How Do You Set Work Part Zero on a CNC Machine?
This guide covers the sequence for setting cnc machine work part zero: edge finding, Z touch-off, work offset entry, and verification. It is written for operators and setup machinists, and it shows how to decide between an edge finder, a probe, and a dial indicator.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
What cnc machine work part zero actually means
Work part zero is the origin point the control uses for every coordinate in your program. It is not the machine home position and it is not the center of the stock by default. You choose it, then you tell the control where it sits in machine coordinates by writing values into a work offset such as G54.
The choice matters more than the measurement method. If the drawing dimensions from the top-left corner of the part, set zero there. If they run from a bore center, set zero on that bore. Setting zero somewhere convenient and then doing arithmetic in your head at the machine is how setups go wrong at 2 a.m.
Most shops keep three numbers per axis: the machine coordinate of the reference surface, the work offset that stores it, and the tool length offset that sits on top of it. Mixing up which one you are editing is the single most common cause of a crash on a new setup.
- 1G54 through G59Standard work offsets. Use one per vise jaw position or per operation.
- 2G54.1 P1 and upExtended offsets for pallets, tombstones, and 5-axis fixtures.
- 3G92 is not a work offsetIt shifts the coordinate system from the current position. Avoid it in setup.
Edge finder, probe, or indicator: which one to use
A mechanical edge finder is the default for one-off parts. Spin it at 500–800 rpm, feed in by hand until the tip kicks off center, then back off and move in 0.005 mm increments to find the exact kick point. Add or subtract half the tip diameter, typically 5 mm or 10 mm, depending on the model.
A spindle probe removes the arithmetic. The probe stylus touches the surface, the control records the position, and the offset page fills in with the radius already compensated. On a 16-position 5-axis cell, probing every part is the only way to hold ±0.005 mm across a batch without a full re-setup.
A dial indicator on a magnetic base or an indicator holder suits round parts and existing bores. Indicate the bore in two axes, split the difference between the high and low readings, and set zero on the center. This is slower than a probe but it also catches a bore that is out of round, which a probe will happily average into a wrong center.
- 1Edge finderBest for square corners on one or two parts. Cheap, no calibration.
- 2ProbeBest for repeats, castings, and anything with a tolerance under ±0.02 mm.
- 3IndicatorBest for bores, shafts, and verifying that a fixture has not moved.
Where to place zero on different part shapes
Rectangular plates are easy. Zero at the top-left corner with Z on the top face, so all X values are positive and all Y values are negative. That matches the way most CAM software posts code and it keeps the operator from flipping a sign.
Round parts get zero at the center of the largest turned diameter or the main bore. If the part has a bolt circle, use the circle center too. Setting zero on the outside edge of a round part means every hole coordinate carries a radius offset that nobody will remember at inspection.
Castings and weldments need a datum that exists before machining. Rough stock surfaces move by 1–3 mm, so zero on a machined pad or a fixtured pin, not on the raw casting skin. If you zero on a rough surface, the first facing pass will cut unevenly and the finished part will be thin on one side.
On 5-axis work, zero usually lives at the center of the rotary table, not on the part. The CAM post handles the transform from table center to part origin. Chasing zero on the part itself costs an hour and gains nothing.
- 1PlatesTop-left corner, Z on the top face.
- 2Round partsCenter of the main bore or turned diameter.
- 3CastingsA machined pad or fixtured pin, never the raw skin.
- 45-axisRotary table center, transformed in CAM.
Mistakes that move cnc machine work part zero
Thermal growth is real. A spindle that has run for two hours is longer than a cold one. On a machine cutting to ±0.005 mm, warm up the spindle for 15–20 minutes before you touch off Z, or accept that your first ten parts will run high.
Chips under the part are the classic one. A 0.05 mm chip under a corner lifts that corner by 0.05 mm, and the offset you set is now wrong by that amount. Blow off the vise jaws and the part face before every touch-off, not just the first one of the day.
Tool length offsets and work offsets are separate pages. If Z reads 0.000 in the work offset but the tool is still 80 mm above the part, the tool length offset is missing or was entered in the wrong register. Check both pages before you press cycle start.
Finally, a loose edge finder or a probe stylus with a bent tip gives you a number that looks clean and is off by 0.1 mm. Run the probe calibration cycle at the start of every shift, or at minimum once a week.
- 1Cold spindleWarm up 15–20 minutes before touching Z.
- 2Chips under the partA 0.05 mm chip becomes a 0.05 mm offset error.
- 3Wrong offset pageTool length and work offset are not the same thing.
- 4Bent stylusCalibrate the probe weekly, or every shift on tight work.
Step by step: setting cnc machine work part zero
Sequence for a typical vertical mill with a vise and a square plate. Adjust the numbers for your machine and control.
- 1Clean the fixture and the partWipe the vise jaws, the parallels, and the bottom face of the stock. Blow air across the jaws. Any chip or burr at this stage becomes a zero error you will chase for an hour.
- 2Load the edge finder and spin it upChuck the edge finder, start the spindle at 500–800 rpm. Bring it close to the X face by hand in 0.01 mm steps until the tip kicks off center, then back off and re-approach in 0.005 mm increments to find the exact point.
- 3Enter the X offset with the radiusNote the machine X coordinate at the kick point, then subtract or add half the tip diameter. For a 10 mm tip touching the left face, add 5 mm. Write the result into G54 X and confirm the number on screen.
- 4Repeat for YMove to the front face and repeat the same procedure. Enter the compensated value into G54 Y. Do not skip the re-approach step; the first kick point is always a few microns early.
- 5Touch off Z on the top faceLoad the shortest tool in the program, or use a gauge block. Jog down in 0.01 mm steps until the tool just marks a sheet of paper or the gauge block drags. Enter the machine Z into G54 Z, then verify the tool length offset is loaded.
- 6Verify with a rapid moveIn MDI, command G0 G54 X0 Y0 Z25. Watch the machine position readout. X0 Y0 should sit at the corner you chose, and Z25 should be 25 mm above the top face. If anything looks wrong, re-measure before cutting.
- 7Cut a test featureRun a shallow facing pass or a spot drill at the corner. Measure the result with calipers or a height gauge. If it is off by more than 0.02 mm, adjust the offset and repeat. Do not adjust the program.
- 8Record the numbers on the setup sheetWrite the G54 values, the tool numbers, and the date on the setup sheet that travels with the job. The next operator will thank you, and the next run of the same part will start from a known place.
Choosing a method for cnc machine work part zero
Match the method to the batch size, the tolerance, and the part shape. A probe is not always the right answer.
| Method | Typical accuracy | Best for | Watch out for |
|---|---|---|---|
| Mechanical edge finder | ±0.01 to ±0.02 mm | One-off plates and simple corners | Spindle speed and tip diameter errors |
| Spindle probe | ±0.002 to ±0.005 mm | Batches, castings, tight tolerances | Needs calibration and a clean surface |
| Dial indicator | ±0.005 mm | Bores, shafts, round parts | Slow, and it averages out-of-round bores |
| Gauge block on Z | ±0.005 mm | Any Z touch-off on a flat face | Block thickness and chip entrapment |
| Tool touching paper | ±0.05 mm | Rough setups and first articles | Paper thickness varies by brand and humidity |
Get the zero right before the first cut
Manual edge finding is fine for one or two parts. For batches, castings, or any tolerance under ±0.02 mm, probe the part and record the numbers on the setup sheet. If your drawing dimensions from a corner, zero on that corner, not on a convenient face.
Frequently asked questions
Can I set cnc machine work part zero without an edge finder?
Yes. A dowel pin or a ground rod in a collet works. Spin it at low rpm and approach the face until a 0.02 mm feeler gauge will not pass. Note the coordinate, then subtract half the pin diameter.
The accuracy is around ±0.02 mm, which is fine for most first operations but not for a finished bore position. For anything tighter, use a probe or an indicator.
Why does my Z zero change after a tool change?
Most likely the tool length offset is wrong or was not loaded. Work offset and tool length offset are separate registers. Check the tool length page against the setup sheet.
A second cause is a pull-out or a loose collet. Mark the tool shank and the holder with a paint pen, run a few cuts, and see if the mark has moved.
Should I set zero on the stock or on the finished surface?
Set it on the surface the drawing dimensions from. If the print is dimensioned from the finished top face, zero on the finished top face, even if that means calculating the stock allowance before the first cut.
Zeroing on the stock is faster but it means every Z depth in the program needs a manual correction. That correction is where the error creeps in.
How often should I re-verify cnc machine work part zero?
At the start of every shift, after any crash or alarm, and after a fixture change. If you are running a batch of parts on the same setup with no changes, verifying once a day is usually enough.
On 5-axis work or any job with a tolerance under ±0.01 mm, probe the part before each cycle. The extra 30 seconds is cheaper than a scrapped casting.
Does a 5-axis machine need a different zero procedure?
The measurement steps are the same, but the zero usually lives at the rotary table center. The CAM post transforms from table center to the part origin, so you set the table center once and let the software handle the rest.
If you set zero on the part itself on a 5-axis machine, every rotation of the table moves your origin in machine coordinates. That is a recipe for a crash.
What tolerance can I realistically hold after setting zero?
Manual edge finding with a good edge finder holds about ±0.02 mm on position. A calibrated spindle probe holds ±0.005 mm or better.
The zeroing method is only one part of the total error stack. Thermal growth, fixture rigidity, and tool deflection all add to it. Getting zero right removes one error source, not all of them.
Send us your part and we will set the zero
Upload a STEP file and a drawing. We reply with a quotation and a free DFM analysis within 12 hours, and production can start within 24 hours of approval.
12-hour quote100% inspectionNo minimum order quantityNDA on request
More setup notes from the floor
We publish setup notes, tooling trials and inspection data from the factory floor.
