2.1 Coordinate Systems, Machine Axes, & Work Planes
Key Takeaways
Machine coordinates use the axis references established at zero return. G54 through G59 select stored work origins for part programs.
On the illustrated vertical mill, +X is tool motion to the right relative to the part, +Y is toward the rear and +Z increases spindle-to-part clearance.
A, B and C denote rotations about X, Y and Z. The right-hand rule describes positive rotation in the programmed coordinate system.
G17 selects XY with I and J center offsets, G18 selects XZ with I and K, and G19 selects YZ with J and K on a Haas mill.
In ordinary Haas axis motion, G90 specifies an endpoint relative to the active origin. G91 specifies a signed displacement from the current position.
2.1 Coordinate Systems, Machine Axes and Work Planes
Read a coordinate by asking three questions: Which point is zero? What are the positive directions? Does this value give a destination or a displacement? A single number such as X2.000 can produce different tool motion after the operator selects another fixture offset or the program changes distance mode.
Machine Reference and the Part Origin
The machine coordinate system (MCS) gives positions relative to the machine’s axis reference. On a Haas mill, zero return establishes machine zero. The physical travel envelope, limit switches or sensors, and any change position are separate machine details. G53 uses machine coordinates for its own block and ignores work and tool offsets during that block. G28 commands a return to machine zero and can first travel through an intermediate position. Check the commanded path even when the endpoint is known.
A work coordinate system (WCS) gives the program an origin on or near the part. If the drawing locates holes from a lower-left corner, locating work X0 and Y0 at that corner may let you enter the dimensions directly. The setup sheet defines the actual reference. On a Haas mill, G54 through G59 select six work offsets. G154 P1 through G154 P99 access the additional work offsets. Confirm the register in the program and on the setup sheet. For fixture pickup, see Work Coordinates and Fixture Offset Setting.
| Control reference | Question it answers | Example |
|---|---|---|
| Machine coordinates | Where is the axis relative to machine zero? | Confirm a verified retract shown on the machine-position display. |
| Work coordinates | Where is the programmed point relative to the fixture origin? | Program X1.250 from the lower-left corner in G54. |
| Distance mode | Is the value a work position or a change from the current position? | G90 X1.250 or G91 X1.250. |
On a three-axis Haas mill with parallel work and machine axes and no other shifts, if two vises have origins at machine X −10.000 and −6.000 in, respectively, work X +1.250 gives machine X −8.750 in in the first vise and −4.750 in in the second. Work X is the same on the drawing. The physical target changes with the selected origin.
Cartesian Axes and the Right-Hand Rule
Use the right thumb for +X, index finger for +Y and middle finger for +Z, mutually perpendicular. On the illustrated vertical mill, standing at the operator side:
- +X: Tool motion to your right relative to the part. If the table alone moves in X, it moves left.
- +Y: Tool motion toward the rear relative to the part. If the table alone moves in Y, it moves toward the operator.
- +Z: Tool moves away from the workpiece along the spindle axis.
The same relative-coordinate idea applies to rotary motion. A nominal A axis rotates about X, B about Y and C about Z. Point your right thumb along the positive linear axis. Your curled fingers show positive rotary motion in programmed coordinates, counterclockwise as viewed from the positive end toward the origin. The physical direction of a moving table depends on the machine configuration. Use the manufacturer’s diagram for the actual machine.
Selecting a Plane
The active plane tells the Haas mill which axes describe a circular move. It also determines which arc-center addresses can appear. The third axis can move independently of the circular interpolation for a helical move where supported. Haas two-dimensional cutter compensation with G41 or G42 uses G17. Selecting another plane for an arc does not redirect a vertical mill’s standard Z tool-length compensation onto another linear axis.
| Plane | Circular endpoint axes | Signed center offsets from the arc start |
|---|---|---|
| G17, XY | X, Y | I along X, J along Y |
| G18, XZ | X, Z | I along X, K along Z |
| G19, YZ | Y, Z | J along Y, K along Z |
For direction, view XY from +Z toward the origin, XZ from +Y, and YZ from +X. Use the control documentation when working with a rotary or transformed coordinate system.
Trace Absolute and Incremental Motion
In these two independent graphics traces the established work position starts at X0.000 and the tool is already at a verified clearance. Use G20 for inches. The examples move along X only.
G20 G90 G01 X1.000 F10.0 (Arrive at work X1.000)
X3.000 (Travel +2.000 to work X3.000)
X4.000 (Travel +1.000 to work X4.000)
G20 G91 G01 X1.000 F10.0 (Arrive at work X1.000)
X3.000 (Travel +3.000 to work X4.000)
X4.000 (Travel +4.000 to work X8.000)
G90 (Restore the caller's expected distance mode)
Both traces use a previously established feed-per-minute mode. The first trace can also be expressed incrementally with X displacements +1.000, +2.000, +1.000. To convert any ordinary segment, subtract the previous position from the next one. If the next point were X2.500 after X4.000, the incremental input would be X−1.500. When reviewing an incremental routine, maintain a running sum and check where control returns to the caller.
Haas Setting 162 affects the interpretation of various integer axis addresses. Writing the decimal explicitly in examples such as X2.000 makes the intended scale clear. Set and verify units and distance mode at the point in the program that relies on them.
Sources: Haas basic mill programming, axis conventions workbook, Haas rotary operation, and Haas G-code reference.
How does a Haas mill’s machine coordinate system differ from a work coordinate system such as G54?
The operator redefines machine zero for each job.
Machine coordinates use the axis reference established at zero return. G54 selects a stored part or fixture origin.
Machine coordinates apply only to five-axis machines.
G54 sets the spindle speed rather than a position reference.
On the illustrated vertical mill, what does a positive Z move do?
The tool moves away from the part along the spindle axis.
The tool moves toward the part along the spindle axis.
The tool moves across the part along the horizontal X axis.
The tool moves toward the rear along the horizontal Y axis.
On a Haas mill, which endpoint axes and center addresses belong to a G18 arc?
X and Y with I and J
Y and Z with J and K
X and Z with I and K
A and B with J and K
With G20 and G91 active and X currently at −1.000 in, an ordinary linear block commands X2.000. Where is X afterward?
At work X2.000 in
At machine X0.000 in
At work X−3.000 in
At work X+1.000 in
Sections you finish are checked off in the contents.