Coordinate Systems & Work Offsets

Every reference article on this site — Fanuc #5221, Siemens $P_UIFR, Okuma VZOFX, Heidenhain preset tables — assumes you already understand what a work offset is and why a part program never talks to the machine in raw machine coordinates. This page teaches that foundation once, in control-neutral terms, then hands you the map back to each control’s specific registers. If you have ever touched off an edge finder, typed a number into a G54 screen, or wondered why your part machined 3 inches from where you expected, this is the concept underneath it.

Two Coordinate Systems: Machine and Work

A CNC machine actually has two coordinate systems running at all times, and confusing them is the single most common cause of a scrapped part or a crash.

The Machine Coordinate System (MCS) is fixed to the machine itself. Its origin — machine zero (machine home) — is a physical point the control finds every power-up by driving each axis to its reference point (the home switch plus the encoder grid/marker pulse). Machine zero never moves. On most vertical machining centers it sits at a corner of travel with all axes fully retracted, so machine coordinates are typically all-negative numbers. The MCS is the machine’s ground truth: it is where limit switches, tool-change positions, and pallet locations are measured from.

The Work Coordinate System (WCS) is fixed to your part. Its origin — part zero or program zero — is wherever you decide to program from: a corner of the vise, the center of a bore, the top of the stock. CAM posts everything relative to this point. The whole reason we don’t program in machine coordinates is portability: a fixture that sits at a slightly different spot tomorrow, a second part in the other vise, or the same program run on a different machine would all need every coordinate rewritten. Instead, the program stays put and only one number set — the offset — changes.

The relationship is exactly this:

Work position (what you program)  =  Machine position  −  Work offset

… or rearranged, the offset IS the vector from machine zero to part zero:

Work offset  =  Machine position of part zero  −  Machine zero (0)

So the work offset is nothing more than the machine coordinates of your part zero. When you “set G54,” you are telling the control: “my part’s origin lives here, at this spot in the machine.” Everything the program commands is then measured from that spot. To move in raw machine coordinates for a single block — a safe retract to a fixed clearance, a move to a tool-change position — use G53, which is a one-shot, non-modal command that ignores all work offsets for that block only.

Here is that chain in one picture — the same offset values as the G10 example later on this page:

The Standard Work Offsets

A control does not store just one work offset — it stores a table of them, so one program can address several fixtures, a tombstone’s faces, or multiple parts without changing a coordinate. These are the ISO/Fanuc-standard members of the family, and the same G-codes appear on Haas, Mazak, Mitsubishi, and Siemens ISO mode.

These stack. On a Fanuc-family control the effective part zero is the sum of every layer that is active:

Work position  =  Machine position
− External(common) offset
− Active work offset (G54 … G59, or G54.1 Pn)
− G52 local offset
− G92 shift

Read it top to bottom as layers of shift: the external offset moves everything, the selected G54–G59 sets the part, G52 nudges to a local feature, and G92 (if used) adds one more shift. Most jobs use exactly one layer — a single G54 — and that is the healthy default. Siemens organizes the same idea as frames rather than stacked G-codes: a base frame, the settable frame (G54–G59), and a programmable frame (TRANS/ROT, the G52/G68 analog) chain together into the total active frame. See the Sinumerik Programming Basics article for how TRANS and G500 map to G52 and offset cancel.

How Each Control Names the Offset Registers

This is the payoff. The concept above is universal; the register you read or write is control-specific. Every offset lives at an addressable location, and once you know the address you can read it, log it, or overwrite it from a macro. Each row links to that control’s full reference on this site.

Two things to notice. First, the Fanuc-family controls (Fanuc, Haas, Mazak, Mitsubishi) deliberately share the #5221–#5226 map for G54 and #7001+ for the extended set — a macro that touches offsets is largely portable among them. The one trap: #5201–#5206 is the external offset on Fanuc/Mazak/Mitsubishi but the G52 shift on Haas. Second, Siemens, Heidenhain, and Okuma abandon numbered registers for named ones — a frame, a table row, a function-and-axis name — but the underlying quantity is identical: the vector from machine zero to part zero.

Setting a Work Offset

There are three ways the number gets into the register, from most manual to most automated.

1. At the machine (touch-off). The everyday method. Put an edge finder, dowel, or spindle probe against a known feature, read the machine position, and store it into the offset. Most controls have a “set” softkey on the offset page that captures the current axis position for you (jog-and-set); for Z you typically touch the tool or a gauge block to the top of the part. A wireless or wired touch probe automates the touch-off with a cycle — probe two edges for X / Y, a bore for a center, or a boss for a datum — and writes the result directly into G54 without arithmetic. The key idea is unchanged: whatever the method, you are measuring where part zero sits in machine coordinates and storing that vector.

2. From the program with G10. The G10 command (programmable data input) writes offset registers straight from NC code — no macro option required. For work offsets the format is G10 L2 P__, where P1–P6 select G54–G59 and P0 selects the external offset; the extended offsets use L20 with P1–P48. The active G90/G91 mode matters: G90 writes an absolute value, G91 adds to whatever is already there.

G90 G10 L2 P0 X-10.0             ; external offset X = -10 (shifts ALL offsets)
G90 G10 L2 P1 X-450.0 Y-375.0 Z0 ; set G54 absolutely (P1 = G54)
G90 G10 L2 P3 X-630.0 Y-408.0    ; set G56; Z omitted, so G56 Z is left unchanged
G91 G10 L2 P1 X5.0               ; ADD 5 mm to the current G54 X (incremental)
G10 L20 P1 X-200.0 Y-150.0 Z0    ; set the first EXTENDED offset (G54.1 P1)

A common pattern: an operator measures a fixture once, then a short G10 preamble at the top of the program stamps every offset for the tombstone so nothing depends on stale screen values.

3. From a macro (probe → write the register). Because the offset registers are ordinary system variables, a probing routine can capture a measured position and write it back. This is the heart of in-process probing: trip the probe with a G31 skip move, read the trigger position out of the skip variables (#5061–#5063 on Fanuc), and store the result into the active offset. For example, adding a probed correction to G54 X is a single line:

#5221 = #5221 + #500   ; add the probing result (#500) to G54 X

The same move on a Siemens control writes the frame — $P_UIFR[1,X,TR] = $P_UIFR[1,X,TR] + R1 — and on Okuma writes the named variable, VZOFX[1] = VZOFX[1] + VC1. For the mechanics of reading skip positions and writing offset variables safely (save/restore modal state, absolute vs incremental), see Modal & Position Data, which walks through the #5061/#5221 pairing used by every probing macro.

Tool Length vs. Work Offset — Don’t Confuse Them

These are the two offsets people mix up, and they answer two different questions. The work offset (G54) answers “where is the part?” — it is one vector per fixture, shared by every tool. The tool length offset (called with G43 H__ on Fanuc-style controls, automatic via the D-edge on Siemens) answers “how far does this particular tool stick out of the spindle?” — it is one value per tool. In the Z axis both stack up: the machine drops the spindle to work-offset Z plus the active tool length so that Z0 in the program lands on the part top no matter which tool is loaded.

Getting the split wrong is a classic error: bake a tool’s stick-out into the G54 Z and every other tool cuts at the wrong depth; conversely, set part location in a tool offset and only one tool finds the part. The clean rule is part geometry goes in the work offset, tool geometry goes in the tool offset. For how each control stores tool length and radius — geometry vs. wear, memory types A/B/C, the #2001/#2401 registers — see Tool Offset Variables.

Common Gotchas & Crashes

The through-line for all of these: know which coordinate system a number lives in before you trust it. A value that is correct in machine coordinates is a crash in work coordinates, and vice versa. When in doubt, single-block the first moves and watch the position display switch between machine and work readouts.

References

• Peter Smid, Fanuc CNC Custom Macros, Industrial Press, 2004 — Chapter 5 (Data Setting / G10) and the work-offset concept chapters.
• Fanuc, Operator’s Manual / Parameter Manual, FANUC Corporation.