How Many Types of Offset in CNC Machine Control?
Five corrections cover almost every job we run: work offset, tool length, cutter radius, wear and fixture position. This guide shows what each one corrects, how to set it on a Fanuc or Siemens control, and which numbers to trust when a part comes out of tolerance.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
How many types of offset in CNC machine control exist?
In practice we work with five corrections, and they map to five different questions on the shop floor. Where is the part? How long is the tool? How wide is the tool? How far has the tool worn? Where does the fixture sit? Each question gets its own register in the control, and mixing them up is the most common cause of a scrapped first part.
Work offset answers the first question. It defines the part origin in the machine coordinate system, usually G54 through G59. Set it from an edge finder, a 3D taster or a probe, and the program can use X0 Y0 Z0 at a corner or at the center of a bore.
Tool length offset compensates for the difference in length between holders. Tool 1 may be 120 mm longer than tool 8. Without a length value the control has no idea where the tip is, and the first rapid move will drive it into the stock.
Cutter radius offset tells the control the actual radius of the cutting tool, so the programmed path describes the finished contour and not the centerline. Wear offset is the small trim an operator adds after measuring a part. Fixture offset covers pallets, tombstones and vise jaws that move between setups.
That is the full count for a standard 3-axis mill. Multi-spindle lathes add a few more registers for each turret station, but the logic stays the same: one number per physical reality.
- 1Work offsetG54–G59, part zero in machine coordinates.
- 2Tool length offsetH register, one per holder.
- 3Cutter radius offsetD register, actual tool radius.
- 4Wear offsetSmall trim added after inspection.
Work offset and tool length offset: setting the numbers
Start with work offset. Touch off the X and Y faces with a 10 mm edge finder at 600–800 rpm, or use a 3D taster and zero the dial. For Z, touch the top of the stock with a 20 mm gauge block or set the tool directly on the surface. Store the values in G54 and confirm the display reads the same as your setup sheet.
For tool length, load each holder into the spindle and bring the tip down to a known Z reference. The two common methods are the touch-off method and the gauge-line method. Touch-off is faster on a job shop; the gauge line is more repeatable on a production cell because it removes the operator from the measurement.
A presetter gives better numbers. Measure each tool offline, write the length to the holder chip or a setup sheet, then load the values into the H registers. On a 16-tool job that saves 20–40 minutes of spindle downtime and removes most of the human error.
One rule we enforce: never edit a length offset while the tool is in the cut. Stop the spindle, retract to a safe Z, then change the register. Editing on the fly is how a rougher ends up 3 mm deep in a pocket wall.
- 1Edge finder speed600–800 rpm for a 10 mm tip.
- 2Probe routineUse for batches above 20 parts.
- 3PresetterOffline measurement, values written to H registers.
Cutter radius offset and wear offset: keeping size in tolerance
Cutter radius offset is what lets you program the part, not the toolpath. On a Fanuc control it lives in the D register and is activated with G41 for the left side of the path or G42 for the right. Get the side wrong and the cutter walks into the wall, usually on the first lead-in move.
The radius value should be the real radius of the tool, measured with a micrometer or a tool presetter, not the nominal size printed on the box. A 12 mm end mill can measure 11.94 mm after regrinding. If the register still says 6.00 mm, every contour will come out 0.06 mm small.
Wear offset is the trim on top of radius. After the first part is inspected, add the difference between measured and nominal size to the wear column. On a 50 mm bore that reads 49.96 mm, add 0.02 mm to the wear value and the next part should land on size.
Keep the two separate. If you correct size by editing the radius, the next regrind resets the whole geometry and your trim disappears. Wear is the adjustment layer, radius is the physical truth of the tool.
- 1G41 left, G42 rightMatch the side to the cut direction.
- 2Measure the real radiusReground tools shrink by 0.03–0.08 mm.
- 3Wear is the trim layerKeep it under 0.05 mm per adjustment.
Fixture offset and multi-setup work
Fixture offset matters when the same program runs on a tombstone, a pallet or a second vise. Instead of rewriting the program, you store the shift in a separate work coordinate such as G55 for the second station. The program stays the same; the origin moves.
On a 4-axis or 5-axis machine the rotary centerline is part of the setup. Measure the center of the rotary table, store it as a reference, and use it to calculate the part position for each angle. If the centerline is off by 0.1 mm, every angled feature will be off by the same amount.
Pallet systems reward good bookkeeping. Number each pallet, keep a printed sheet of its G54 values, and re-verify with a probe after every changeover. We see fewer crashes on pallet jobs than on one-off vises, because the numbers are documented instead of remembered.
For small batches, a simple vise with soft jaws and a single G54 is faster. Fixture offsets pay off when the setup repeats more than a few times per week, or when the part is too large to move without re-indicating.
- 1G55 for station twoSame program, shifted origin.
- 2Rotary centerlineMeasure and store before angled features.
- 3Pallet sheetDocumented values beat memory.
Step by step: setting the five offsets safely
- 11. Clean and load the fixtureStone the vise jaws or tombstone, remove chips from the locating faces, and torque the clamps to the fixture sheet value. A chip under a jaw can tilt a part by 0.05 mm over 100 mm.
- 22. Set the work offsetTouch X and Y with an edge finder at 600–800 rpm, then Z on the stock top with a gauge block. Store in G54 and write the values on the setup sheet.
- 33. Measure every toolUse a presetter or touch off each holder at the gauge line. Load the lengths into the H registers and check that the active tool number matches the program.
- 44. Enter cutter radiusMeasure the real radius of each cutter, including reground tools, and store it in the D register. Do not leave the nominal box size in the control.
- 55. Zero the wear columnsClear all wear values before the first part. A leftover 0.1 mm trim from the previous job will scrap the new one on the first pass.
- 66. Dry run in single blockRun the program with the tool 20–50 mm above the stock, feed override at 0, and watch the distance-to-go display on every approach move.
- 77. Cut and measure the first partTake a light first pass, check the critical dimensions on the CMM or with a micrometer, then apply wear offsets only where the size is out.
- 88. Record and lock the setupWrite the final values on the setup sheet, back up the offset file, and set a control lock or password if the machine supports it.
Offset type comparison
| Offset type | Typical register | What it corrects | When to adjust |
|---|---|---|---|
| Work offset | G54–G59 | Part zero in machine space | New fixture or new part position |
| Tool length | H register | Difference in holder length | Tool change or new holder |
| Cutter radius | D register | Actual tool radius | New or reground cutter |
| Wear | Wear column | Small size trim after inspection | After measuring the first part |
| Fixture | G55 or pallet sheet | Shift between stations or pallets | Changeover to a second station |
Set the five offsets, then cut
Work offset, tool length, cutter radius, wear and fixture position cover nearly every setup we see. Get them right and the first part lands on size.
Frequently asked questions
How many types of offset in CNC machine control do I need to learn first?
Learn work offset and tool length offset first. Those two keep the tool out of the fixture and off the table.
Cutter radius and wear come next, once you start holding size on a contour. Fixture offset is a batch-production topic and can wait until you run multiple stations.
Why did my part come out 0.1 mm oversize?
Check the wear column before anything else. A leftover trim value from the previous job is the most common cause.
If wear is zero, measure the cutter radius. A reground tool that still carries its nominal radius in the D register will cut oversize on every contour.
Can I set offsets while the spindle is running?
No. Retract to a safe Z, stop the spindle, then edit the register.
Editing a length or radius value during a cut changes the geometry mid-path and will usually break the tool or scrap the part.
Do I need a tool presetter for accurate offsets?
Not for one-off work. A gauge block and a dial indicator are enough to hold ±0.02 mm on most jobs.
A presetter pays back on batches above 20 parts or on machines with 16 or more tools, because it removes spindle downtime and operator variance.
How do I handle offsets on a 5-axis machine?
Add the rotary centerline to the setup. Measure the table center, store it, and use it to calculate the part position at each angle.
Work offset still sets the part origin. The rotary reference sits on top of it, and both need to be correct before the first angled cut.
What tolerance can I expect after offsets are set correctly?
On our 5-axis and mill-turn centers we hold ±0.005 mm on critical features when the setup is verified with a probe.
Surface finish on a well-controlled setup lands between Ra 0.8 and 1.6 μm, or Ra 0.2–0.8 μm after fine finishing.
Need parts cut with verified offsets?
Send your drawings and we will quote within 12 hours, with a free DFM review on the first pass.
12-hour quote±0.005 mm tolerance100% inspectionNo minimum order
More from GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
