Skip to main content

Coordinate Systems

Understanding coordinate systems is fundamental to CNC operation. Coordinate systems define how the machine interprets positions and movements. grblHAL supports multiple coordinate systems that work together to provide flexibility, accuracy, and ease of use.

This guide will explain the different coordinate systems, how they relate to each other, and how to use them effectively.

The Big Picture: Two Main Coordinate Systems​

CNC machines use two primary coordinate systems that work together:

  1. Machine Coordinate System (MCS) - The machine's fixed, absolute reference
  2. Work Coordinate System (WCS) - Your workpiece's movable reference

Think of it this way:

  • Machine coordinates = Where the machine thinks it is in its physical space
  • Work coordinates = Where the tool is relative to your workpiece

Machine Coordinate System (MCS)​

The Machine Coordinate System is the machine's absolute, fixed reference frame. It never changes.

Key Characteristics​

  • Origin (Machine Zero): Established by the homing cycle ($H)
  • Fixed: Does not change unless you re-home the machine
  • Absolute: Always represents the machine's physical position
  • Accessed with G53: Bypasses all work offsets

Machine Zero Location​

Machine zero is typically located at one of the machine's physical limits:

  • X/Y: Usually at the back-right corner. This means the working area is typically in negative coordinates. (Exceptions exist for machines configured with HOMING_FORCE_SET_ORIGIN, where zero depends on switch locations).
  • Z: Usually at the top (maximum Z height).

Example:

After homing, machine position might be:
MPos: 0.000, 0.000, 0.000

When to Use Machine Coordinates​

Use G53 (machine coordinate system) when you need to move to a fixed physical location on the machine:

  • Tool changes - Move to a fixed tool change position
  • Parking - Move to a safe parking location
  • Probing - Move to a fixed probe location
  • Safety - Retract to a known safe height

Example:

G53 G0 Z0        ; Rapid to machine Z-zero (top)
G53 G0 X0 Y0     ; Rapid to machine X/Y zero
Important

Only use G53 after homing! Machine coordinates are meaningless if the machine hasn't been homed. Using G53 without homing can cause crashes.

Work Coordinate Systems (WCS)​

The Work Coordinate System is a user-defined coordinate system that represents your workpiece's position and orientation. This is where you do all your actual machining.

Why Work Coordinates Matter​

Imagine you're machining a part. Your CAM software generates G-code assuming the part's origin is at a specific location (e.g., the front-left corner). But when you clamp the part on your machine table, it could be anywhere!

Work offsets solve this problem by telling the machine: "The part's origin is at this location relative to machine zero."

Available Work Coordinate Systems​

grblHAL supports multiple work coordinate systems, allowing you to have several parts or setups loaded simultaneously:

G-CodeWork OffsetCommon Use
G54Work Offset 1Primary/default workpiece
G55Work Offset 2Second workpiece or setup
G56Work Offset 3Third workpiece
G57Work Offset 4Fourth workpiece
G58Work Offset 5Fifth workpiece
G59Work Offset 6Sixth workpiece
G59.1Work Offset 7Extended offset 1
G59.2Work Offset 8Extended offset 2
G59.3Work Offset 9Extended offset 3
Default

G54 is the default work coordinate system. When you power on grblHAL, G54 is automatically active.

Special Use: G59.3

G59.3 (Work Offset 9) has a special role in grblHAL's Tool Change logic.

  • If Tool Change Mode ($341) is set to 2 or 3, grblHAL uses G59.3 as the dedicated location for tool probing/touch-off.
  • In these modes, do not use G59.3 for regular workpieces, or your setup will be overwritten during tool changes.

How Work Offsets Work​

A work offset is simply a translation (shift) applied to all programmed coordinates.

The Math​

Machine Position = Work Position + Work Offset

Example:

  • Work Offset (G54): X=100, Y=50, Z=10
  • Programmed Position: X=20, Y=30, Z=-5
  • Actual Machine Position: X=120, Y=80, Z=5

When you command G0 X20 Y30, the machine actually moves to machine coordinates X=120, Y=80.

Setting Work Offsets​

There are several ways to set work offsets in grblHAL:

The G10 L20 command sets the work offset so that the current machine position becomes the specified work coordinate.

Syntax:

G10 L20 P<offset_number> X<value> Y<value> Z<value>

Parameters:

  • P = Offset number (1=G54, 2=G55, 3=G56, etc.)
  • X, Y, Z = The work coordinates you want at the current position

Example:

; Move to the front-left corner of your workpiece
G0 X100 Y50 Z10  ; (in machine coordinates)

; Set this position as X0 Y0 Z0 in G54
G10 L20 P1 X0 Y0 Z0

; Now the current position is work coordinate 0,0,0

Method 2: Using G10 L2 (Absolute Offset)​

The G10 L2 command sets the work offset to an absolute value in machine coordinates.

Syntax:

G10 L2 P<offset_number> X<value> Y<value> Z<value>

Example:

; Set G54 origin to machine position X=100, Y=50, Z=10
G10 L2 P1 X100 Y50 Z10

Method 3: Manual Entry (Sender-Specific)​

Most G-code senders have a "Set Work Zero" or "Zero XYZ" button that:

  1. Reads the current machine position
  2. Sets the active work offset so that position = 0,0,0

Typical workflow:

  1. Jog to your workpiece origin (e.g., front-left corner, top surface)
  2. Click "Zero X", "Zero Y", "Zero Z" (or "Zero All")
  3. The sender sends G10 L20 P1 X0 Y0 Z0 for you

Viewing Work Offsets​

To see all current work offset values, send:

$#

Example output:

[G54:100.000,50.000,10.000]
[G55:200.000,50.000,10.000]
[G56:300.000,50.000,10.000]
[G57:0.000,0.000,0.000]
[G58:0.000,0.000,0.000]
[G59:0.000,0.000,0.000]
[G28:0.000,0.000,0.000]
[G30:0.000,0.000,0.000]
[G92:0.000,0.000,0.000]
[TLO:0.000]
[PRB:0.000,0.000,0.000:0]

This shows:

  • G54 origin is at machine position X=100, Y=50, Z=10
  • G55 origin is at machine position X=200, Y=50, Z=10
  • G56 origin is at machine position X=300, Y=50, Z=10
  • G57-G59 are not set (0,0,0)

Practical Example: Multiple Parts​

Let's say you're machining 3 identical parts on your table:

Setup​

  1. Home the machine: $H
  2. Clamp three parts at different locations on the table
  3. Set work offsets for each part:
; Part 1 (G54)
G0 X100 Y50 Z10      ; Jog to Part 1 origin
G10 L20 P1 X0 Y0 Z0  ; Set G54

; Part 2 (G55)
G0 X250 Y50 Z10      ; Jog to Part 2 origin
G10 L20 P2 X0 Y0 Z0  ; Set G55

; Part 3 (G56)
G0 X400 Y50 Z10      ; Jog to Part 3 origin
G10 L20 P3 X0 Y0 Z0  ; Set G56

Running the Job​

; Machine Part 1
G54              ; Select Part 1 coordinate system
M98 P100         ; Call machining program (P100.macro)

; Machine Part 2
G55              ; Select Part 2 coordinate system
M98 P100         ; Call same program, different location

; Machine Part 3
G56              ; Select Part 3 coordinate system
M98 P100         ; Call same program again

M30              ; End program

The same G-code program runs three times, but at three different physical locations thanks to work offsets!

G92: Temporary Coordinate Offset​

G92 is a temporary, volatile coordinate offset that's applied on top of the active work coordinate system (G54-G59).

How G92 Works​

Final Position = Work Position + Work Offset (G54) + G92 Offset

When to Use G92​

  • Rotary axis zeroing - Reset A/B/C axis to 0° at current position
  • Legacy G-code - Some old CAM posts use G92
  • Quick adjustments - Temporary shift without changing work offset
warning

G92 is easy to forget and can cause crashes. Modern practice favors using dedicated work coordinate systems (G54-G59) instead of G92.

G92 Commands​

CommandAction
G92 X0 Y0 Z0Set current position as 0,0,0 (temporary)
G92.1Cancel G92 offset
G92.2Suspend G92 offset
G92.3Restore suspended G92 offset

Example:

G54              ; Using G54 work offset
G0 X10 Y10       ; Move to X=10, Y=10 in G54
G92 X0 Y0        ; Call this position 0,0 (G92 offset applied)
G0 X5 Y5         ; Move to X=5, Y=5 (relative to G92)
G92.1            ; Cancel G92, back to normal G54

Position Display: WPos vs MPos​

When you query position with ?, you'll see two types of coordinates:

<Idle|WPos:10.000,20.000,5.000|MPos:110.000,70.000,15.000>
  • WPos (Work Position): Position in the active work coordinate system
  • MPos (Machine Position): Absolute machine position

Relationship:

MPos = WPos + Active Work Offset

In this example:

  • Work position: X=10, Y=20, Z=5
  • Machine position: X=110, Y=70, Z=15
  • Therefore, work offset (G54) is: X=100, Y=50, Z=10

Best Practices​

1. Always Use Work Coordinates for Machining​

Bad:

G53 G0 X150 Y200  ; Using machine coordinates for cutting

Good:

G54               ; Select work coordinate system
G0 X50 Y100       ; Use work coordinates

2. Set Work Zero at a Consistent Location​

Choose a repeatable reference point on your workpiece:

  • Front-left corner, top surface (most common)
  • Center of part, top surface
  • Center of a hole or feature

3. Document Your Setup​

Keep notes on:

  • Which work offset (G54-G59) is used for which part/setup
  • Where the work zero is located on the part
  • Any special considerations (rotated parts, fixtures, etc.)

4. Use G53 for Safety Moves​

Always use G53 for moves to fixed machine locations:

G53 G0 Z0        ; Retract to machine top (safe)
T2 M6            ; Tool change
G53 G0 X0 Y0     ; Move to tool change position

5. Verify Offsets Before Machining​

After setting work offsets:

  1. Jog to work zero: G0 X0 Y0 Z0
  2. Verify the tool is at the expected location
  3. Test with air cuts before actual machining

6. Avoid G92 Unless Necessary​

Use G54-G59 work offsets instead of G92 for better clarity and safety.

Common Coordinate System Mistakes​

Mistake 1: Using G53 Without Homing​

; Machine not homed!
G53 G0 Z0  ; CRASH! Machine doesn't know where Z0 is

Fix: Always home first: $H

Mistake 2: Forgetting Active Work Offset​

G55              ; Switch to G55
; ... do some work ...
; Forget that G55 is still active
G0 X0 Y0         ; Oops! Moving to G55 zero, not G54 zero

Fix: Explicitly set work offset at start of program:

G54              ; Always specify which offset to use
G0 X0 Y0

Mistake 3: Setting Work Zero While in G91 (Incremental Mode)​

G91              ; Incremental mode
G10 L20 P1 X0    ; This won't work as expected!

Fix: Always use G90 (absolute mode) when setting work offsets:

G90              ; Absolute mode
G10 L20 P1 X0 Y0 Z0

Quick Reference Commands​

CommandDescription
G54 - G59Select work coordinate system 1-6
G59.1 - G59.3Select work coordinate system 7-9
G53Use machine coordinate system (one-shot)
G10 L20 P<n> X- Y- Z-Set work offset (current position method)
G10 L2 P<n> X- Y- Z-Set work offset (absolute method)
$#View all coordinate offsets
G92 X- Y- Z-Set temporary offset
G92.1Cancel G92 offset

Coordinate System Hierarchy​

Understanding the order of coordinate transformations:

1. Machine Coordinates (MCS)
   ↓
2. + Work Offset (G54-G59)
   ↓
3. + G92 Temporary Offset
   ↓
4. + Tool Length Offset (G43)
   ↓
5. = Final Tool Position

Example:

  • Machine position: X=100
  • G54 offset: X=50
  • G92 offset: X=10
  • Tool length offset: Z=25
  • Final position: X=160, Z=25

Next Steps​

Now that you understand coordinate systems:

  1. Practice setting work offsets - Set up a simple part and practice zeroing
  2. Learn about tool offsets - See Automatic Tool Changer
  3. Explore probing - Automate work offset setup with Probing
  4. Study G-code - See Complete G-code Reference
Pro Tip

Many CNC operators create a "setup sheet" template that documents:

  • Part name and revision
  • Work offset used (G54, G55, etc.)
  • Work zero location on the part
  • Tool list with lengths
  • Material and stock size

This makes setups repeatable and reduces errors!

Download our Printable CNC Setup Sheet (Open link, then standardized Print to PDF)