The Ultimate CNC G-Code Examples & Programming Library 2026 — FANUC, Haas, Milling, Turning, Drilling, Tapping, Macros and M98/M99 Programs

THE ULTIMATE CNC G-CODE EXAMPLES & PROGRAMMING LIBRARY 2026

FANUC, Haas, CNC Milling, Turning, Drilling, Tapping, Subprograms, Macro B and Professional CNC Programming Examples

The Complete CNC Program Examples, G-Code Reference and Practical Programming Guide

Welcome to the Ultimate CNC G-Code Examples & Programming Library 2026.

This reference is designed for CNC operators, programmers, machinists, manufacturing engineers, students, and technicians who want to understand CNC programming through practical examples.

Instead of memorizing isolated commands, you will learn how G-codes, M-codes, coordinates, offsets, cutting parameters, subprograms, and macro logic work together.

Inside this library, you will find examples covering:

• CNC milling
• CNC drilling
• Peck drilling
• Tapping
• Circular interpolation
• Slot milling
• Rectangular profiles
• Tool length compensation
• Work coordinate systems
• Subprograms
• FANUC-style Macro B
• Bolt-circle calculations
• CNC turning
• Spindle speed modes
• Professional programming practices
• Common programming errors
• Program verification

Important: Read Before Using Any Example

The programs in this guide are educational examples, not production-ready machine programs.

Most milling examples use common FANUC-style ISO conventions. Some commands are shared with Haas controls, but compatibility must be checked against the exact machine.

The turning examples use general FANUC-style concepts. Turning cycles and formats differ significantly by controller and series.

Every example requires verification of:

• Controller model and software
• Installed control options
• Machine configuration
• Axis travel and direction
• Tooling and tool offsets
• Workholding and fixtures
• Stock dimensions
• Work coordinate system
• Feedrates and spindle speeds
• Toolpath clearance
• Collision risk
• Machine-specific M-codes

Before any physical execution, use an appropriate controller-aware simulator, verify the setup, and follow your machine’s approved prove-out procedure.

Never copy an unfamiliar CNC program directly into a production machine and press Cycle Start.

PART I — CNC PROGRAMMING FOUNDATIONS

SECTION 1 — BASIC CNC PROGRAM STRUCTURE

A CNC program typically contains:

1. Program identification
2. Initial modal-state commands
3. Work coordinate selection
4. Tool selection
5. Spindle commands
6. Tool length compensation
7. Positioning
8. Cutting operations
9. Retraction
10. Program termination

Example 1 — Basic FANUC-Style Milling Program

%

O1001 (BASIC MILLING EXAMPLE)

G21 G17 G90 G40 G49 G80

G54

T01 M06

S1500 M03

G00 X10. Y10.

G43 H01 Z50.

M08

G01 Z-2. F100.

G01 X60. F250.

G00 Z50.

M09

M05

M30

%

Explanation

O1001 identifies the program.

G21 selects metric units.

G17 selects the XY plane.

G90 selects absolute positioning.

G40 cancels cutter radius compensation.

G49 cancels tool length compensation.

G80 cancels canned cycles.

G54 selects a work coordinate system.

T01 M06 requests a tool change on compatible machines.

S1500 M03 requests clockwise spindle rotation at 1500 RPM.

G00 performs rapid positioning.

G43 H01 activates the designated tool length compensation.

M08 activates coolant on compatible machines.

G01 performs feed-controlled linear interpolation.

M30 ends the program.

Important: This example assumes the programmed coordinates, tool length, stock, and fixture clearances have been independently verified. Its startup and retract sequence is not a universal safe-start template.

SECTION 2 — G00 RAPID POSITIONING

G00 is used for rapid positioning.

Example 2

G90 G00 X50. Y25.

This commands positioning to X50 and Y25 in the active coordinate system.

The exact rapid trajectory may depend on the controller and machine.

Professional note: A safe destination does not guarantee a safe rapid path.

SECTION 3 — G01 LINEAR INTERPOLATION

G01 moves an axis or multiple axes at a programmed feedrate.

Example 3

G90 G01 X80. Y20. F300.

The tool moves toward X80 Y20 at a programmed feedrate of 300 units per minute when the active feed mode is feed per minute.

The actual units depend on the unit-selection mode.

SECTION 4 — G02 CLOCKWISE ARC

G02 commands clockwise circular interpolation in the selected plane.

Example 4 — Quarter-Circle Arc

Assumptions:

• XY plane active
• Incremental arc-center offsets supported
• Starting point X10 Y0
• Arc center X0 Y0

G17 G90

G00 X10. Y0.

G03 X0. Y10. I-10. J0.

This example uses G03, not G02, because the movement from the positive X axis toward the positive Y axis is counterclockwise.

To move clockwise from X0 Y10 to X10 Y0:

G02 X10. Y0. I0. J-10.

This distinction is important when troubleshooting arc direction.

SECTION 5 — G03 COUNTERCLOCKWISE ARC

Example 5

G17 G90

G00 X10. Y0.

G03 X0. Y10. I-10. J0.

The example describes a quarter-circle arc with a radius of 10 units.

Verify the controller’s arc-center convention before use.

SECTION 6 — G90 ABSOLUTE POSITIONING

G90 commands absolute positioning on many milling controls.

Example 6

G90

G01 X10. F200.

X20.

X30.

The programmed X destinations are:

10

20

30

Each coordinate refers to the active coordinate system’s origin.

SECTION 7 — G91 INCREMENTAL POSITIONING

G91 commands incremental positioning.

Example 7

G91

G01 X10. F200.

X10.

X10.

G90

Each X10 move adds 10 units to the current X position.

The final G90 restores absolute positioning.

Professional shortcut: Explicitly restore the positioning mode expected by the calling program.

SECTION 8 — G54 WORK COORDINATE SYSTEM

G54 commonly selects a work coordinate system.

Example 8

G90 G54

G00 X0. Y0.

The destination is X0 Y0 in the G54 coordinate system.

Its physical machine location depends on the stored work offset.

SECTION 9 — G55 SECOND WORK OFFSET

Example 9

G90 G55

G00 X0. Y0.

G55 can reference a different work setup or fixture location.

Common application

Machine identical parts at separate fixture locations using different work offsets.

The work offsets must be measured and verified.

SECTION 10 — G43 TOOL LENGTH COMPENSATION

Example 10

G90 G00 X20. Y20.

G43 H01 Z50.

On compatible controls, G43 activates positive tool length compensation using the selected H offset.

Incorrect tool length data can create serious collision hazards.

PART II — CNC DRILLING PROGRAM EXAMPLES

SECTION 11 — G81 SIMPLE DRILLING

Example 11 — Three-Hole Drilling Pattern

%

O1101 (G81 DRILLING)

G21 G17 G90 G40 G49 G80

G54

T01 M06

S1200 M03

G00 X10. Y10.

G43 H01 Z50.

M08

G98 G81 Z-12. R3. F120.

X30. Y10.

X50. Y10.

G80

G00 Z50.

M09

M05

M30

%

What this example demonstrates

The first G81 block defines the drilling cycle.

The following XY positions repeat the drilling operation.

G80 cancels the cycle.

On many FANUC-style mills, G98 selects return to the initial level during a canned cycle. Verify the exact machine’s behavior and initial level before use.

SECTION 12 — G82 DWELL DRILLING

G82 adds a dwell at the bottom of a drilling cycle on many compatible controls.

Example 12

G90 G98 G82 X20. Y20. Z-8. R3. P1000 F100.

G80

Controller note: The units and interpretation of the P dwell parameter vary by controller and programming format. Do not assume P1000 always means one second.

SECTION 13 — G83 PECK DRILLING

G83 is commonly used for deeper holes where chip evacuation is important.

Example 13

G90 G98 G83 X20. Y20. Z-30. R3. Q5. F120.

G80

Common FANUC-style interpretation:

Z-30. — Final depth

R3. — R plane

Q5. — Peck increment

F120. — Feedrate

Peck behavior, retract behavior, and supported parameters depend on the controller.

SECTION 14 — MULTIPLE G83 HOLES

Example 14

G90 G98 G83 X10. Y10. Z-25. R3. Q4. F100.

X30. Y10.

X50. Y10.

X70. Y10.

G80

This pattern avoids repeating the full drilling-cycle definition for every hole.

The actual toolpath must be checked for fixture and stock clearance.

SECTION 15 — G84 TAPPING

G84 is commonly associated with tapping cycles.

Example 15 — Metric Pitch Calculation

Assume:

Thread pitch = 1.5 mm

Spindle speed = 500 RPM

For feed-per-minute tapping:

Feed = Pitch × RPM

Feed = 1.5 × 500 = 750 mm/min

Illustrative cycle:

G90 G84 X20. Y20. Z-15. R3. F750.

G80

Important: This is not a complete machine-ready rigid-tapping program. Spindle synchronization, required modes, speed commands, feed conventions, and cycle syntax are controller-specific.

SECTION 16 — G73 HIGH-SPEED PECK DRILLING

Some FANUC-style milling controls support G73 as a chip-breaking or high-speed peck-drilling cycle.

Example 16

G90 G73 X20. Y20. Z-18. R3. Q3. F150.

G80

G73 behavior can differ from G83.

Check the official cycle description for your control.

SECTION 17 — LINEAR HOLE PATTERN

Suppose five holes are spaced 20 mm apart.

Starting X = 10 mm.

The positions are:

10

30

50

70

90

Example 17

G90 G98 G81 X10. Y20. Z-10. R3. F100.

X30.

X50.

X70.

X90.

G80

This is a compact approach to repeated drilling.

SECTION 18 — RECTANGULAR HOLE PATTERN

A four-corner hole pattern can be programmed with four positions.

Example 18

G90 G98 G81 X10. Y10. Z-10. R3. F100.

X70. Y10.

X70. Y50.

X10. Y50.

G80

The example demonstrates coordinate reuse within a modal drilling cycle.

PART III — MILLING GEOMETRY EXAMPLES

SECTION 19 — STRAIGHT SLOT CENTERLINE

Example 19

G90 G01 X10. Y20. F250.

X90. Y20.

This represents a straight tool-center movement.

It does not define a complete slot machining process.

Actual slot width depends on tool diameter and cutting strategy.

SECTION 20 — RECTANGULAR TOOLPATH

Example 20

G90 G01 X10. Y10. F250.

X90. Y10.

X90. Y60.

X10. Y60.

X10. Y10.

This describes a rectangular tool-center path.

Important: It is not automatically a finished rectangular part contour. Cutter diameter, compensation, depth, lead-in, stock, and fixture conditions must be accounted for.

SECTION 21 — SQUARE PROFILE

Example 21

G90 G01 X0. Y0. F200.

X50. Y0.

X50. Y50.

X0. Y50.

X0. Y0.

The tool-center path forms a 50 × 50 square.

This is useful for learning coordinate programming.

SECTION 22 — CIRCULAR CONTOUR USING TWO ARCS

Assume the starting point is X10 Y0 and the intended circle center is X0 Y0.

Example 22

G17 G90

G00 X10. Y0.

G03 X-10. Y0. I-10. J0.

G03 X10. Y0. I10. J0.

This describes a full circle using two semicircular moves.

Actual machining requires appropriate tool engagement, depth control, and compensation.

SECTION 23 — SPIRAL TOOLPATH CONCEPT

A spiral milling strategy gradually changes the radial position as the tool rotates around a center.

Conceptually:

Radius = Initial Radius + Growth Per Revolution

X = Center X + Radius × COS(Angle)

Y = Center Y + Radius × SIN(Angle)

The path may be generated by CAM or a controller-supported macro.

Spiral machining requires attention to tool engagement, interpolation capability, and stock removal.

SECTION 24 — HELICAL INTERPOLATION CONCEPT

Helical interpolation combines circular movement with axial movement.

A conceptual example:

G17

G03 X-10. Y0. I-10. J0. Z-1.

G03 X10. Y0. I10. J0. Z-2.

Assumptions:

• The first arc begins at X10 Y0
• Arc-center offsets are incremental
• The controller supports simultaneous circular and Z interpolation

This is a geometric illustration only, not a complete helical-boring routine.

SECTION 25 — FACE MILLING PATTERN

A basic raster face-milling strategy moves across a surface in parallel passes.

Concept:

PASS 1 — X positive

STEP OVER — Y positive

PASS 2 — X negative

STEP OVER — Y positive

PASS 3 — X positive

The stepover depends on tool diameter, engagement, surface-finish requirements, and material.

A complete production routine should be generated or verified for the actual tool and stock.

SECTION 26 — Z-LEVEL ROUGHING

Z-level roughing removes material at multiple depths.

Example depth sequence:

Z = -2 mm

Z = -4 mm

Z = -6 mm

Z = -8 mm

This approach can be used for pockets and contours.

The correct depth per pass depends on the tool, material, machine rigidity, and cutting strategy.

SECTION 27 — FINISHING ALLOWANCE

Professional programs often separate roughing from finishing.

Example:

Target wall position = X50.000

Roughing allowance = 0.300 mm

Finishing pass removes the remaining allowance.

The actual roughing tool-center position depends on which side of the wall is machined and whether cutter compensation is used.

PART IV — CNC SUBPROGRAM EXAMPLES

SECTION 28 — M98 SUBPROGRAM CALL

On many FANUC-style controls, M98 calls a subprogram.

Example 28 — Main Program

%

O1200 (MAIN PROGRAM)

G21 G17 G90 G40 G49 G80

G54

T01 M06

S1000 M03

G00 X20. Y20.

G43 H01 Z50.

M98 P2000

M05

M30

%

Subprogram

%

O2000 (SUBPROGRAM)

G90 G00 Z10.

G01 Z-2. F100.

G01 X40. F200.

G00 Z50.

M99

%

Explanation

The main program calls O2000.

The subprogram executes its movements.

M99 returns control to the caller on compatible controls.

Important: The subprogram assumes a specific tool, spindle, work offset, entry position, and verified clearances. The example demonstrates call structure rather than a validated machining operation.

SECTION 29 — M98 REPEAT COUNT

Some FANUC-style controls allow a repeat count to be included in the subprogram call.

Example 29

M98 P30002000

On controls using the common eight-digit P convention, this can represent:

Repeat count = 30

Subprogram number = 02000

Critical compatibility note: M98 repeat-count encoding is controller- and format-dependent. Other controls use different syntax, and some may interpret this value differently or reject it.

Always verify the exact manual before use.

SECTION 30 — M99 SUBPROGRAM RETURN

Example 30

O2100

(EDUCATIONAL SUBPROGRAM)

M99

M99 commonly returns from a subprogram.

The behavior can differ when the program is executed directly or when optional return addresses are used.

SECTION 31 — NESTED SUBPROGRAMS

A nested subprogram calls another subprogram.

Concept:

MAIN PROGRAM

↓

SUBPROGRAM A

↓

SUBPROGRAM B

↓

RETURN TO A

↓

RETURN TO MAIN

Potential benefits:

• Reusable operations
• Reduced duplicate code
• Modular program structure

Potential problems:

• Missing programs
• Incorrect return behavior
• Excessive nesting
• Unexpected modal state

SECTION 32 — HAAS M97 LOCAL SUBPROGRAM

On supported Haas controls, M97 can call a local subprogram using a sequence number.

Example 32 — Structural Illustration

O1300

M97 P100

M30

N100

(LOCAL SUBPROGRAM BODY)

M99

This example illustrates the call-and-return relationship.

It contains no cutting movement and is not a complete machining program.

Verify the applicable Haas control documentation for local subprogram rules.

SECTION 33 — M198 EXTERNAL PROGRAM CALL

M198 is associated with external subprogram calls on some controls.

Its syntax and storage behavior vary.

Typical troubleshooting questions:

• Is external program execution supported?
• Is the program available?
• Is the media configured correctly?
• Is the program reference valid?
• Is the machine using the required option?

Do not assume M198 is supported on every FANUC-style machine.

PART V — FANUC MACRO B PROGRAMMING

SECTION 34 — MACRO VARIABLES

FANUC Macro B uses variables to store values and perform calculations.

Illustrative assignments:

#100 = 50.

#101 = 25.

#102 = [#100 + #101]

After these assignments:

#102 = 75

Variable availability and persistence depend on the controller series and installed macro options.

SECTION 35 — MACRO ARITHMETIC

Example 35

#100 = 20.

#101 = 5.

#102 = [#100 * #101]

#103 = [#100 / #101]

Results:

#102 = 100

#103 = 4

Always validate divisors and input ranges.

SECTION 36 — PARAMETRIC POSITION CALCULATION

Example 36

#100 = 10. (START X)

#101 = 20. (SPACING)

#102 = 3.  (INDEX)

#103 = [#100 + #101 * #102]

Calculated result:

#103 = 70

This formula can generate repeated feature positions.

SECTION 37 — IF / GOTO LOGIC

Example 37 — Educational Macro Logic

#100 = 5

IF [#100 GT 10] GOTO 100

#101 = 1

GOTO 200

N100 #101 = 2

N200

Because #100 is 5, the condition is false and #101 becomes 1.

Macro syntax and permitted control-flow constructs must be verified for the controller.

SECTION 38 — WHILE LOOP

Example 38

#100 = 1

WHILE [#100 LE 5] DO1

  #101 = [#100 * 10]

  #100 = [#100 + 1]

END1

The loop processes index values 1 through 5.

This is an arithmetic demonstration and does not command machine movement.

SECTION 39 — MACRO INPUT VALIDATION

A professional macro should reject invalid inputs.

Conceptual logic:

IF HOLE_COUNT <= 0:

    STOP WITH EXPLANATION

IF RADIUS <= 0:

    STOP WITH EXPLANATION

IF REQUESTED_DEPTH EXCEEDS LIMIT:

    STOP WITH EXPLANATION

This is pseudocode, not executable CNC syntax.

On supported controls, validated alarm-generation mechanisms can be used to stop a program with an informative message.

SECTION 40 — BOLT CIRCLE FORMULA

For N equally spaced holes:

Angle Step = 360 / N

Angle = Start Angle + Index × Angle Step

X = Center X + Radius × COS(Angle)

Y = Center Y + Radius × SIN(Angle)

Example:

Center = X0 Y0

Radius = 40 mm

Hole count = 8

Angle step = 45 degrees

SECTION 41 — BOLT CIRCLE COORDINATES

For an eight-hole pattern with a 40 mm radius:

Hole	Angle	X	Y
1	0°	40.000	0.000
2	45°	28.284	28.284
3	90°	0.000	40.000
4	135°	-28.284	28.284
5	180°	-40.000	0.000
6	225°	-28.284	-28.284
7	270°	0.000	-40.000
8	315°	28.284	-28.284

Coordinates are rounded to three decimal places.

SECTION 42 — BOLT CIRCLE MACRO CALCULATION

Example 42 — FANUC Macro B-Style Calculation

#100 = 0.    (CENTER X)

#101 = 0.    (CENTER Y)

#102 = 40.   (RADIUS)

#103 = 8.    (HOLE COUNT)

#104 = 0.    (START ANGLE)

#105 = 0.    (INDEX)

WHILE [#105 LT #103] DO1

  #106 = [#104 + #105 * 360. / #103]

  #107 = [#100 + #102 * COS[#106]]

  #108 = [#101 + #102 * SIN[#106]]

  #105 = [#105 + 1]

END1

This calculates hole positions but does not drill them.

On supported FANUC Macro B controls, trigonometric functions commonly use degrees.

A production implementation must validate the hole count, radius, coordinates, drilling cycle, clearances, and machine configuration.

SECTION 43 — GRID PATTERN FORMULA

For a rectangular grid:

X = Start X + Column × X Spacing

Y = Start Y + Row × Y Spacing

Example:

4 columns

3 rows

X spacing = 20 mm

Y spacing = 15 mm

Total holes:

4 × 3 = 12

A nested-loop macro can calculate these positions.

SECTION 44 — NESTED LOOP CONCEPT

FOR EACH ROW:

    FOR EACH COLUMN:

        CALCULATE X

        CALCULATE Y

        PROCESS FEATURE

This is pseudocode.

Actual CNC syntax depends on the controller’s macro language.

SECTION 45 — PARAMETRIC PART FAMILIES

Instead of storing a separate program for every similar part, a macro can accept parameters such as:

• Part length
• Part width
• Hole diameter
• Hole spacing
• Hole count
• Machining depth
• Finishing allowance

This approach can reduce duplicate code and simplify controlled program maintenance.

PART VI — CNC TURNING PROGRAMMING

SECTION 46 — CNC LATHE PROGRAM STRUCTURE

A CNC lathe program commonly includes:

• Work offset
• Tool selection
• Spindle mode
• Spindle speed
• Feed mode
• Tool geometry offsets
• Approach movement
• Cutting movement
• Retraction
• Program termination

Turning syntax is particularly controller-specific.

Tool call formats, canned cycles, diameter/radius programming, and feed conventions must be verified.

SECTION 47 — G96 CONSTANT SURFACE SPEED

G96 is commonly used for constant surface speed in turning.

The controller adjusts spindle RPM as the cutting diameter changes.

For metric units:

RPM = (1000 × Cutting Speed) / (π × Diameter)

Example:

Cutting speed = 180 m/min

Diameter = 60 mm

RPM ≈ 955

As diameter decreases, the calculated RPM increases.

A suitable spindle speed limit must be established according to the machine and process.

SECTION 48 — G97 CONSTANT RPM

G97 commonly selects fixed spindle speed in turning.

Example 48

G97 S1200 M03

On a compatible lathe, this requests clockwise spindle rotation at 1200 RPM.

Verify the machine’s spindle-direction conventions and operating conditions.

SECTION 49 — FEED PER REVOLUTION

Feed per revolution is widely used in turning.

Example:

Feed = 0.20 mm/rev

Spindle speed = 1000 RPM

Equivalent linear feed at constant RPM:

0.20 × 1000 = 200 mm/min

The G-code used to select feed per revolution depends on the controller and machine type.

Important: G98/G99 meanings in turning may differ from G98/G99 canned-cycle return meanings in milling.

SECTION 50 — G71 ROUGH TURNING CYCLE

G71 is associated with rough turning on many FANUC-style lathes.

However, there are multiple G71 programming formats.

Some controls use one-line formats.

Others use two-line formats.

Parameters and profile definitions vary.

Conceptual process

1. Define roughing allowance.
2. Define depth of cut.
3. Define contour profile.
4. Execute repeated roughing passes.
5. Leave specified finishing stock.

Do not copy G71 syntax from an unrelated controller generation.

SECTION 51 — G70 FINISHING CYCLE

On many FANUC-style lathes, G70 is used to finish a previously defined profile.

A common workflow is:

G71 — Roughing

G70 — Finishing

The exact profile reference and cycle format depend on the control.

SECTION 52 — G72 FACING ROUGHING

G72 is associated with facing roughing cycles on many FANUC-style turning controls.

It is useful for removing material primarily in the facing direction.

As with G71, syntax and parameters vary.

SECTION 53 — G76 THREADING CYCLE

G76 is a commonly used threading cycle on many CNC lathes.

Potential parameters include:

• Thread pitch
• Thread depth
• Finishing allowance
• Number of finishing passes
• Infeed behavior
• Thread geometry

Critical: G76 formats vary significantly between controller generations.

A two-line G76 program from one machine must not be assumed compatible with another.

SECTION 54 — THREAD PITCH AND LEAD

For a single-start thread:

Lead = Pitch

For a multi-start thread:

Lead = Pitch × Number of Starts

Example:

Pitch = 2 mm

Starts = 2

Lead = 4 mm per revolution

Threading synchronization and cycle programming must follow the specific controller documentation.

PART VII — PROFESSIONAL CNC PROGRAMMING SHORTCUTS

SECTION 55 — USE MODAL COMMANDS INTENTIONALLY

Modal commands remain active according to the controller’s rules.

This can reduce repeated code.

However, excessive reliance on implicit modal state makes debugging harder.

Professional programs balance compactness with clarity.

SECTION 56 — REPLACE REPETITION WITH SUBPROGRAMS

If an operation is repeated at multiple locations, a reusable subprogram may simplify maintenance.

Potential benefits:

• Less duplicated code
• Easier corrections
• Consistent operation logic
• Smaller program size

Every subprogram must define or document its required entry state.

SECTION 57 — REPLACE FIXED COORDINATES WITH FORMULAS

For repeated geometry, use calculations.

Examples:

Bolt circles

Hole grids

Linear arrays

Radial slots

Part families

Variable spacing

Mathematical generation can reduce manual coordinate errors when properly validated.

SECTION 58 — USE CANNED CYCLES WHERE APPROPRIATE

Canned cycles can simplify common operations.

Examples:

G81 — Drilling

G82 — Dwell drilling

G83 — Deep-hole drilling

G84 — Tapping

Always confirm the supported cycle format and behavior.

SECTION 59 — CONTROL RETRACT HEIGHTS

Excessive retract distances increase cycle time.

Insufficient retract distances increase collision risk.

The correct retract strategy depends on:

• Fixture geometry
• Stock geometry
• Tool length
• Holder dimensions
• Machine kinematics
• Operation sequence

Optimization must never sacrifice verified clearance.

SECTION 60 — MINIMIZE UNNECESSARY TOOL CHANGES

Operation planning can reduce repeated tool changes.

Possible improvements:

• Group compatible operations
• Plan tool order
• Reuse verified tools
• Coordinate multiple fixtures

The best sequence also depends on setup stability, part quality, and inspection requirements.

SECTION 61 — USE MEANINGFUL PROGRAM COMMENTS

Example 61

O1500 (ALUMINUM PLATE – OP10)

(TOOL 01 – 6MM DRILL)

(WORK OFFSET – G54)

(VERIFY SETUP BEFORE EXECUTION)

Comments improve readability and reduce ambiguity.

They do not replace setup verification.

SECTION 62 — VERIFY TOOL NUMBERS AND OFFSETS

Common mistakes include:

• Wrong tool number
• Wrong H offset
• Wrong D offset
• Incorrect measured tool length
• Incorrect tool diameter
• Tool replacement without data verification

The tool table and physical setup must agree.

SECTION 63 — CHECK PROGRAM MODAL STATE

Important modes include:

• Units
• Plane
• Absolute/incremental positioning
• Feed mode
• Work offset
• Tool length compensation
• Cutter compensation
• Canned-cycle state
• Spindle mode

Many unexpected movements originate from an earlier modal command.

SECTION 64 — CHECK SUBPROGRAM ENTRY CONDITIONS

Before calling a subprogram, establish its requirements.

For example:

Expected tool

Expected work offset

Expected coordinate mode

Expected feed mode

Expected entry position

Expected safe clearance

A reusable subprogram is only reliable when its assumptions are explicit.

SECTION 65 — VALIDATE MACRO INPUTS

Professional macros should reject:

• Zero hole counts
• Negative radii where invalid
• Excessive depths
• Invalid tool dimensions
• Coordinates outside approved ranges
• Unsupported parameter combinations

Never calculate motion from unchecked inputs.

PART VIII — CNC TROUBLESHOOTING EXAMPLES

SECTION 66 — WHY DOES G02 OR G03 ALARM?

Check:

1. Active plane
2. Arc direction
3. Start and end points
4. I/J/K or R values
5. Controller arc conventions
6. Geometry consistency

A geometrically impossible arc cannot be repaired by changing feedrate.

SECTION 67 — WHY DOES G83 NOT WORK?

Potential causes:

• Incorrect peck value
• Incorrect R plane
• Incorrect depth
• Unsupported syntax
• Wrong active mode
• Controller-specific cycle requirements

Verify the cycle definition for the exact control.

SECTION 68 — WHY DOES M98 NOT WORK?

Potential causes:

• Subprogram missing
• Incorrect program number
• Incorrect call format
• Unsupported storage configuration
• Excessive nesting
• Program access restrictions

Check the caller and target program together.

SECTION 69 — WHY DOES M99 LOOP FOREVER?

Possible causes:

• M99 used in the wrong context
• Incorrect subprogram structure
• Wrong return behavior
• Main program executed as a loop
• Incorrect call chain

Use a subprogram call graph to trace execution.

SECTION 70 — WHY DOES THE TOOL MOVE TO THE WRONG POSITION?

Check:

• G90/G91
• G54–G59
• Tool length compensation
• Machine coordinates
• Macro calculations
• Work offset values
• Program restart state

The problematic move may be caused by a command several blocks earlier.

SECTION 71 — WHY DOES G84 TAP INCORRECTLY?

Check:

• Thread pitch
• Spindle speed
• Feedrate
• Feed mode
• Rigid-tapping requirements
• Spindle synchronization
• Tool and holder
• Controller-specific cycle syntax

Never assume the same tapping program works on all machines.

SECTION 72 — WHY DOES THE CNC PROGRAM RUN SLOWLY?

Possible reasons:

• Excessive air cutting
• Long retracts
• Unnecessary tool changes
• Dense CAM output
• Controller look-ahead limitations
• Acceleration limits
• Excessive corner deceleration
• Conservative cutting parameters

Optimize only after confirming that the current program is safe and dimensionally correct.

PART IX — CNC PROGRAMMING CALCULATORS

SECTION 73 — SPINDLE SPEED CALCULATOR

Metric formula:

RPM = (1000 × Vc) / (π × D)

Where:

Vc = Cutting speed in m/min

D = Tool or workpiece diameter in mm

Example:

Vc = 120 m/min

D = 10 mm

RPM ≈ 3820

This is a mathematical calculation, not a recommendation for a particular tool or material.

SECTION 74 — MILLING FEEDRATE CALCULATOR

For a milling cutter:

Feedrate = RPM × Number of Teeth × Feed per Tooth

Example:

RPM = 3000

Teeth = 4

Feed per tooth = 0.05 mm

Feedrate:

3000 × 4 × 0.05 = 600 mm/min

Actual cutting parameters must be selected using tool and material data.

SECTION 75 — DRILLING FEEDRATE CALCULATOR

For feed per revolution:

Feedrate = RPM × Feed per Revolution

Example:

RPM = 1200

Feed per revolution = 0.10 mm

Feedrate:

120 mm/min

SECTION 76 — BOLT CIRCLE CALCULATOR

Inputs:

• Center X
• Center Y
• Radius
• Hole count
• Start angle

Outputs:

• Hole angles
• X coordinates
• Y coordinates

This is a strong candidate for an interactive CNC website tool.

SECTION 77 — ARC CENTER CALCULATOR

Inputs:

• Start point
• End point
• Radius
• Direction
• Plane

Outputs:

• Valid possible arc centers
• I/J/K values
• Arc sweep

Arc-center solutions must be evaluated for the requested direction and sweep.

SECTION 78 — CYCLE TIME ESTIMATOR

A basic estimator can consider:

• Cutting distance
• Programmed feed
• Rapid distance
• Tool changes
• Spindle acceleration
• Drilling cycles
• Dwell times

A basic feed-move estimate is:

Time = Distance / Feedrate

Actual CNC cycle time also depends on machine dynamics, control processing, acceleration, and operation-specific behavior.

PART X — CONTROLLER-SPECIFIC PROGRAMMING

SECTION 79 — FANUC PROGRAMMING

Common areas:

G-code and M-code programming

Macro B

M98/M99

Canned cycles

Tool compensation

Work offsets

High-speed machining options

Advanced transformations

The exact FANUC series and machine-builder configuration must be identified.

SECTION 80 — HAAS PROGRAMMING

Common areas:

Haas G-code

Haas M-code

M97 local subprograms

M98/M99

G12/G13 circular pocketing

G187 accuracy control

Haas macros

Probing integration

Do not assume every Haas feature exists on every control generation.

SECTION 81 — SIEMENS SINUMERIK PROGRAMMING

SINUMERIK programming can include:

DIN/ISO-style commands

Controller-specific cycles

High-level programming constructs

Coordinate transformations

CYCLE832

TRAORI

Advanced tool management

Digital-twin workflows

Siemens programming conventions are not interchangeable with FANUC Macro B syntax.

SECTION 82 — CNC LATHE VS CNC MILL

The same code number can have different meanings depending on the machine type and controller.

Important differences include:

• Feed modes
• Canned cycles
• Tool selection
• Work coordinate conventions
• Diameter programming
• Spindle modes
• Compensation

Always identify whether a reference applies to milling or turning.

PART XI — BUILDING A CNC CODE EXAMPLES DATABASE

SECTION 83 — THE IDEAL CNC EXAMPLE PAGE

Every example should include:

Program title

What the program demonstrates.

Controller

Exact control family and version.

Machine type

Mill, lathe, or other machine.

Required options

Macro, probing, advanced cycle, or other requirements.

Setup assumptions

Tool, stock, work offset, and coordinate system.

Code

Readable, formatted NC program.

Line-by-line explanation

Meaning of each important command.

Expected toolpath

Diagram or simulation where available.

Common errors

Typical mistakes and diagnostic checks.

Verification

Required simulation and setup checks.

Official references

Applicable manufacturer documentation.

SECTION 84 — SEARCH BY G-CODE

Examples:

G00 example

G01 example

G02 example

G03 example

G43 example

G54 example

G81 example

G82 example

G83 example

G84 example

G90 example

G91 example

G96 example

G97 example

SECTION 85 — SEARCH BY M-CODE

Examples:

M03 example

M04 example

M05 example

M06 example

M08 example

M09 example

M30 example

M97 example

M98 example

M99 example

M198 example

SECTION 86 — SEARCH BY MACHINING OPERATION

Examples:

CNC face milling program

CNC pocket milling program

CNC slot milling program

CNC drilling program

CNC peck drilling program

CNC tapping program

CNC bolt circle program

CNC thread milling concept

CNC rough turning cycle

CNC finishing cycle

CNC threading cycle

CNC macro programming

SECTION 87 — SEARCH BY DIFFICULTY

Beginner

Basic positioning

Straight-line machining

Work offsets

Simple drilling

Intermediate

Arcs

Canned cycles

Tool compensation

Subprograms

Advanced

Macro variables

Loops

Parametric geometry

Controller-specific cycles

Expert

5-axis transformations

Probing

Adaptive machining

Digital-twin verification

Machine automation

PART XII — CNC PROGRAMMING FAQ

SECTION 88 — WHAT IS THE MOST COMMON CNC PROGRAM?

There is no single most common program for every shop.

However, basic positioning, drilling, contouring, and tool-change operations are fundamental to many CNC machining workflows.

SECTION 89 — CAN I COPY A CNC PROGRAM FROM THE INTERNET?

You can study an example, but you should not execute it on a physical machine without verifying controller compatibility, machine configuration, tooling, offsets, workholding, motion, and safety.

SECTION 90 — IS FANUC G-CODE THE SAME AS HAAS G-CODE?

They share many programming concepts, but they are not identical.

Subprograms, macros, canned cycles, M-codes, and advanced features may differ.

SECTION 91 — WHAT IS THE DIFFERENCE BETWEEN M98 AND M99?

On many FANUC-style controls:

M98 calls a subprogram.

M99 returns from a subprogram or performs controller-specific return/repetition behavior.

Exact behavior depends on the control.

SECTION 92 — WHAT IS THE DIFFERENCE BETWEEN G81 AND G83?

G81 commonly performs a basic drilling cycle.

G83 commonly performs peck drilling with repeated cutting and retract behavior.

The exact motion depends on the controller.

SECTION 93 — WHAT IS THE DIFFERENCE BETWEEN G90 AND G91?

G90 commonly selects absolute positioning.

G91 commonly selects incremental positioning.

Incorrect use can cause unexpected machine movement.

SECTION 94 — WHAT IS FANUC MACRO B?

Macro B is a controller programming capability that supports variables, calculations, conditions, and loops on appropriately equipped FANUC controls.

It can be used for parametric machining and automation.

SECTION 95 — WHAT IS THE BEST WAY TO LEARN CNC G-CODE?

A practical learning sequence is:

Understand coordinates.

Learn basic motion.

Understand work offsets.

Understand tool compensation.

Practice drilling cycles.

Learn arcs.

Study subprograms.

Learn macro programming.

Use simulation.

Verify controller-specific behavior.

SECTION 96 — CAN AI WRITE CNC PROGRAMS?

AI can assist with explanations, program structure, calculations, and draft code.

However, AI-generated NC code may contain unsupported commands, incorrect assumptions, or unsafe movements.

Controller-specific verification remains essential.

PART XIII — THE FUTURE OF CNC PROGRAMMING IN 2026

SECTION 97 — AI-ASSISTED CNC PROGRAMMING

Modern manufacturing software increasingly incorporates AI-assisted capabilities.

Potential applications include:

• Feature recognition
• Tool selection assistance
• Machining strategy recommendations
• Program explanation
• Process documentation
• Manufacturing knowledge retrieval

AI should support engineering judgment rather than replace program verification.

SECTION 98 — CNC DIGITAL TWINS

A CNC digital twin can represent the machine environment.

Potential elements include:

• Machine axes
• Kinematics
• Tool assemblies
• Stock
• Fixtures
• NC program
• Controller behavior

Machine-specific simulation can help detect problems that simple G-code visualization may miss.

SECTION 99 — CLOSED-LOOP CNC PROGRAMMING

Closed-loop machining integrates measurement and correction.

Concept:

MACHINE

↓

MEASURE

↓

COMPARE

↓

VALIDATE

↓

CORRECT

↓

VERIFY

Automatic correction must use validated measurements and controlled correction limits.

SECTION 100 — THE PROFESSIONAL CNC PROGRAMMING WORKFLOW

A reliable workflow is:

UNDERSTAND THE DRAWING

↓

PLAN THE OPERATION

↓

SELECT THE TOOL

↓

VERIFY THE SETUP

↓

WRITE OR GENERATE THE PROGRAM

↓

CHECK THE CONTROLLER SYNTAX

↓

VERIFY MODAL STATES

↓

CHECK OFFSETS

↓

SIMULATE THE TOOLPATH

↓

VERIFY MACHINE AND FIXTURE CLEARANCE

↓

PERFORM CONTROLLED PROVE-OUT

↓

INSPECT THE PART

↓

DOCUMENT THE RESULT

The most valuable CNC program is not necessarily the shortest program.

It is the program that is understandable, maintainable, efficient, and correctly verified for its intended machine.

FINAL REFERENCE — CNC PROGRAMMING QUICK LOOKUP

Code	Common function	Important note
G00	Rapid positioning	Verify motion path
G01	Linear interpolation	Feed mode matters
G02	Clockwise arc	Plane and center matter
G03	Counterclockwise arc	Plane and center matter
G17	XY plane	Common milling convention
G18	XZ plane	Common turning/arc convention
G19	YZ plane	Controller-specific applications
G20	Inch units	Verify controller behavior
G21	Metric units	Verify controller behavior
G40	Cancel cutter compensation	Check lead-out requirements
G41	Cutter compensation left	Geometry and lead-in matter
G42	Cutter compensation right	Geometry and lead-in matter
G43	Tool length compensation	Verify H offset
G49	Cancel tool length compensation	Verify subsequent motion
G54	Work offset	Verify setup
G55	Work offset	Verify setup
G80	Cancel canned cycle	Avoid unintended repetition
G81	Drilling cycle	Verify Z and R
G82	Dwell drilling	Verify dwell units
G83	Peck drilling	Verify Q and retract behavior
G84	Tapping	Verify synchronization
G90	Absolute positioning	Track modal state
G91	Incremental positioning	Track modal state
G96	Constant surface speed	Common turning function
G97	Constant RPM	Common turning function
M03	Spindle clockwise	Verify machine convention
M04	Spindle counterclockwise	Verify machine convention
M05	Spindle stop	Common convention
M06	Tool change	Machine-specific
M08	Coolant on	Machine-specific
M09	Coolant off	Machine-specific
M30	Program end	Common convention
M97	Local subprogram	Haas-specific usage
M98	Subprogram call	Syntax varies
M99	Subprogram return	Context matters
M198	External program call	Option/controller dependent

CONCLUSION — FROM CNC CODE EXAMPLES TO PROFESSIONAL PROGRAMMING

Learning CNC programming requires more than memorizing G-codes.

A professional CNC programmer understands:

MOTION

How the machine moves.

COORDINATES

How positions are defined.

OFFSETS

How tools and workpieces are located.

CYCLES

How repeated operations are programmed.

SUBPROGRAMS

How code can be reused.

MACROS

How logic and mathematics generate motion.

CONTROLLERS

Why programming conventions differ.

VERIFICATION

How programs are checked before machining.

AUTOMATION

How CNC programming connects to measurement, monitoring, and production systems.

The most effective approach is to combine real programming examples with clear explanations, controller-specific documentation, and reliable verification methods.

LEARN THE CODE. UNDERSTAND THE LOGIC. VERIFY THE MACHINE. PROGRAM WITH CONFIDENCE.

2026 Edition — CNC G-Code Examples, FANUC and Haas Programming, Milling, Turning, Drilling, Tapping, M98/M99 Subprograms, Macro B and Professional CNC Programming Reference.