How to Find Part Offsets CNC Machine
A shop-floor walkthrough for machinists and process engineers. You will learn how to find part offsets cnc machine setups need, with an edge finder, a dial indicator or a spindle probe, what tolerance each method holds, and when a setup should be re-datumed instead of trusted.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
What a part offset stores and why it decides the run
A part offset is a set of numbers held in the control that defines where program zero sits relative to machine home. On a Fanuc-style control these live in G54 through G59; on a Siemens control they are the work offset table. Once you find part offsets cnc machine coordinates and store them, every commanded move is measured from that stored point, not from the table.
The stored value has three components. X and Y place the datum corner or center in the work envelope. Z sets the top face that all depths reference. A fourth value, the work offset number called by the program, decides which set the control reads. Get the number wrong and the machine cuts in the right shape at the wrong place.
Offsets also carry a rotary component on 4-axis and 5-axis work. The rotary table center and the tilt pivot must be known before the part offset means anything, which is why a 5-axis setup is usually proved with a probe rather than an edge finder.
The practical consequence is simple. Offset error is a constant shift. If X is off by 0.05 mm, every feature on every part is off by 0.05 mm in the same direction. That is why setup time is not wasted time.
Prepare the machine and the blank before you touch off
Clean the table, the vise and the part before any measurement. A chip under a vise jaw lifts the part by 0.02–0.05 mm and shows up later as a taper. Stone any burr on the part edges, especially on saw-cut faces, because a burr pushes an edge finder off by its own height.
Warm the spindle. A cold spindle grows 0.02–0.04 mm in Z over the first 30 minutes at 8,000 rpm. For work holding ±0.01 mm, run a 15-minute warm-up cycle or leave the machine running between setups.
Check that the vise or fixture is parallel to the X axis with a dial indicator on the fixed jaw. Aim for 0.01 mm over 150 mm. If the jaw reads 0.03 mm, fix the vise before you find part offsets cnc machine values, or the error is baked into the run.
Confirm tool length offsets separately. Part offsets locate the part; tool offsets locate the tool. Mixing the two is the most common cause of a first part cut 2 mm too deep.
Pick the method that matches your tolerance
Three methods cover most work. A mechanical edge finder is fast and cheap and holds about ±0.02 mm in experienced hands. A dial indicator on a magnetic base or an Indicol holder holds ±0.01 mm and is the right choice for bores and finished edges. A spindle-mounted touch probe holds ±0.005 mm and repeats without operator feel.
Choose by the tightest feature on the print, not by habit. If the drawing calls out ±0.05 mm on a hole position, an edge finder is enough. If it calls out ±0.01 mm true position, indicate the datum or probe it. If the part has a bore datum, never use an edge finder on the outside of the boss.
For production runs above roughly 50 parts, a probe pays for itself. It removes the operator-to-operator variation and lets a second shift reproduce the first shift's setup from stored values.
For one-off prototypes in soft material, the edge finder is still the fastest route, provided you verify the first feature with a caliper or a gauge before cutting the rest.
Verify the offset before you cut metal
After storing X, Y and Z, run the program in single block with the feed override low and watch the distance-to-go display on the first approach move. Distance-to-go should match the print within your tolerance. If it does not, stop and re-check the offset value rather than adjusting the program.
Dry run above the part with a 5–10 mm clearance plane. On a 3-axis job this catches a wrong Z or a missing fixture clearance. On a 5-axis job, dry run with the rotary axes in the actual cutting position, because the part can swing into the table or the trunnion.
Cut the first feature and measure it. Compare the measured position to the print. A consistent shift of 0.03 mm across features means the offset needs a small correction; a random spread across features means the setup is moving and the fixture needs attention.
Record the final offset values, the tool numbers and the probe stylus used in the setup sheet. The next operator should be able to repeat the job without re-deriving anything.
How to find part offsets cnc machine step by step
- 11. Clean and load the partWipe the table, vise jaws and part faces. Seat the part against the fixed jaw and the stop. Tighten in two passes to about 60–70% of final torque so the part does not creep.
- 22. Indicate the vise or fixtureSweep the fixed jaw with a dial indicator. Target 0.01 mm over 150 mm. Tap the vise into alignment, then finish the clamping torque.
- 33. Establish the machine referenceSend the machine to home or a known reference position with G28 or G53. Confirm the position display reads the expected values before you start.
- 44. Locate X and YEdge finder: run at 500–800 rpm, approach at 0.02 mm steps, and subtract or add half the tip diameter (typically 5 mm or 10 mm). Indicator: sweep the datum edge and zero on the lowest reading.
- 55. Touch off ZUse a gauge block or a 50 mm tool setter on the true top face. Remove the block thickness from the reading. Never touch off on a saw-cut skin or a burr.
- 66. Store and label the offsetWrite X, Y and Z into G54 or the offset the program calls. Note the datum corner and the direction of the half-tip compensation in the setup sheet.
- 77. Verify with distance-to-goRun the first approach in single block at 25% rapid. Compare distance-to-go with the print. Re-check the offset if the difference exceeds 0.02 mm.
- 88. Cut, measure, correct onceCut a test feature, measure it, and apply a single correction. Do not chase the reading with repeated small edits.
Edge finder, indicator or probe
Tolerance figures are what each method holds in normal shop conditions, not the best case.
| Method | Typical accuracy | Best for | Watch out for |
|---|---|---|---|
| Mechanical edge finder | ±0.02 mm | Prismatic edges, one-offs, soft material | Tip runout and operator feel |
| Dial indicator | ±0.01 mm | Bores, finished edges, rotary centers | Magnetic base slip and stylus deflection |
| Spindle touch probe | ±0.005 mm | Production runs, 5-axis, bore datums | Stylus ball wear and dirty contact faces |
| Gauge block on Z | ±0.01 mm | Flat top faces and depth references | Chips under the block |
| Tool setter on Z | ±0.005 mm | Repeat Z across many tools | Wrong tool number loaded |
Match the method to the print
If the tightest callout is looser than ±0.05 mm, an edge finder is enough. If it is ±0.01 mm true position, indicate or probe. Do not spend 40 minutes probing a bracket that a 3-minute edge finder can locate.
Common questions
How do I find part offsets cnc machine setups without a probe?
Use an edge finder for X and Y and a gauge block for Z. Run the edge finder at 500–800 rpm and approach the edge in 0.02 mm steps so the tip kicks out cleanly.
Compensate for half the tip diameter in the direction you approached, then verify the stored value with a distance-to-go check before cutting.
Should I use G54 or G55 for a second vise?
Give each vise or fixture its own offset number. G54 for the first, G55 for the second, and so on.
Keep a written list of which offset belongs to which fixture. Programs that call the wrong offset cut a correct shape in the wrong place.
Why does my first part come out shifted every time?
A consistent shift points to the offset value, a random spread points to the fixture. Check for chips under the part and for a vise jaw that is not square to the X axis.
If the shift changes with spindle speed, the spindle is growing in Z and the setup needs a warm-up cycle.
How often should offsets be re-checked?
Re-check at the start of every shift and after any crash, tool change error or power interruption. On long runs, probe the datum every 20–30 parts.
Store the values in the setup sheet so a re-check is a comparison, not a fresh measurement.
Can I copy offsets from one machine to another?
No. Offsets are machine-specific because they reference that machine's home position.
Transfer the datum strategy and the method, then re-measure on the second machine.
What tolerance can GreatLight hold on a datum-critical part?
We work to ±0.005 mm on high-precision parts and inspect 100% before shipment, with reports on request.
Fixture design and datum strategy are reviewed during the DFM step, which runs within 12 hours of quoting.
Send us the print and the datum plan
Upload your CAD and we will return a quote and a DFM review within 12 hours, including a note on which datum features we would use for the setup.
12-hour quote100% inspection±0.005 mm tolerance
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
