Setup fundamentals

CNC Table Point Setup Guide: Work Offsets That Hold ±0.005 mm

Every dimension on the print traces back to one thing: where the machine thinks the part sits. This guide walks through a repeatable CNC table point setup for 3-axis and 5-axis mills, from vise prep to verified offsets. Read it to judge which method fits your part, and where cheap shortcuts will cost you a rework.

Get Instant Quote Talk to an Engineer

±0.005 mm5-axis capable100% inspection

CNC table point setup on a grey mill with a vise and indicator

On this page

1
Key takeaways
2
What CNC table point setup actually controls
3
Choosing a datum that survives the second operation
4
Probing, edge finding, and when each is good enough
5
Common pitfalls that scrap parts
6
Step by step: a repeatable table point setup
7
Which setup method fits your part

Quick answer

Key takeaways

Offsets are the whole gameG54–G59 tell the control where the part sits. Get them wrong and every feature shifts together.

Pick the datum before the soft jawsDecide X0 Y0 Z0 from the print and the fixture, not from whatever face is easiest to reach.

Indicate, don't eyeballA dial test indicator at 0.01 mm resolution beats any visual alignment on a vise jaw.

Verify twice, cut onceDry-run the first tool and check the offset with a gauge block or probe before the first cut.

Rotation needs its own offsetOn 4-axis and 5-axis work, a tilted table adds error that a single work offset cannot absorb.

Section 1

What CNC table point setup actually controls

Table point setup is the link between the CAD model and the physical blank. The CAM software writes toolpaths around a coordinate system. The machine knows nothing about that model until you tell it where the origin sits in machine coordinates. Work offsets G54 through G59 do that job. Set them, and the tool goes where the program says. Miss by 0.1 mm, and every hole in the part misses by the same 0.1 mm.

People sometimes treat this as a first-day skill and move on. That is a mistake. On a 3-axis mill with a single vise, one offset is usually enough. Add a rotary table, a second operation, or a tombstone with four parts, and the offset structure becomes the difference between a 99.99% pass rate and a scrap bin. We see this constantly on tight-tolerance work, where a misplaced datum shows up as a bolt pattern that will not seat.

The setup has three parts. First, physical location: the blank sits square and stable in the fixture. Second, the datum decision: which corner or feature becomes X0 Y0 Z0. Third, the verification: an independent check that the control agrees with reality. Skip any one and the other two will not save you.

1
Work offsetG54–G59 store the part origin in machine coordinates.
2
DatumThe print feature that defines X0, Y0, Z0.
3
VerificationA gauge block, indicator, or probe check before cutting.

Section 2

Choosing a datum that survives the second operation

A datum is only useful if it still exists when you need to re-reference the part. On a simple plate, the finished left edge and top face work fine. On a part that gets flipped for the second op, the first-op faces may be machined away or covered by chips. In that case, pick a datum from a feature that stays untouched, or plan a reference pad that you cut off at the end.

For a cnc table point setup on a 5-axis machine, the datum often needs to sit at the rotary center. That means the offset is not just X, Y, Z. You also need the pivot point of the trunnion or table, and the tool center point offset. If the pivot is off by 0.02 mm and you run simultaneous motion, the surface finish will ripple and the profile will drift. On our 16 simultaneous 5-axis centers we treat the pivot as a calibration item, checked before a long run, not a one-time number.

There is a practical test for any datum choice. Ask: if I come back to this part tomorrow with a fresh setup, can I find the same zero within 0.01 mm? If the answer is no, the datum is too vague. A sharp corner is better than a blended edge. A ground face is better than a saw cut. A bored hole is better than a drilled one.

Section 3

Probing, edge finding, and when each is good enough

Edge finders are cheap and fine for general work. Spin the tip at 500–1,000 rpm, touch the edge until it kicks off, and add half the tip diameter. On a 10 mm tip that is 5 mm. The accuracy is around 0.02–0.05 mm depending on feel and spindle speed. That is acceptable for a bracket with ±0.1 mm tolerances, and not acceptable for a bearing bore.

A dial test indicator on a magnetic base gives 0.01 mm resolution and lets you sweep a face or bore. This is the standard method for aligning a vise or a fixture to the X axis. Sweep the fixed jaw and adjust until the needle moves less than half a division over the jaw length. For a 150 mm jaw, holding 0.01 mm total movement means the jaw is square to within about 0.004 degrees.

A spindle probe is faster and repeatable. Touch off on six points and the control calculates the face and its angle. On production runs, probing the fixture once per shift catches thermal drift and chip buildup. The offset is only as good as the probe calibration, so re-calibrate the stylus after any crash, no matter how small. A bent stylus can read 0.03 mm off and still look fine on the screen.

1
Edge finder0.02–0.05 mm. Good for ±0.1 mm features.
2
Dial indicator0.01 mm. Best for vise and fixture alignment.
3
Spindle probe0.005–0.01 mm. Best for production and 5-axis pivots.

Section 4

Common pitfalls that scrap parts

The first pitfall is a datum that moves between operations. If the first op machines the face you used as Z0, the second op has no reliable Z reference. Plan the process so at least one datum face survives, or add a sacrificial reference pad. On parts with a tight flatness callout, this is not optional.

The second is thermal drift. A spindle that has run for two hours is not the same length as a cold one. On a long run, the Z offset can move 0.01–0.03 mm. Re-probe after warm-up and at shift changes. If the shop is not temperature controlled, expect more drift in summer. We run 100% inspection before shipment for this reason, and in-process checks catch drift before it becomes a batch problem.

The third is chip contamination under the part. A single aluminum chip 0.05 mm thick under a corner will tilt a 200 mm part by roughly 0.015 mm across its length, and more if the chip sits near one edge. Clean the fixture between every part on a production run. Air blast is not enough on castings with sticky chips.

The fourth is a wrong offset sign or wrong work offset call. A program that calls G55 while the setup is in G54 will cut air or crash. Put the active work offset in the program header and on the setup sheet. Dry-run the first approach move every time the program changes.

Procedure

Step by step: a repeatable table point setup

1
Clean and stone the table and fixtureWipe the table, then stone any burrs on the vise base and the part's locating faces. A 0.02 mm chip under a vise will tilt the part and you will chase the error all day. Torque the vise bolts in a cross pattern to the maker's spec, usually 40–70 N·m for a 150 mm vise.
2
Seat the blank and confirm contactPush the part against the fixed jaw and down onto the parallels. Tap with a soft mallet, then check the parallels slide with light drag. For thin parts use three or more support points. Never rely on the movable jaw to pull the part flat.
3
Indicate the fixture or part faceSweep the fixed jaw or a machined face with a dial test indicator. Target under 0.01 mm total movement over the length you sweep. If it is out, loosen, tap, and re-torque. Do not compensate with a rotated work offset unless the part is genuinely angled.
4
Set X and Y zeroUse the probe or edge finder on the chosen datum edges. Enter the values into G54. For a corner datum, touch both edges. For a bore datum, probe four points and let the control compute the center. Record the numbers in the setup sheet.
5
Set Z zero on a known surfaceTouch the tool to a gauge block or the top of a known parallel. If using a 50 mm gauge block, subtract 50 mm from the machine position. Set Z0 on the face the CAM program expects, and mark whether the program uses the top of stock or the finished face.
6
Verify with an independent checkMove to a known feature and compare the machine position to the print. A 10 mm gauge block against a 10 mm slot should not fit or should just drag. On a probe-equipped machine, re-probe the datum and confirm the offset repeats within 0.005 mm.
7
Dry-run the first toolRun the first toolpath 10 mm above the part with rapid override low. Watch the readout at each approach move. If the tool goes to the wrong side of the part, stop and check the offset sign. A wrong sign is the most common setup error on a new program.
8
Record and lock the offsetsWrite the G54 values and the probe calibration date on the setup sheet. Lock the offset page if the control allows it. On a long run, re-probe every 8 hours or after any shift change to catch thermal drift.

Selection

Which setup method fits your part

Pick based on tolerance, quantity, and machine type.

Method	Typical accuracy	Best for	Avoid when
Edge finder	0.02–0.05 mm	One-off brackets, ±0.1 mm work	Bearing bores, tight bolt patterns
Dial indicator	0.01 mm	Vise and fixture alignment	High-volume runs, 5-axis pivots
Spindle probe	0.005–0.01 mm	Production, 4-axis and 5-axis	Uncalibrated stylus, dirty faces
Hard stop + gauge	0.01–0.02 mm	Repeat parts on a tombstone	First article, complex datums
Laser tool setter	0.005 mm on tool length	Tool length and breakage checks	Part datum location

Setup discipline is cheaper than rework

If your part has tight datums, a rotary axis, or a second operation, invest in probing and a written setup sheet. If it is a one-off bracket, an edge finder and a gauge block will do. Either way, verify before you cut.

Get Instant Quote Talk to an Engineer

FAQs

Table point setup questions

How often should I re-check work offsets on a production run?

At the start of each shift, after any spindle warm-up cycle, and after a tool change that involves a new holder. If the shop temperature swings more than 2 °C, check more often. On a probe-equipped machine, a quick re-probe of the datum takes under a minute and confirms the offset still repeats within 0.005 mm.

Can I use the same work offset for a 4-axis rotary setup?

No. A rotary table adds a pivot point and a rotation axis. You need the pivot location in machine coordinates, and on a trunnion you also need the tool center point offset. A single G54 value usually cannot describe both the part origin and the rotary center. Use separate offsets or a kinematic model in the control.

What tolerance can a vise setup realistically hold?

A clean, stoned vise with a dial-indicated fixed jaw can hold 0.01–0.02 mm on the datum faces, and the part features follow if the CAM setup matches. Pushing below 0.01 mm on a vise often means fighting jaw lift and part tilt. For tighter work, use a dedicated fixture or soft jaws machined in place.

Why does my Z zero change after a tool change?

Most often it is tool length, not the work offset. Check that the tool length offset matches the holder and that the pull stud is clean. A chip on the spindle taper or a worn retention knob can shift tool length by 0.01 mm or more. Re-measure the tool on the setter and compare.

Is probing worth it for a one-off prototype?

For a simple part, an edge finder and a gauge block are faster. For a complex 5-axis part with tight datums, probing saves time because a single bad offset can scrap hours of machining. The break-even is usually around the point where the part value exceeds the setup time.

How do I set the datum on a casting with no machined faces?

Use a fixturing feature or a locating boss if the casting has one. If not, set up on the as-cast surface and expect 0.1–0.3 mm variation. For tight work, add a machining allowance and cut a reference face first. Never assume an as-cast surface is flat or square.