Process guide

CNC parts processing tips for engineers and buyers

This guide covers the decisions that decide whether a machined part comes off the machine in spec or comes back for rework. It is written for design engineers, manufacturing engineers, and sourcing teams who need to review a part before it goes to a shop. Read it and you can judge which features are risky, which tolerances are worth paying for, and what to check before the first chip is cut.

Get Instant Quote Talk to an Engineer

±0.005 mm toleranceRa 0.2–0.8 μm finishNo minimum order12-hour DFM response

Custom auto spare parts made with 5-axis CNC parts processing tips

On this page

Key takeaways

Fix DFM before quotingA deep pocket with a 2 mm corner radius costs more than the same pocket at 4 mm. Change the drawing, not the machine.

Tolerance drives costDefault to ±0.05 mm on non-critical features. Reserve ±0.005 mm for fits, bores, and datums.

Pick finish by functionRa 1.6–3.2 μm is fine as machined. Go to Ra 0.8–1.6 μm only where a seal, bearing, or slide touches.

Setup count sets lead timeEach new setup adds fixture time and stack-up error. Fewer setups usually means tighter results.

Inspect to the datumA part that measures well off one face and fails off another is a datum problem, not a machining problem.

Design review

Start with DFM, not with the quote

Most cost in CNC parts processing is locked in at the drawing stage. A shop can only remove material in the directions its tools can reach. If a feature sits inside a pocket, behind a shoulder, or under a boss, the cutter either cannot reach it or has to be long and thin, which means chatter and slow feed rates.

Walk the part face by face before you release it. Ask what tool reaches each feature, from which direction, and how the part is held while that cut happens. If you cannot answer all three, the shop will quote a high number or send the part back with questions, and both add days.

The usual fixes are cheap on paper. Open a corner radius, add a relief groove at the bottom of a thread, break a sharp internal edge, or move a hole off a slanted surface. None of these change function. All of them cut cycle time.

1
Set a minimum internal radiusKeep it at least one third of the pocket depth; below that, tool breakage risk climbs.
2
Give cutters an exitA closed slot needs a plunge entry. An open slot can be milled with a ramp.
3
Avoid thin walls earlyWalls under 0.8 mm deflect under cutting force, even in aluminium.
4
Keep deep holes shallowDrill depth over 8 × diameter needs peck cycles and a straight start.

Tolerance and finish

Spend tolerance where it matters

A ±0.005 mm callout on a mounting hole is wasted money. The same callout on a bearing bore is necessary. Machining cost rises in steps as tolerance tightens, because tighter tolerance means slower feed, more passes, temperature control, and more inspection time.

The practical approach is to separate features into two groups. Fits, bores, seal faces, and anything that locates another part get the tight numbers. Everything else gets a general tolerance block. On a typical part, only 10 to 20 percent of dimensions actually need ±0.005 mm.

Surface finish follows the same logic. Ra 1.6–3.2 μm covers most brackets, covers, and housings. A seal running on a shaft wants Ra 0.8–1.6 μm. Sliding surfaces and optical seats may need Ra 0.2–0.8 μm, which usually means a finishing pass or a secondary operation such as lapping or polishing.

One more point: finish and tolerance interact. A very smooth surface on a thin wall can relax after clamping is released. If the part springs, the dimension drifts even though the machine held position. Stress relief or a lighter finishing pass fixes it.

Material and setup

Match material and setup to the cut

Material choice changes feeds, speeds, and tool life. Aluminium 6061 machines fast and holds tolerance well, which makes it the default for prototypes and low-volume parts. Stainless 304 work-hardens if the cutter rubs, so you need a sharp tool, a steady feed, and no dwell in the cut. Titanium TC4 (Ti-6Al-4V) needs lower surface speed and plenty of coolant.

If a part has to be stiff, wear resistant, or heat treated after machining, the choice shifts. 4140 and 4340 give good strength after heat treatment. 17-4PH holds up in corrosive service. Plastics such as POM and PEEK machine cleanly but move with temperature, so hold them in a fixture that does not over-constrain them.

Setup is the other half. Every time the part is moved to a new fixture, error stacks up. A part machined in three setups can easily lose 0.02 mm across the sequence even if each setup is perfect. Five-axis work helps here because more faces are cut in one setup.

For long parts, support matters more than speed. On a 4,000 mm part, sag between supports shows up as a taper. Add steady rests or a tailstock, and take lighter passes near the free end.

Quality control

Inspection and common failure points

Inspection is where good processing shows up. A shop that checks only the final part misses drift that started on part three. The stronger approach is to check raw material, watch the process, and confirm the final part against the drawing.

The most common failure is a datum mismatch. The drawing says the hole is located from face A, but the setup used face B as the stop. The part measures correctly on the machine and fails on the inspection table. Fix the datum, and the problem disappears.

Burrs are the second most common issue. A burr on a sealing face or a thread start can cause a leak or cross-threading. Deburring should be part of the process, not a cleanup afterthought. Specify it on the drawing and name the edges that matter.

Thermal drift is the third. A spindle that has run for two hours is warmer than one that just started, and the same program cuts a different size. Shops that hold ±0.005 mm regularly let the machine warm up and check a test cut before running the batch.

Workflow

Seven steps to run a part through processing

Follow this order. Skipping a step usually costs more time later than it saves now.

1
1. Review the drawing for reachCheck every pocket, hole, and undercut against tool access. Note the minimum internal radius and any feature deeper than 4 × its width.
2
2. Split dimensions into tight and looseMark fits and datums at ±0.005 mm to ±0.02 mm. Leave everything else at ±0.1 mm or the general tolerance block.
3
3. Choose material and stock formPlate, bar, or casting changes both cost and setup. Castings reduce roughing time but need a cleanup pass and may have hard spots.
4
4. Plan the setup sequenceAim for the fewest setups. Machine all datums in setup one. Leave a 0.3–0.5 mm finishing allowance on faces that will be re-clamped.
5
5. Set speeds, feeds, and coolantAluminium 6061 runs at 300–600 m/min surface speed. Stainless 304 drops to 120–180 m/min. Titanium TC4 stays near 40–60 m/min. Use coolant on any deep cut.
6
6. Control temperature and chipsLet the part cool before the finishing pass. Clear chips from pockets; recut chips damage finish and break small tools.
7
7. Inspect against the datumMeasure from the same datum the drawing uses. Check the first part fully, then sample in-process and do a final check before shipment.

Decision table

Choosing tolerance, finish, and process by feature

Use this to decide what to call out on the drawing.

Feature	Tolerance	Surface finish	Process note
Bearing bore	±0.005 mm	Ra 0.8–1.6 μm	Bore in one setup, finish last
Seal face	±0.02 mm	Ra 0.8–1.6 μm	No tool dwell, light finishing pass
Mounting hole	±0.1 mm	Ra 1.6–3.2 μm	Drill or drill and ream
Pocket floor	±0.05 mm	Ra 1.6–3.2 μm	Corner radius ≥ 1/3 depth
Sliding surface	±0.02 mm	Ra 0.2–0.8 μm	Polish or lap after milling
Cosmetic panel	±0.2 mm	Ra 1.6–3.2 μm	Bead blast hides tool marks
Threaded hole	Class 6H	Ra 1.6–3.2 μm	Add relief groove at thread end
Weld prep edge	±0.5 mm	Ra 3.2 μm or better	Deburr before welding

FAQs

Questions engineers ask before machining

How tight a tolerance can CNC parts processing hold?

On a well-set-up machine, ±0.005 mm is achievable on critical features such as bores and datums. On general dimensions, ±0.05 mm to ±0.1 mm is normal and far cheaper.

If you need tighter than ±0.005 mm across many features, expect slower production, more inspection, and possibly a secondary finishing operation.

What surface finish should I specify for a machined part?

Ra 1.6–3.2 μm is the standard as-machined finish and is fine for most brackets and housings. Choose Ra 0.8–1.6 μm for seal faces and bearing fits.

Ra 0.2–0.8 μm is for sliding surfaces and optical seats. It usually needs a separate finishing pass or a polishing step, so only call it out where it changes function.

Which features should I avoid when designing for CNC?

Avoid deep narrow pockets, sharp internal corners, and holes drilled into slanted surfaces. All three need special tools or extra setups.

Thin unsupported walls under 0.8 mm also cause trouble. They deflect during cutting and move after the clamp is released, so the final size is hard to predict.

How does setup count affect cost and accuracy?

Every setup adds fixture time, re-clamping error, and inspection. A part machined in three setups can lose 0.02 mm or more across the sequence.

Five-axis machining reduces setup count by cutting more faces in one position, which usually improves both accuracy and lead time on complex parts.

When is 5-axis machining worth it over 3-axis?

Use 5-axis when the part has features on multiple faces, angled holes, or contoured surfaces that would need several fixtures on a 3-axis machine.

For a simple plate with holes on one face, 3-axis is faster and cheaper. Match the machine to the geometry, not the other way around.

What do I need to send for an accurate quote and DFM review?

Send a 3D model plus a 2D drawing with tolerances, material, finish, and quantity. Note which dimensions are functional and which are reference.

If a feature is hard to inspect, say so. The shop can suggest a different callout that is easier to measure and just as functional.