How to Use the Position Record Button on a CNC Machine
The position record button CNC machine operators rely on stores the current axis values so you can reuse them as work offsets, fixture references, or retract points. This guide is written for operators, setup techs, and process engineers who need repeatable setups. After reading it, you will know which coordinate system to record, how to verify the stored value, and when the button is the wrong tool for the job.
Key takeaways
What the position record button CNC machine function actually stores
Every CNC control keeps several coordinate sets running at the same time. Machine coordinates are fixed to the home switch. Work coordinates shift with the active offset, usually G54 to G59. Relative coordinates are a scratch register you can zero anywhere. The position record button CNC machine function copies the numbers currently shown on the active display into a register you choose.
That last part matters. The button does not measure anything and it does not touch the tool. It is a copy command. If the display is showing relative coordinates and you write them into G55, you have stored a number that means nothing to the machine. Read the display label before you press the soft key.
Most controls label the key as POSITION RECORD, POSI REC, RECORD, or a small icon near the offset page. Fanuc keeps it inside the offset/setting page. Siemens 828D and 840D place it near the work offset table. Haas puts it on the offset page as a function key. The path differs, the idea does not.
- 1Machine coordinatesUse for soft limits, travel checks, and parking positions.
- 2Work coordinatesUse for G54-G59 offsets, fixture origins, and second-op datums.
- 3Relative coordinatesUse for step-and-repeat distances, not for offsets.
Where this function saves time on real parts
The classic use is a fixture that comes off and goes back on. If the vise or tombstone locates on dowel pins, you can record the fixture origin once, store it in G55, and recall it next run. The pins repeat, the offset repeats. On a 4,000 mm bed with several stations, that saves an hour of edge finding per setup.
The second use is the safe retract point. Jog the spindle to a clear spot above the fixture, record the machine coordinates, and write them into the tool change macro or the program end block. Now every tool retracts to the same place. No more crashed probes on the way home.
The third use is deep-cavity or long-reach work. When a tool has to enter a pocket at an angle, record the entry point in relative coordinates, then move the axes there by hand and watch the distance-to-go. This is faster than typing a G0 line and safer than trusting your memory of the drawing.
It is a poor fit for first-article datums on a new part. If the datum is defined by a bore or a face you have not indicated yet, record after indicating, not before. Recording a rough position and then touching off the same feature will give you two different numbers and no way to tell which one is right.
Checks to run before every record
Confirm the active work offset. The offset page shows which G-code is live, but the display sometimes follows the last one you selected, not the one the program will call. Check M-code and G-code state at the top of the screen.
Confirm the units. A machine in inch mode will happily record 0.3937 where you expected 10.000. Mixing inch and metric offsets is one of the most common setup errors, and it usually shows up as a tool buried in the stock.
Confirm the tool length offset is cancelled or correct. If you record a Z position while a tool length offset is active, the stored Z includes that offset. Load the next tool and the number is wrong by the offset amount. Cancel G43 before recording Z.
Confirm the axes are not drifting. On an older machine, a loose coupling or a failing encoder can move the display a few microns while you stand still. Watch the display for 10 seconds. If the last digit keeps walking, fix the machine before you trust the number.
Step by step: using the position record button on a CNC machine
The sequence below works on Fanuc, Siemens, and Haas controls. Menu names differ, order does not.
- 1Set the mode and cancel compensationSwitch to JOG or HANDLE mode. Cancel cutter comp and tool length comp (G40, G49). Confirm the units (G20 or G21) match the drawing.
- 2Select the coordinate display you wantPress POS or the position key and page to the set you need: ABS (work), REL (relative), or MACHINE. The label at the top of the display tells you which one is active.
- 3Jog to the target pointUse the handwheel at ×10 or ×100 for the approach, then ×1 for the last 0.5 mm. For a fixture origin, touch the pin or the stop face with a dial indicator and zero the indicator.
- 4Open the offset or register pageGo to the work offset table (G54-G59) or the common variable page. Highlight the register you intend to write. On Haas, press the OFFSET key; on Fanuc, press OFFSET/SETTING.
- 5Press the position record button CNC machine soft keyThe control fills the highlighted register with the current values of the active display. On most controls the axis letters flash once to confirm. If nothing changes, the display and the register do not match.
- 6Verify the number by re-reading itMove off the point by 20-50 mm, then use RESTORE or a G0 move to return. The distance-to-go should read 0.000 in all recorded axes. A mismatch means the offset was written to the wrong register.
- 7Dry run the first approachRapid to Z +50 mm above the part, then feed down at 50-100 mm/min with your hand on the feed hold. Watch the position display, not the tool.
- 8Re-record anything you joggedIf you touched the handwheel after recording, the stored value is stale. Re-record that axis before the next cycle.
Which coordinate set to record, and when
Pick the row that matches your task. Wrong row, wrong number.
| Task | Record this | Where it goes | Typical error |
|---|---|---|---|
| Fixture origin for repeat setups | Work (ABS) | G54-G59 offset | Stored while a different offset was active |
| Safe retract above the vise | Machine | Program end block or macro | Uses work coords, moves with the offset |
| Step-and-repeat pitch | Relative (REL) | Operator notes or macro | Written into an offset register |
| Second-op datum after flipping | Work (ABS) | G55 or G56 | Old Z offset left active |
| Soft limit or travel check | Machine | Setup sheet only | Confused with part zero |
| Probe stylus entry point | Work (ABS) | G54 with probe active | Tool length offset still live on Z |
Record, verify, then cut
The position record button is a copy command, not a measurement. Treat it that way: store into the correct register, prove the number with a distance-to-go check, and dry run the first approach. Skip any of those three and the first part becomes the setup gauge.
Questions operators ask about the record function
The button does nothing when I press it. What is wrong?
On most controls the record key only writes into a register that is already highlighted and in edit-enabled state. If the offset page is in a read-only or protected mode, the key is ignored.
Check three things: the parameter write protect key, the active display page, and whether you are on an offset table that accepts input. On Fanuc, look for the PWE setting. On Haas, confirm the setting page is not locked.
Can I record a position while the spindle is running?
Yes, but there is rarely a good reason to. The recorded value is a snapshot of the display at the moment of the press, and a moving axis will give you a number that is already stale by the time the tool reaches the next block.
If you need a point during a cycle, use a program stop (M0) or an optional stop, jog to the point, record, then resume. Recording on the fly is how people store a Z value 2 mm off from where they thought it was.
Why is my stored Z value different from what the display showed?
Almost always because a tool length offset was active. The display shows the compensated position, and the record function stores what the display shows.
Cancel G49 before you record Z, or record with the same tool loaded that the program will use for that operation. Do not mix the two approaches in one setup.
Do I need to re-record after changing a fixture or a jaw?
Yes, unless the fixture locates on hardened pins or a dowel pattern that you have verified with an indicator. A vise jaw moved by 0.02 mm shifts the datum by 0.02 mm, and the stored offset will not know.
Re-indicate the datum, record again, and dry run the first approach. On tight-tolerance parts at ±0.005 mm, that check is not optional.
How does this compare with using a touch probe?
A probe measures the feature and writes the offset automatically, which removes the handwheel and the reading error. The record button is still useful for retract points, parking positions, and any location that is not defined by a surface you can touch.
Many shops use both: probe for the datum, record for the safe positions. The two do not conflict as long as you keep the probe calibration current.
What should be on the setup sheet after recording?
The offset register used, the axis values stored, the tool number and length offset, and the date. Add a note if the fixture was re-indicated.
A setup sheet that lists G54 X, Y, Z with three decimal places lets the next operator reproduce the setup in minutes. A sheet that says see machine memory does not.
Send us the part, we will send back the process
Upload your model and drawings. We return a quotation with free DFM analysis within 12 hours, and production can start within 24 hours. No minimum order quantity, from one prototype to 10,000+ parts.
12-hour quote100% inspectionNDA on request
More setup and machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
