NC process control

NC precise machining process: from setup sheet to inspection report

This page walks through the steps we use to hold ±0.005 mm on production parts. It is written for engineers and buyers who need to judge whether a shop can repeat a tolerance, not just hit it once. Read it before you release a drawing with tight position or profile callouts.

Get Instant Quote Talk to an Engineer

±0.005 mm tolerance16 five-axis centers100% inspection3-5 day shipping

NC precise machining process setup being checked on a CNC machine

On this page

1
What matters most
2
What an NC precise machining process actually controls
3
Reading the drawing before the first cut
4
Choice of machine and fixture for the job
5
Cutting parameters that hold size
6
In-process checks and how to react
7
The NC precise machining process, step by step
8
Which setup fits which part

Key takeaways

What matters most

Tolerance lives in the setupA ±0.005 mm callout fails at workholding long before it fails at the toolpath.

Probe every critical datumTouch-off on the fixture, not on the vise jaw. Datum shift is the top cause of scrap.

Cut the finish pass lastRough with 0.3-0.5 mm stock, then take one light finishing pass at full depth.

Measure with the part coolAluminium grows 23 µm per metre per 1 °C. Measure after the part reaches 20 °C.

Reports on requestRaw material check, in-process monitoring and final inspection records are available.

Section 1

What an NC precise machining process actually controls

An NC precise machining process is not one setting. It is a chain of decisions that starts with the drawing review and ends with a signed inspection report. Break any link and the tight callout on your print becomes a coin flip. We see this most often on parts with a true position under 0.02 mm, a profile of 0.01 mm, or a bore that must mate with a pressed bearing.

The chain has four links: setup, toolpath, cutting conditions and measurement. Each one has its own error budget. If the setup eats 0.008 mm of your ±0.005 mm, no amount of spindle accuracy will save the part. So we allocate the budget before cutting, not after.

A useful way to think about it: the machine only repeats what the fixture and the program allow. A top-end five-axis center with a thermal drift of 2 µm is wasted if the vise jaw lifts the part 10 µm on the second operation.

This matters most when quantities rise. One prototype can be hand-fitted. A 10,000 part run cannot. The process has to hold the same number on part one and part ten thousand, and that is a discipline question more than an equipment question.

1
Setup errorFixture flatness, jaw lift, clamp deflection, datum shift after re-chucking.
2
Toolpath errorCutter deflection, tool runout, lead-in marks, leftover stock on the finish pass.
3
Thermal errorSpindle growth, coolant temperature, part growth before measurement.
4
Metrology errorProbe calibration, CMM stylus size, measuring a warm part.

Section 2

Reading the drawing before the first cut

Every tight job starts with a DFM review. We look for features that cannot be reached in one setup, thin walls under 0.8 mm, deep pockets with a depth-to-width ratio above 4:1, and tolerances that stack on the same datum. The quote you get back includes notes on all of these.

The first question is datum strategy. If the drawing calls out a bore as datum A but the bore is finished in operation two, then operation one has to leave enough stock to correct any shift. We normally leave 0.2-0.3 mm on the bore wall for the finishing pass.

The second question is access. A five-axis machine can tilt the tool to reach a side wall in one setup, but only if the tool holder clears the surrounding material. A 20 mm wall next to a Ø6 mm cutter shank will hit the holder at a 40° tilt. We check this in the CAM simulation, not on the machine.

Once those two questions are answered, the setup sheet is written. It lists the fixture, the datum, the probe routine, the stock allowance and the torque values for every clamp. The operator does not improvise from a sketch.

1
Features in two setupsLeave 0.2-0.3 mm on mating surfaces for the second operation.
2
Thin wallsBelow 0.8 mm, plan a support or a sacrificial rib, and take light passes.

Section 3

Choice of machine and fixture for the job

Not every tight part needs five axes. A flat plate with holes on one face runs faster and cheaper on a three-axis mill. We reserve the 16 simultaneous five-axis centers for parts with compound angles, deep cavities on multiple faces, or a position tolerance that would be lost in a second re-chuck.

For large work we run up to 4,000 mm on the long travel. Medium parts sit in the 750 × 1,150 × 550 mm and 600 × 600 × 600 mm envelopes, and compact work goes to the 500 × 500 × 450 mm or 500 × 310 × 200 mm machines. The Ø400 mm rotary table handles parts that need continuous indexing.

Fixture choice follows the tolerance. For ±0.005 mm work we prefer a dedicated plate with a machined pocket and four low-profile clamps, or a dovetail block for parts that cannot tolerate top clamping. A standard vise is fine for ±0.05 mm, but it will not hold a 5 µm callout.

Material matters too. Aluminium 6061 and 7075 cut clean and hold size well. Stainless 316 and 17-4PH move more after roughing, so we plan a stress-relief step or a semi-finish pass before the final cut. Titanium TC4 needs lower surface speed and steady coolant to avoid work hardening at the cut edge.

1
Three-axisFlat parts, holes on one face, tolerances from ±0.02 mm up.
2
Four-axisCylindrical features and parts indexed around one axis.
3
Five-axisCompound angles, multi-face cavities, one-setup position control.

Section 4

Cutting parameters that hold size

The finishing pass decides the final dimension, so treat it as a separate operation. Roughing removes bulk with a bigger radial depth of cut and leaves 0.3-0.5 mm of stock on the walls and floor. Then a semi-finish pass brings it to 0.05-0.1 mm, and the finish pass takes that in one continuous cut at full depth.

For aluminium with a carbide end mill, we run 300-600 m/min surface speed and 0.05-0.1 mm per tooth feed. Steel drops to 100-200 m/min. Stainless and titanium run lower still, 60-120 m/min, with more coolant and a sharper edge geometry. These are starting points, not a fixed recipe.

Tool runout is the quiet killer. A cutter with 0.02 mm of runout will cut a slot 0.02 mm wide on one side and leave a step on the floor. Check runout with a dial indicator at the cutting edge before the finish pass, and replace the holder if it exceeds 0.01 mm.

Heat is the other variable. A 20 °C shop is not the same as a 20 °C part. Aluminium expands about 23 µm per metre per 1 °C, so a 300 mm part measured 5 °C above ambient reads roughly 35 µm large. Let the part stabilise before the final measurement, or measure and compensate deliberately.

1
RoughLeave 0.3-0.5 mm on walls and floor.
2
Semi-finishBring stock down to 0.05-0.1 mm.
3
FinishOne continuous pass at full depth, no dwell marks.
4
RunoutKeep below 0.01 mm at the cutting edge.

Section 5

In-process checks and how to react

We probe the datum after every re-chuck and log the shift. If the shift exceeds 0.01 mm, the operator stops and re-probes rather than pushing through. This single habit removes most of the scrap we would otherwise see on tight parts.

During the run we check a first article against the drawing, then sample at a fixed interval. For a ±0.005 mm feature, the sample is measured on a CMM with the part at room temperature. For looser features, a micrometer or bore gauge is enough and keeps the cycle moving.

When a dimension drifts, the fix is usually a cutter compensation change, not a new program. Adjust the wear offset by half the measured error and re-cut one part. If the drift comes back within ten parts, the problem is thermal or the tool is wearing, and the tool change interval needs to shorten.

Surface finish is checked alongside size. We work to Ra 0.8-1.6 µm as a standard machined finish, Ra 0.2-0.8 µm when the drawing calls for it, and Ra 1.6-3.2 µm for as-machined surfaces. A finish that suddenly roughens usually means the tool edge has dulled.

1
Datum shift over 0.01 mmStop, re-probe, re-zero before continuing.
2
Steady driftAdjust wear offset by half the error, then re-measure.
3
Repeating driftShorten the tool change interval or check coolant temperature.

How we run it

The NC precise machining process, step by step

Follow these in order. Skipping step 2 or 5 is the most common cause of a failed first article.

1
Review the drawing and allocate the error budgetList every tight feature, its datum and its tolerance. Split the tolerance across setup, toolpath, tool wear and measurement before quoting. Flag any feature that needs two setups.
2
Design the fixture and write the setup sheetUse a machined pocket plate or dovetail block for ±0.005 mm work. Record clamp torque, datum points, stock allowance (0.2-0.3 mm on mating faces) and the probe routine on one sheet.
3
Probe the datum after clampingTouch off on the fixture datum, not on a vise jaw. Log the shift. If it exceeds 0.01 mm, re-seat the part and probe again before cutting.
4
Rough and semi-finish, then let the part coolRough with 0.3-0.5 mm of stock left. Semi-finish down to 0.05-0.1 mm. Pause 10-15 minutes so the part and fixture reach shop temperature.
5
Check tool runout and take the finish passMeasure runout at the cutting edge (target under 0.01 mm). Cut the finish pass in one continuous move at full depth. Do not stop mid-contour.
6
Measure the first article at room temperatureCool the part to roughly 20 °C, then measure on a CMM for tight features or with a micrometer for open tolerances. Record the actual values, not just pass or fail.
7
Adjust wear offsets, then run the batchChange the offset by half the measured error and re-cut one part. Confirm, then release the batch with a fixed sampling interval.
8
Inspect 100% before shipmentRaw material check, in-process monitoring and final inspection are recorded. Reports are available on request with the shipment.

Process choice

Which setup fits which part

Pick the row that matches your part, then confirm with the tolerance column.

Part type	Setup	Typical tolerance	When it is the wrong choice
Flat plate, holes on one face	Three-axis, soft jaws	±0.05 mm	Compound angles or side features
Shaft with keyways and flats	Four-axis or mill-turn	±0.02 mm	Deep multi-face pockets
Housing with angled ports	Five-axis, one setup	±0.005 mm	Simple prismatic parts, cost not justified
Large frame up to 4,000 mm	Five-axis, long travel	±0.02 mm	Parts that fit a compact machine
Thin-wall cover	Five-axis with support ribs	±0.01 mm	Wall under 0.8 mm without support
Impeller or blade profile	Five-axis, continuous indexing	±0.005 mm	Prismatic geometry with no free-form surface

FAQs

Common questions

Can you hold ±0.005 mm on every feature of a part?

No, and any shop that says yes is overselling. We hold ±0.005 mm on the features that are reachable in the same setup, measured at room temperature.

Features cut in a second operation carry the re-chuck error, which is usually 0.01-0.02 mm even with probing. If your drawing needs ±0.005 mm across two setups, the design should be changed or the features consolidated.

How do you decide between three-axis and five-axis?

We look at three things: how many faces carry tight features, whether the angles are compound, and whether a second setup would consume too much of the tolerance.

If all tight features sit on one face and the tolerance is ±0.02 mm or looser, three-axis is faster and cheaper. Five-axis earns its cost when one setup replaces two or more, or when the tool must tilt to reach a wall.

What surface finish can I expect on a standard machined part?

Standard machined surfaces come out at Ra 1.6-3.2 µm. We hold Ra 0.8-1.6 µm when the drawing calls for it, and Ra 0.2-0.8 µm on request for sealing faces or bearing bores.

Finish and tolerance interact. A tighter finish usually means a lighter finishing pass, which takes longer and costs more. Tell us the function of the surface so we can pick the right band.

How do you handle a part that moves after roughing?

We plan for it. Stainless 316, 17-4PH and some titanium grades move after material is removed because internal stress is released.

The usual fix is a semi-finish pass, a pause to let the part stabilise, then the finish pass. On parts with very tight flatness, we may ask for stress-relieved stock or split the machining into two sessions.

What inspection data comes with the parts?

Raw material check, in-process monitoring and final inspection are part of the standard route, and 100% of parts are inspected before shipment.

Inspection reports are available on request. Tell us which dimensions matter at the quote stage so the report covers them rather than a generic list.

What happens if the first article fails?

The run stops. We measure the failed feature, compare it with the error budget from the setup sheet, and find which link moved: setup, tool wear or temperature.

Then we correct it, re-cut one part and re-measure before the batch continues. You get told what changed, not just that it is fixed.