Offsets are how a CNC machine is told about the real world. A program describes a part in perfect coordinates, but the vise sits wherever the setup person clamped it, every tool sticks out of its holder by a different amount, and cutters get smaller as they wear. Offsets are the stored numbers that bridge that gap, so one program can run on Monday and again in March without a single line of code being edited.

If you have ever wondered why the same program cuts a good part on one machine and scrap on another, the answer is almost always an offset.

What Is an Offset on a CNC Machine?

Think of offsets as the memory buttons on a calculator. You store a value once, then refer to it by name for the rest of the job instead of typing it in again. In a CNC control, an offset is a numbered storage location holding a measurement, and like a calculator memory it means nothing until a program calls for it.

That separation is the whole point. The programmer writes the part. The setup person measures the machine. The two meet at the offset table, which is why a well written program contains almost no numbers that describe your particular machine, your particular vise, or the tool you happened to grab.

Most controls group offsets into two tables: one for where the part is, and one for the tools. Nearly every offset you will touch belongs to one of those two families.

The Main Types of CNC Offsets

This is the question most operators are really asking, so here is the short answer before the detail.

Offset type What it corrects for Typical code
Work offset Where the part is sitting on the table G54 to G59 on Fanuc and Haas
Tool length offset How far each tool sticks out of the spindle G43 with an H number
Wear offset Small size changes as a tool dulls Wear column of the tool table
Cutter radius compensation The size of a milling cutter G41 or G42 with a D number
Tool nose radius compensation The rounded tip of a turning insert G41 or G42 on a lathe

The first three do the heavy lifting on a typical job, and they are covered in full below.

Work Offsets: G54 Through G59

A work offset tells the control where the part zero is, measured from machine zero, the coordinate origin the machine establishes when it homes. Once it is set, the program can describe the part from its own corner or centre and ignore where the fixture actually sits.

On Fanuc and Haas controls, which cover most of the machines in a typical job shop, you get at least six standard work offsets, called up with G54, G55, G56, G57, G58 and G59. Other controls do the same job differently, and it is worth knowing which one you are standing in front of. Siemens gives you G54 to G57 as standard and uses G58 and G59 for something else entirely, Okuma selects work offsets with G15 H1 and upward, and a Mazak running Mazatrol carries the zero in the program’s work coordinate header rather than in a G code at all.

The six are not ranked by importance, but G54 is not quite arbitrary either. Most controls power up with G54 already active, so a program that never calls a work offset will run in G54 whether you meant it to or not. That is exactly why leaving a stale number in G54 catches people out. Whether a reset also returns you to G54 is a parameter on Fanuc, so check your own machine rather than assume it.

Setting one means locating the part zero, usually with an edge finder, a probe or an indicator, and storing the machine position of that point into the chosen offset register. From then on, a command like G54 G00 X0 Y0 sends the tool to your part zero rather than to the corner of the table.

Where this earns its keep is repeat work and multiple fixtures. Run four vises across the table and you can give each one its own offset, G54 through G57, then call the same subprogram four times. Nothing in the cutting code changes. Only the offset call does. Tear the setup down, put it back next year, re-find the zero, and the program is good again.

Two related items are worth knowing. G92 is an older way of shifting the coordinate system that is still found in legacy mill programs, and it behaves differently from a work offset because it is declared in the program rather than stored in a table, which makes it much easier to leave in a bad state. A G92 shift is easy to leave behind, and the controls do not agree on how to get rid of it. On Fanuc it survives a reset, on many Fanuc controls it survives a power cycle too, and the command that actually clears it is G92.1 X0 Y0 Z0. Haas works differently: it does not accept G92.1, it shows the accumulated shift at the bottom of the Work Offsets page where you can zero it by hand, and it clears the shift on power up and on a zero return. Note also that on most Fanuc lathes, the ones running G code system A, G92 is not a coordinate shift at all but the thread cutting cycle, and the coordinate set command is G50 instead.

Many controls also offer extended work offsets when six are not enough, giving dozens of extra registers for fixture plates and pallets. The syntax is vendor specific: G54.1 P1 and upward on Fanuc, G154 P1 through P99 on Haas, with older Haas machines using G110 through G129 for the first twenty of the same registers, and G505 upward on Siemens.

Because work offsets are expressed in machine coordinates, it helps to be comfortable with how your control reports position in the first place. Our guide to absolute versus incremental motion covers that distinction, and know your machine is a useful companion if you are new to the control you are standing in front of.

Tool Length Offsets: G43 and the H Register

No two tools stick out of the spindle by the same amount, and a programmer writing the part months earlier has no way to predict that. The tool length offset solves it. Each tool’s length is measured during setup and stored in its own register, then the program activates it when that tool is loaded.

The usual form is G43 H01, which means “apply tool length compensation using the value in register one.” G43 applies the stored length, G44 applies it in the negative direction and is rarely used on modern equipment, and G49 cancels compensation altogether. The H number points at the register, and by convention shops keep H numbers matched to tool numbers so that tool 5 uses H05. Most controls do not enforce that by default, though some will: Haas Setting 15, H and T Code Agreement, alarms out if the H code does not match the tool in the spindle, though it will not catch H00. Plenty of shops leave it off because programmers want to assign offsets freely, which is exactly how mismatches survive to the spindle.

Lengths are typically set one of two ways. A tool presetter measures each holder and tool assembly away from the machine, which is fast and keeps the spindle cutting. Alternatively the operator touches each tool off a known surface at the machine and lets the control record the position. These two methods do not produce the same number and they are not interchangeable: a presetter gives you assembly length from the gauge line, while touching off at the machine usually stores the distance from machine zero down to the part. A shop moving from one method to the other has to change how Z zero is carried in the work offset, and skipping that step is a reliable way to crash a machine. Presetting is the more repeatable of the two, and it is one of the practical reasons shops standardise on consistent, good condition holders rather than a mixed drawer of whatever fits. Our tool holders 101 guide covers the common taper families, and HSK versus CAT explains why the interface itself affects how repeatably a tool seats, and therefore how much you can trust a length you measured last week.

A worn or damaged holder is a genuine accuracy problem here, because a length offset assumes the assembly seats the same way every time it is loaded. If it does not, the number in the register is correct and the part is still wrong.

Wear Offsets: Holding Size as a Tool Dulls

A geometry offset says how long or how big a tool is. A wear offset says how much that has drifted since setup, and it is the one operators touch most often.

Cutting tools do not stay the same size. Inserts dull, end mills lose a little diameter, and a finishing pass that held size perfectly at eight in the morning can start leaving parts a few thousandths oversize by mid afternoon. Rather than re-measuring and rewriting the geometry offset, the operator nudges the wear offset by the small amount needed and the next part comes back in tolerance.

Most controls keep wear in its own column alongside geometry, and the control simply adds the two. Keeping them separate matters more than it first appears. Geometry is what the tool is, measured once at setup. Wear is what has changed since, and it is expected to creep. When an operator dumps a correction into the geometry column instead, the record of the tool’s true length is lost, and the next person to load that tool inherits a number nobody can verify. On Fanuc this split depends on which offset memory type the machine was built with, since the oldest type stores a single value per offset number and gives you no separate wear column at all.

Turning centres lean on this especially hard, because the operator is holding a diameter directly. On a lathe you will commonly see a tool called with something like T0101, where the first pair is the tool station and the second pair is the offset it uses. Adjusting the wear offset for that station walks the diameter in by the amount you enter, which is how a lathe operator holds a tight size across a run without touching the program.

One habit worth building: wear offsets should be small. A wear correction measured in tenths or a few thousandths is doing its job. A wear correction of a quarter inch is not wear, it is a mistake somewhere else, and entering it hides the real problem instead of fixing it.

Cutter Radius and Tool Nose Radius Compensation

The remaining offsets describe the shape of the cutting edge rather than its position.

Cutter radius compensation lets a programmer write the path of the finished profile rather than the path of the cutter centre. The control then offsets the toolpath by the size stored against that tool, called up with G41 for left of the path or G42 for right, both judged looking along the direction the tool is travelling, with a D number pointing at the register, and cancelled with G40. The practical payoff is that a half inch end mill can be replaced with one that has been resharpened slightly undersize, and only the stored value needs to change.

It also gives you a clean way to leave finishing stock, by deliberately entering a value slightly larger than the tool really is. Check first whether your control stores that register as a radius or as a diameter, because it decides how much stock you actually get. On Haas that is Setting 40, Tool Offset Measure, and when it is set to diameter the control shifts the path by half the value you enter. Put another way, an extra .010 in the register leaves .010 of stock on one machine and .005 on another.

Two habits keep compensation out of trouble. Turn it on and off in a linear move, never on an arc, and make the lead in move at least as long as the cutter radius. A lot of compensation alarms and gouged lead ins come from breaking one of those two rules.

Tool nose radius compensation is the turning equivalent. The tip of a turning insert is not a sharp point but a small radius, and on any taper or contour that radius causes the cut to deviate from the programmed path. Compensation corrects it, using the stored nose radius along with a tip orientation code that tells the control which way the insert faces. On a lathe the offset number comes from the second pair of digits in the T word rather than from a D word. On straight diameters and faces it makes no difference, which is why it is often the last thing an operator learns and the first thing blamed when a chamfer comes out wrong.

Work Offsets vs Tool Offsets: The Difference

This is the distinction that trips up most people learning a control, and it has a one line answer.

A work offset describes where the part is. A tool offset describes the tool doing the cutting.

Change the fixture, move the vise, or set the job up again next year, and the work offset changes while every tool offset stays valid. Swap a dull end mill for a fresh one and the tool offsets for that station change while the work offset is untouched. When a whole part comes out shifted in one direction, suspect the work offset. When one feature is wrong while everything else is fine, suspect the offset belonging to the tool that cut it.

Common Offset Mistakes

  • The next tool starting with no compensation, or with the last tool’s. Forgetting to cancel with G49 or G40 at the end of a tool is untidy and occasionally expensive, but it is usually survivable, because the next G43 H__ replaces the active length rather than adding to it. The crash that actually recurs is the mirror image: the next tool begins cutting with no G43 at all, or with the previous tool’s H number still in effect. Worth knowing separately, retract Z before commanding G49, because on many controls the cancel itself shifts Z by whatever value was sitting in the offset register.
  • H and D numbers that do not match the tool. Tool 7 running on H06 puts the tool out by the difference between the two stored lengths, which can be an inch or more if the two tools are nothing alike. Whether that is too deep or too shallow depends on which tool is longer. If H06 was never set at all the control applies no compensation whatever, so the programmed Z now applies to the spindle gauge line instead of to the tool tip. Which way that fails depends on how your shop measures lengths: touch off numbers leave the tool high and cutting air, presetter numbers leave it low by the whole length of the tool, and that second one breaks something. The program looks perfect on screen throughout.
  • Correcting geometry when you meant wear. It fixes today’s part and destroys the record of the tool’s real length.
  • Trusting an old offset after a holder change. A length is only as repeatable as the taper it was measured in. A damaged or worn holder makes a good number lie.
  • Using G92 in a shop that otherwise uses work offsets. It works, but on a Fanuc it leaves a shift the next operator will not find anywhere in the G54 to G59 table, and it survives a reset. Clear it with G92.1 X0 Y0 Z0. On a Haas the shift at least shows at the bottom of the Work Offsets page, and you clear it there, because Haas does not accept G92.1.

Frequently Asked Questions

What is a tool offset in CNC?
A tool offset is a stored measurement describing the cutting tool, most often its length and its diameter or nose radius. The program calls the offset by number so the same code runs correctly with whatever tool is actually loaded.
How many types of offsets are there in CNC?
There are five you will touch routinely: work offsets, tool length offsets, wear offsets, cutter radius compensation and tool nose radius compensation. The first two are set at setup, and wear is adjusted during the run. Older programs may also use G92 to shift the coordinate system.
What is the difference between G54 and G43?
G54 is a work offset and tells the machine where the part is. G43 applies a tool length offset and tells the machine how far the current tool sticks out of the spindle. A typical program uses both.
Why are there six work offsets, G54 to G59?
So one machine can hold several setups at once. Each fixture or vise gets its own offset, and the same cutting code can be called for each one without editing. Six is the Fanuc and Haas standard. Siemens gives you G54 to G57, and most controls offer extended registers when you need more.
What happens if I forget G49 or G40?
Compensation stays active into the next tool or move. It is often survivable, because the next G43 H replaces the active length offset rather than adding to it, but it is untidy and it can cut a profile in the wrong place. Retract Z before you command G49, since on many controls the cancel itself shifts Z by whatever value was sitting in the offset register.
Should a wear offset ever be large?
No. Wear corrections should be small. A large one means something else is wrong, such as a mistyped geometry value or the wrong tool in the station.

About Tool Holder Exchange

Tool Holder Exchange buys and sells used CNC tool holders and carbide tooling. If you have holders, collets or carbide sitting idle after a machine change or a shop closure, we buy carbide tooling and tool holders and can tell you what it is worth.