Coordinate Systems: Absolute, Incremental, and Work Offsets

Why Coordinate Systems Matter

Every CNC program is a set of instructions that tells the machine where to move. Before the machine can follow those instructions, both the programmer and the control need to agree on where zero is and how distances are measured. Get that wrong and the cutter goes to the wrong place — at best you scrap a part, at worst you crash the spindle into the workholding. Understanding coordinate systems is therefore one of the most fundamental — and most safety-critical — skills in CNC machining.

The Two Ways to State a Position: G90 and G91

G90 — Absolute mode tells the machine to move to a position measured from a fixed origin point (called the program zero or workpiece origin). Every coordinate in absolute mode is a direct address from that single reference point. If your program zero is the lower-left corner of a part and you command `G90 G01 X2.000 Y1.500`, the tool moves to exactly 2.000 inches right and 1.500 inches up from that corner — regardless of where the tool was before.

G91 — Incremental mode tells the machine to move a stated distance and direction from wherever the tool currently is. If the tool sits at X2.000 Y1.500 and you command `G91 G01 X0.500 Y-0.750`, the tool moves an additional 0.500 right and 0.750 down, arriving at X2.500 Y0.750 in absolute terms.

Both modes are legal and useful. Absolute (G90) is the default and the safer choice for most programmed moves because an error in one block does not carry forward into the next. Incremental (G91) is handy for repeated patterns, drilling cycles, and moves relative to a current position. Many shops use G90 for the bulk of a program and switch to G91 only where it genuinely simplifies the math.

Key rule: Always know which modal code is active. A G90 or G91 stays in effect until the other is commanded — it does not reset itself. Confirm modal state at the start of every program and after any manual intervention.

Machine Zero vs. Workpiece Zero

The machine itself has a fixed reference called machine home or machine zero (sometimes written G53). Home is set by the builder and is typically a corner of the machine's travel envelope. You almost never program from machine zero directly because the workpiece is never sitting exactly at machine home.

Instead, you define a workpiece coordinate system (WCS) — a new zero point located on or relative to the part. On Haas controls (and most other FANUC-compatible controls), you store this offset in one of the work offset registers: G54 through G59. Each register holds an X, Y, and Z value that describes where the workpiece origin is located relative to machine home.

When your program calls `G54`, the control reads those stored values and shifts its internal reference frame. Every subsequent X, Y, Z coordinate in the program is then measured from the G54 origin, not from machine home.

G54–G59: Six Standard Work Offsets

The six standard work offsets let you store up to six different workpiece positions without rewriting your program. Common uses include:

• G54 — First part, or the only part on a simple setup.
• G55 / G56 — A second or third part on a fixture, or a second operation datum.
• G57–G59 — Additional setups, sub-plates, or fixture positions.

To use a work offset you must measure where the workpiece origin is in machine coordinates and enter those values into the offset table on the control. On a Haas mill this is done through the Offset page, Work tab. Typical methods to find the offset values include using an edge finder, a 3-D probe, or a test indicator — the result is a set of X, Y, Z machine-coordinate values you type into the correct G54–G59 row.

Setting Up Offsets: Step-by-Step Logic

1. Decide where the program zero will be on the part (common choices: lower-left corner of stock, center of a bore, or a datum called out on the print).

2. With the machine at home and the part in the fixture, find the machine-coordinate position of that chosen point using an edge finder or probe.

3. Enter those machine-coordinate values into the G54 (or G55, etc.) offset table.

4. In your program, call `G54` before any cutting moves.

5. The control subtracts the stored offset from machine home so that all programmed coordinates are now relative to your chosen workpiece origin.

Safety Points

• Verify before you cut. After entering offset values, use the machine's dry-run or single-block mode with the feed-rate override turned down and the spindle off. Watch the tool path carefully before allowing any actual cutting.
• Lockout/tagout (LOTO). Whenever you reach inside the machine envelope to set an edge finder or adjust workholding, follow your facility's LOTO procedure. The machine must be in a safe state — not simply paused.
• PPE. Safety glasses are required at all times on the shop floor. When indicating a part by hand, keep fingers away from spindle tooling.
• Never assume a modal code. If a previous operator or program left the machine in G91, your absolute-mode moves will produce wrong positions. Always open a new program with a known modal state (`G90`, `G17`, `G20` or `G21`, etc.).
• Check the Z offset carefully. An incorrect Z offset in G54 is the most common cause of a tool crashing into the part or the vise jaw. Double-check Z before the first approach move.