Cut CNC order costs immediately

• 1
  Key takeaways
• 2
  Where the money actually goes
• 3
  Design changes that cut CNC order costs immediately
• 4
  Tolerance bands: tighten only what mates
• 5
  Setup count, five-axis, and the cost of re-clamping
• 6
  Material and stock choice
• 7
  Quantity, finishing, and inspection scope
• 8
  Step by step: prepare an RFQ that prices low

Roughly three quarters of a machined part's cost is locked in by the 3D model. You can shop the job around, but a drawing with a 0.4 mm deep pocket and a sharp internal corner will be expensive everywhere. The fastest savings come from changing the part, not the supplier.

Start with internal corners. A standard end mill leaves a radius equal to its own radius. If your corner is drawn at 0.5 mm, the shop has to reach for a small cutter, run it slow, and often burn a second operation. Open the corner to 1.5–3 mm and the same feature runs on a normal tool.

Then look at depth-to-width ratios. Pockets deeper than four times the cutter diameter force long, thin tools that deflect, squeal, and break. When you can, cap pocket depth at 3× the width or rough it out with a larger tool and finish only the last few millimeters.

Thin walls are the quiet budget killer. Walls under 1 mm move under clamping pressure, so the shop has to take lighter passes, add support, and inspect more. Keeping walls at 1.5 mm or thicker on aluminum usually removes an entire finishing pass.

• 1
  Open internal radiiMatch the corner radius to the largest cutter that can reach the feature.
• 2
  Cap pocket depthAim for 3× the cutter diameter; beyond 4× the tool cost climbs fast.
• 3
  Thicken thin walls1.5 mm minimum on aluminum keeps chatter and rework out of the job.
• 4
  Drop cosmetic calloutsRa 0.4 μm on a face nobody touches buys nothing.

A general tolerance block of ±0.1 mm is normal for non-critical features. When a designer tightens the whole drawing to ±0.005 mm, the shop has to treat every dimension as critical. That means more inspection, slower feeds, and a higher scrap rate. The price follows.

Split the drawing into two groups. Mating surfaces, bearing bores, seal grooves, and dowel holes get the tight tolerance. Everything else stays at the block tolerance. On a typical bracket or housing, that single change can move 20–40% of the dimensions out of the critical bucket.

Position tolerance deserves the same treatment. A true position callout of Ø0.05 mm on a hole pattern may force a jig-bored setup or an on-machine probe. If the mating part has clearance, Ø0.2 mm often works and runs on a standard setup.

Surface finish belongs in the same conversation. Ra 0.8–1.6 μm is a normal machined finish. Ra 0.2–0.8 μm requires slower finishing passes or a secondary operation. Reserve the fine band for sealing faces and sliding surfaces.

• 1
  Two-tier tolerance block±0.005 mm on mating features, ±0.1 mm on the rest.
• 2
  Check true positionØ0.2 mm is usually enough when the mating part has clearance.
• 3
  Match finish to functionRa 0.8–1.6 μm covers most surfaces; go finer only for seals.

Every time a part leaves the table, you pay twice. Once for the fixture and the operator's time, and again in accuracy, because each re-clamp adds stack-up error. On a part that needs four faces machined, a three-axis route may need three or four separate setups.

Five-axis machining collapses those setups into one. The part is clamped once, the table rotates, and all faces are cut in the same coordinate system. On complex housings and brackets, that usually removes the fixture build entirely and shortens the route.

We run 16 simultaneous five-axis machining centers, 12 four-axis mills, and 27 three-axis machines, so the routing decision is made on the part, not on what happens to be free. Simple prismatic parts still run faster on three-axis. Complex, multi-face parts go to five-axis.

The judgment line is roughly this: if a part needs three or more orientations and has features that must stay in relation to each other, five-axis usually wins. If it is a flat plate with holes, three-axis is cheaper and just as accurate.

• 1
  Count the orientationsThree or more faces usually means five-axis pays for itself.
• 2
  Keep datums stableOne setup means one coordinate system and less stack-up.
• 3
  Do not over-spec the machineFlat plates with holes run cheaper on three-axis.

Material affects two numbers: the price of the bar and the speed the cutter can run. Aluminum 6061 machines fast and is cheap to buy. Titanium Ti-6Al-4V, Inconel, and 17-4PH cut slowly, wear tooling, and often need more finishing passes. On the same geometry, the machine time can double or triple.

If the application allows it, a free-machining grade is the simplest saving. Stainless 303 cuts noticeably faster than 304 or 316. Brass C36000 machines faster than C27400. On aluminum, 6061-T6 is the default for most structural parts and is stocked in many sizes.

Stock size matters as much as alloy. A part cut from a bar that is 5 mm oversized wastes material and machine time in roughing. Buying near-net stock, or designing around standard bar and plate sizes, removes that waste before the job starts.

Do not change material just to save a few percent if the part sees load, heat, or corrosion. A cheaper alloy that fails in service costs far more than the machining you saved.

• 1
  Free-machining grades303 stainless and C36000 brass cut faster than their general-purpose cousins.
• 2
  Near-net stockOrder bar and plate close to final size to cut roughing time.
• 3
  Do not trade functionLoad, heat, and corrosion requirements come before price.

Unit price falls as quantity rises because setup and programming are spread over more parts. There is no minimum order quantity here, so a single prototype is possible. But the price per part at one piece and at fifty pieces are different numbers, and it is worth asking for both.

Finishing is often quoted as a separate line. Anodizing, plating, powder coating, and laser marking all add handling, masking, and turnaround. If only one face is visible, mask the rest. If the marking is a serial number, keep the character height at 1.5 mm or more so it stays legible.

Inspection scope drives cost quietly. A standard job gets a raw material check, in-process monitoring, and a final inspection before shipment. A full dimensional report with every callout measured on a CMM takes time and is priced accordingly. Ask for the report only where the customer or the drawing requires it.

One more lever: let the shop choose the routing. If the drawing specifies a machine or a process step, the quote has to follow it. If you specify the result, the shop can pick the cheaper route.

• 1
  Ask for two quantitiesOne prototype and one production run show where the price breaks.
• 2
  Mask non-visible facesFinishing only what shows saves handling time.
• 3
  Scope the reportFull CMM reports cost more than a standard inspection.