	Counterclockwise (CCW)

---

🧭 Arc Movement Parameters

You can define arcs in two main formats:

🔸 R Format (Radius)

G2 X50 Y50 R25

• Simple and easy to use
• Radius (R) defines the arc curvature
• May cause ambiguity with arcs >180°

🔹 IJK Format (Center Offset)

G3 X50 Y50 I25 J0

• More precise and reliable
• I, J, K define distance from start point to arc center
• I and J are used in G17 (XY plane)
• I and K are used in G18 (XZ plane)
• J and K in G19 (YZ plane)

---

🧪 Example: G17 Plane (XY)

G17               ; XY plane active
G0 X25 Y0
G2 X25 Y50 I0 J25 ; CW arc from Y0 to Y50 with center at Y25

This moves in a clockwise quarter-circle.

---

📐 Visual Explanation (IJK)

• Start point: (25, 0)
• End point: (25, 50)
• Center point: (25, 25)

So:

• I = 0 (center X – start X)
• J = 25 (center Y – start Y)

---

⚠️ Arc Direction Depends on Plane

Make sure you select the correct plane (G17/G18/G19) before programming arcs.

G-Code	Plane	Active Axes	IJK Components
G17	XY	X/Y	I, J
G18	XZ	X/Z	I, K
G19	YZ	Y/Z	J, K

---

🔧 Real-World Example: Milling a Circular Pocket

%
O3001 (Circular Pocket)
G21 G90 G17
T1 M6
G0 X0 Y0
G43 H1 Z100
S1200 M3

G0 Z5
G1 Z-5 F200
G2 X0 Y0 I10 J0 F300 ; Clockwise arc with 10mm radius
G1 Z100
M30
%

---

🔁 G2/G3 with Full Circles

To create a full circle using IJK:

G3 X0 Y0 I10 J0 ; Start and end at same point

Note: This must be supported by the controller. Some require splitting into two semicircles.

---

📊 G2/G3 Syntax Comparison

Format	Syntax	Pros	Cons
R	G2 X.. Y.. R..	Easy to write/read	Ambiguity in >180° arcs
IJK	G3 X.. Y.. I.. J..	Precise control	Requires vector math

---

🧠 Tips for CAM Integration

• CAM software often outputs IJK format, especially for 3D surfaces
• Post-processors allow choosing between R or IJK
• Always double-check the arc direction when editing CAM output manually

---

🛡️ Common Mistakes

Issue	Likely Cause	Solution
Tool moves in wrong arc	Wrong G2/G3 or wrong IJK sign	Reverse G2 ↔ G3 or correct signs
Arc creates unexpected shape	Wrong plane selected (G17/G18/G19)	Set correct plane before arc
Arc goes straight or error	IJK values not matching arc radius	Check vector math or use R format
Full circle not accepted	Controller doesn’t support full arc	Split into 2 semi-circles

---

🔧 Advanced: Helical Interpolation

You can combine G2/G3 with Z-axis motion for helical paths (e.g., thread milling):

G3 X0 Y0 Z-5 I10 J0

This moves in a descending spiral, excellent for boring or threading.

---

📐 How to Calculate IJK Values

Assume:

• Start: (X0 Y0)
• End: (X50 Y0)
• Arc center at (X25 Y25)

So:

• I = 25 (center X – start X)
• J = 25 (center Y – start Y)

G3 X50 Y0 I25 J25

---

🔚 Final Thoughts

Mastering G2 and G3 unlocks powerful contouring capabilities in CNC. Understanding the relationship between arc direction, plane selection, and IJK vs R formatting is essential.

Arcs may look simple, but precision demands clarity. Think like the controller.