CNC G02/G03
Circular Interpolation
Understand clockwise and counterclockwise interpolation, I/J/K centre offsets, R-radius programming, interpolation planes, cutter compensation, toolpath geometry, troubleshooting and inspection.
G02 and G03 are CNC circular interpolation commands. They tell the CNC control to coordinate machine-axis movement along a circular path between programmed points. Correct programming requires the programmer to understand the start point, endpoint, arc centre or radius, active interpolation plane and the relationship between cutter motion and finished part geometry.
G02 / G03 at a Glance
What Are G02 and G03?
G02 and G03 are used to command circular interpolation on CNC machines. Instead of moving between two coordinates using a straight-line G01 move, the CNC control coordinates the machine axes to follow an arc.
The commands are widely used for circular pockets, bosses, bores, radii, contours, interpolation of holes and other machined features containing circular geometry.
G02
Clockwise circular interpolation.
G02 X40. Y20. I10. J0. F200G03
Counterclockwise circular interpolation.
G03 X40. Y20. I10. J0. F200How Circular Interpolation Works
A circular path can be mathematically represented using its centre and radius.
X and Y represent a point on the circle. Xc and Yc represent the centre coordinates and R represents the radius.
The CNC programmer normally does not enter this equation directly. Instead, the controller receives the required endpoint and information defining the circular geometry.
Important: Always establish whether the programmed radius describes the finished part geometry or the centreline of the cutting tool. These are not necessarily the same radius.
G02 vs G03: Understanding Direction
G02 commands clockwise circular interpolation while G03 commands counterclockwise circular interpolation.
The direction must be interpreted relative to the active interpolation plane and machine coordinate system. This is particularly important when machining features in different orientations.
| Command | Meaning | Engineering Check |
|---|---|---|
| G02 | Clockwise circular interpolation | Verify direction relative to active plane |
| G03 | Counterclockwise circular interpolation | Verify direction relative to active plane |
G17, G18 and G19 Circular Interpolation Planes
The CNC control needs to know which two axes define the circular interpolation plane.
| Code | Plane | Circular Axes | Centre Offsets |
|---|---|---|---|
| G17 | XY | X / Y | I / J |
| G18 | XZ | X / Z | I / K |
| G19 | YZ | Y / Z | J / K |
Shop-floor check: Before troubleshooting an arc, verify the active interpolation plane. A correct I/J calculation will not produce the intended path if the control is working in a different plane.
Programming G02/G03 Using I, J and K
I, J and K define the position of the arc centre relative to the starting point of the circular move.
Example in the G17 XY Plane
Worked Example
Suppose the tool starts at:
X20. Y10.The arc centre is located at:
X40. Y30.Therefore:
I = 40 − 20 = +20
J = 30 − 10 = +20The centre offsets are:
I20. J20.Programming Circular Arcs Using R
R-format programming defines the radius of the programmed arc rather than explicitly defining its centre using I/J/K.
G03 X40. Y20. R20. F250R programming can be convenient for simple radius-defined arcs. However, long arcs and controller-specific conventions require careful verification.
Controller-specific behaviour: Always verify the R-format convention in the programming manual for the specific CNC control.
IJK vs R Programming
| Method | Advantages | Considerations |
|---|---|---|
| I / J / K | Explicit centre definition and useful for complex arcs and full circles. | Requires centre-offset calculation. |
| R | Compact and convenient for simple radius-defined arcs. | Long arcs and controller conventions require care. |
Programming a Full 360° Circle
A full circle returns to the starting coordinate. Centre-format programming is commonly used for this type of motion where supported by the CNC control.
G17
G02 I-20. J0. F200The exact syntax should always be verified against the machine control manual because controller implementations can differ.
Helical Interpolation
Circular interpolation can be combined with simultaneous movement along the axis perpendicular to the circular plane. This creates a helical toolpath.
G17
G03 X20. Y0. I-20. J0. Z-5. F150Here the cutter follows a circular path in the XY plane while simultaneously moving in Z.
Helical interpolation can be used for applications such as large-hole interpolation, circular ramps, boring strategies and thread milling.
Toolpath Geometry vs Finished Part Geometry
One of the most important concepts in CNC circular interpolation is understanding that the programmed cutter centreline may not have the same radius as the finished feature.
Finished Feature
Consider an internal circular pocket:
Finished diameter = Ø50 mm
Finished radius = 25 mmCutter Centreline
Assume a Ø10 mm cutter:
Tool radius = 5 mm
Toolpath radius = 25 − 5
= 20 mmKey question: When calculating the arc, are you describing the finished part radius or the cutter centreline radius?
Tooling, Workholding and Setup
Correct G02/G03 programming cannot compensate for an unstable machining setup.
| Factor | Why It Matters |
|---|---|
| Tool diameter | Influences the minimum achievable internal radius. |
| Tool stickout | Longer tools are generally more susceptible to deflection. |
| Spindle runout | Can influence actual material removal and dimensional consistency. |
| Workholding | Poor rigidity can create vibration and dimensional variation. |
| Work offset | Incorrect G54/G55 positioning can shift the entire feature. |
Read the related CNC Setup Planning Guide and CNC Workholding Guide .
Cutting Parameters for Circular Interpolation
G02 and G03 define the motion path. They do not automatically determine the correct cutting speed or feedrate.
| Variable | Influence |
|---|---|
| Material | Influences machinability and cutting behaviour. |
| Tool diameter | Influences engagement and rigidity. |
| Tool geometry | Influences chip formation and cutting load. |
| Radial engagement | Influences cutting force and heat generation. |
| Axial depth | Influences cutting load and deflection. |
n = spindle speed in rpm
Vc = cutting speed in m/min
D = tool diameter in mm
Inspection of Circular Features
A circular feature can meet its nominal diameter while still having problems with circularity, position, surface finish, burrs or other drawing requirements.
| Requirement | Potential Inspection Method |
|---|---|
| General diameter | Appropriate calibrated dimensional instrument |
| Precision bore | Bore gauge |
| Small controlled hole | Pin gauge where appropriate |
| Feature location | Height gauge, probing or CMM |
| Circularity / form | Appropriate form measurement or CMM |
| Surface roughness | Surface roughness measurement equipment |
See the CNC Inspection Guide for the broader inspection process.
G02/G03 Troubleshooting Guide
| Problem | Possible Cause | Check | Action |
|---|---|---|---|
| Arc travels wrong direction | Incorrect G02/G03 | Check start point and direction | Recalculate arc direction |
| Arc alarm | Invalid geometry | Check centre and endpoint | Correct I/J/K or R |
| Wrong diameter | Toolpath or compensation issue | Verify cutter diameter | Correct toolpath or offset |
| Feature shifted | Incorrect work offset | Check G54/G55 | Re-establish work coordinate |
| Poor circular finish | Vibration, deflection or runout | Inspect tool and setup | Improve rigidity and cutting conditions |
| Batch size variation | Tool wear or thermal variation | Track feature size | Implement tool-life and offset control |
Related troubleshooting resources: CNC Chatter | CNC Tool Wear | CNC Tool Deflection
DFM Considerations for Circular Features
Circular geometry is usually straightforward to machine, but certain combinations of radius, depth, tolerance and material can significantly affect the process.
Internal Radius
Very small internal radii may require small cutters, increasing tool deflection and machining time.
Feature Depth
Deep circular features may require longer tools and can increase the risk of vibration.
Tolerance
Tight diameter and form tolerances may require dedicated finishing and inspection strategies.
Inspection
The drawing should specify requirements that can be practically verified using an appropriate inspection method.
For broader drawing interpretation, see the CNC Machining Drawing Guide and GD&T for CNC Machining .
How Circular Interpolation Affects CNC Cost
The ability to generate a circular feature is only one part of process planning. Cycle time, tooling, inspection and setup requirements all influence the production economics.
| Cost Driver | Potential Impact |
|---|---|
| Cycle time | Longer toolpaths increase machining time. |
| Tooling | Small or specialised cutters can increase tooling cost. |
| Setups | Additional orientations increase setup time. |
| Inspection | Tight form requirements can require advanced measurement. |
| Scrap | Incorrect arc geometry can produce dimensional failures. |
Related: CNC Machining Cost and How to Reduce CNC Machining Cost .
Worked CNC Circular Interpolation Example
Consider an internal circular pocket with the following requirements:
| Requirement | Value |
|---|---|
| Finished pocket diameter | Ø50 mm |
| Pocket depth | 10 mm |
| Cutter diameter | Ø10 mm |
Finished feature radius:
25 mmCutter radius:
5 mmTherefore, the cutter centreline follows a nominal Ø40 mm path to generate the Ø50 mm internal feature.
G02/G03 Shop-Floor Checklist
G02/G03 CNC Programming FAQ
What is G02 in CNC?
G02 commands clockwise circular interpolation relative to the active interpolation plane.
What is G03 in CNC?
G03 commands counterclockwise circular interpolation relative to the active interpolation plane.
What do I and J mean in CNC?
In the common G17 XY plane, I represents the X-direction centre offset and J represents the Y-direction centre offset from the arc start point.
What is R in G02/G03?
R specifies the radius of the programmed arc. Detailed interpretation can vary between CNC controllers.
Can G02/G03 create a full circle?
Yes, where the CNC control supports full-circle centre-format interpolation.
What is G17?
G17 selects the XY interpolation plane.
What is G18?
G18 selects the XZ interpolation plane.
What is G19?
G19 selects the YZ interpolation plane.
Why can an R arc produce an unexpected path?
The programmed endpoint and radius can define different arc geometries. Long arcs and controller-specific conventions require particular care.
CNC Machining Knowledge Hub
G02/G03 circular interpolation is one part of the wider CNC programming, machining and inspection workflow. Continue learning through the related Manufyn technical resources below.
CNC G01 Linear Interpolation
Understand feed-controlled linear movement before moving into circular interpolation.
Read G01 Guide →How to Read a CNC Drawing
Understand dimensions, datums and manufacturing intent before programming.
Read Drawing Guide →CNC Tool Deflection
Understand how tool deflection affects circular feature accuracy.
Read Tool Deflection →From CNC Programming to Real Manufacturing
CNC programming is only one part of a successful machining process. Drawing interpretation, setup planning, workholding, tool selection, inspection and process control all influence the final component.
CNC Manufacturing Case Studies
Explore real manufacturing projects and engineering challenges.
24 Hour CNC Turning Prototype →
Engineering Blogs
Connect CNC programming with broader manufacturing engineering and DFM topics.
Design for Manufacturability →
Have a CNC Drawing to Review?
If you are developing a component and need to understand the machining approach, tooling, tolerances or manufacturing requirements, Manufyn can review the requirement.
Discuss a Manufacturing Requirement