China CNC Processing RFQ Guide

Start with a 3D model. STEP and IGES open in CAM without translation loss; native SolidWorks or NX files are fine when you can share them. Add a 2D drawing only for the calls the model cannot carry: fits, datum scheme, GD&T, thread class, surface finish per face, and any marking. A model alone tells the shop shape. It does not tell the shop where the part must seal, slide or press.

State material and temper, not just the alloy family. 6061-T6 and 6061-O cut and finish differently, and 316L machines nothing like 303. Temper changes chip formation, tool wear and the risk of distortion after stress relief. Say whether the stock is plate, bar, extrusion or casting, because a hog-out from plate and a finish-machined casting are two different quotes.

Call out heat treat, plating and passivation as separate line items. A hardened 17-4PH part cannot be finish-machined after aging, so the sequence matters. Note which surfaces stay raw and which get masked. This is where most revision cycles start, and it is cheap to fix on paper.

Give quantities for prototypes, pilot builds and production, plus an annual estimate. Unit price on one piece and on 5,000 pieces differs by more than a machine change. Also name the inspection you need: first article, dimensional report, material cert, or full CMM layout. Those reports take time and add cost, so put them in the first email.

Default to general tolerances unless a function demands tighter. On most parts, ±0.1 mm on non-critical features is enough, and ±0.005 mm is reserved for bores, bearing seats and mating faces. Tightening a whole drawing to ±0.005 mm forces slower passes, more setup checks and more scrap risk. The cost curve is not linear. It turns up sharply.

Surface finish behaves the same way. As-machined at Ra 1.6–3.2 μm suits brackets and covers. Ra 0.8–1.6 μm is a normal finish for sealing faces. Ra 0.2–0.8 μm needs finer tooling, lighter depths of cut and often a separate operation, so keep it on the faces that touch. A blanket note like finish all over to Ra 0.4 μm will be quoted high and may be impossible on deep pockets.

Geometric tolerances need a datum plan. Flatness, perpendicularity and position callouts only mean something when the drawing names the A, B and C datums and shows how the part is held. Without that, the shop guesses, and the CMM report may not match your intent.

Threads, radii and text are small lines that cause big questions. Give thread class, not just size. Give the smallest internal radius the tool can reach. Mark engraving with a minimum character height, since 1.5 mm is the practical floor for laser marking and anything smaller will not read cleanly.

Five-sided work and deep pockets are the two common cost jumps. A part that needs all six faces machined needs either multiple setups or a 5-axis center. Each extra setup adds fixturing and re-datuming, and re-datuming is where position error creeps in. If a face is not functional, leaving it as-cast or as-sawn removes a setup from the route.

Deep pockets and tall thin walls create the other jump. A pocket four times deeper than its width needs long, slender tools that deflect, so the shop cuts at lower feed and takes more spring passes. Walls under 1 mm on aluminum or under 0.5 mm on steel tend to chatter unless the geometry gives the tool support.

Holes smaller than Ø1 mm, sharp internal corners, and undercuts reachable only from one direction all add time. So do cosmetic faces that must stay free of tool marks. It is worth asking whether a corner can carry a radius or a hole can move, because moving a feature 2 mm can remove a setup entirely.

Material availability sets the floor. Common aluminum, 303 and 304 stainless, 1018 and 4140 steel, and standard brass are stocked and machine well. Inconel, titanium and beryllium copper are machinable but slow, and some need special tooling and coolant. PEEK and carbon fibre have their own rules. Name the material early and the quote will not need a second pass.

CNC is a subtraction process, so it wins on tight tolerance, low to mid volume, and geometry that changes between revisions. It loses when the part is a thin shell with uniform wall, when the shape is organic, or when the annual volume runs into tens of thousands of identical pieces with no tolerance tighter than ±0.2 mm.

Thin-walled enclosures, ducting and covers are usually better as sheet metal or die casting. Rubber-like parts and complex internal channels belong to molding or 3D printing. Very large flat plates with a few holes are often laser cut and formed at a fraction of the milling cost.

A mixed route is common. Machine the critical bores and sealing faces, then form or cast the rest. That keeps the tolerance where it matters and takes the cost out everywhere else. It helps to say in the RFQ which dimensions are functional, because that line tells the shop where to spend its time.

Prototypes are a special case. One or two pieces rarely justify tooling, so CNC, vacuum casting or 3D printing carry the load. Once the design freezes, revisit the process. A part that was correctly milled at five pieces may be a casting at 20,000.

Match the shop's machine list to your part envelope. A 4,000 mm part needs a machine that can travel that far, and a Ø400 mm rotary table sets the limit on round work. If your part is 4,000 × 400 × 150 mm, ask which center runs it. A shop that quotes anyway will sub the job out.

Ask how inspection is handled. A shop that inspects 100% before shipment and can send material certs, first article reports and CMM data is easier to work with than one that only checks a sample. Ask what happens when a dimension is out: rework, remake or a deviation request. The answer tells you more than the price.

Confirm the confidentiality route before you upload. An NDA on request and secure file handling protect your drawings. For medical and automotive work, the quality system matters: ISO 9001:2015, IATF 16949:2016, ISO 13485:2016 and ISO 27001:2022 cover different risks. Match the certificate to your industry.

Set the timeline in the RFQ itself. Say when you need the quote, when you can approve, and when the parts must land. A shop that returns a quote and free DFM analysis within 12 hours and can start production within 24 hours gives you room. Parts that ship in 3–5 days keep a pilot build on schedule.