Basics of CNC Machining Design

Thin walls deflect under cutting force. On aluminum, walls down to 0.8 mm are machineable if the height stays under about 10 mm and the cutter can approach from both sides. Push the wall to 20 mm tall and the same 0.8 mm section will chatter, spring back, and finish oversize. A 1.5 mm wall is a safer default for most brackets and housings. In 316 stainless, keep walls at 1.5 mm or thicker, because the higher cutting load pushes thin sections harder.

Floor thickness matters just as much. A 0.5 mm floor in a 40 mm pocket will bow when the cutter passes underneath. We usually suggest floors of 1 mm minimum on aluminum and 1.5 mm on steel and titanium. If the design needs a thin membrane, say for a pressure burst disc, machine it from a thicker blank and grind or lap it afterward. That keeps the CNC setup simple.

Ribs help. A 2 mm wall with a 2 mm rib every 20 mm is stiffer than a 4 mm wall alone, and it saves weight. Add ribs before you add thickness. This is one of the first things our DFM review flags when we see a deep pocket.

• 1
  Aluminum wall minimum0.8 mm short, 1.5 mm general purpose
• 2
  Stainless or titanium wall1.5 mm minimum, 2 mm preferred
• 3
  Floor thickness1 mm aluminum, 1.5 mm steel

Every internal corner has the radius of the cutter that made it. A standard end mill leaves a corner radius roughly equal to its diameter. If you draw a sharp internal corner, the machinist has to stop short, then clean the corner with a smaller tool or EDM. That adds a second setup and hours of time. The fix is simple: give internal corners a radius at least one quarter of the pocket depth, or 2 mm minimum.

Pocket depth drives tool length. A cutter can only reach about three times its diameter before it starts to deflect. A 12 mm deep pocket with a 6 mm corner needs a 6 mm cutter with 12 mm flute length, which is fine. A 60 mm deep pocket with the same 6 mm corner needs a long, slender tool that will chatter and leave a poor finish. In that case, either increase the corner radius or accept a stepped pocket.

Blind holes follow the same logic. A drill leaves a conical tip, so a flat-bottom hole needs a second operation with an end mill. If the design can tolerate a 118° or 140° point, say so on the drawing. It saves a tool change on every part.

• 1
  Internal corner radius≥ 1/4 of pocket depth, 2 mm minimum
• 2
  Depth-to-diameter ratioStay under 3:1 for a rigid cut
• 3
  Blind hole bottomSpecify drill point angle or flat bottom

A general tolerance block on the drawing covers most dimensions. We machine to ±0.1 mm as a default, and that is enough for brackets, covers, and most housings. Only call out tighter tolerance on the dimensions that actually function: a bearing bore, a dowel hole, a sealing face. Every tight tolerance adds inspection time and can force a second setup.

The tightest we hold is ±0.005 mm on critical features, usually on a jig grinder or a high-accuracy 5-axis center. That level is rare and should be reserved for mating surfaces or press fits. If you mark a whole drawing at ±0.005 mm, the quote will reflect the inspection burden, not the machining.

Datums matter more than tolerance values. A drawing with three datums that cannot be reached in one setup will force us to re-fixture the part, and stack-up error grows with each move. Pick datums that a machinist can touch in the first op. For round parts, use the turned diameter as datum A and a face as datum B. That keeps everything in one coordinate system.

Surface finish follows the same rule. Ra 1.6–3.2 μm is the as-machined default and costs nothing extra. Ra 0.8–1.6 μm needs a finishing pass with a sharp tool. Ra 0.2–0.8 μm needs a separate finishing operation, sometimes hand polishing. Specify the finish only where a seal, bearing, or optical surface requires it.

• 1
  Default tolerance±0.1 mm on general dimensions
• 2
  Tight tolerance±0.005 mm on functional features only
• 3
  Default finishRa 1.6–3.2 μm, no extra cost
• 4
  Fine finishRa 0.2–0.8 μm, adds a finishing op

The number of setups is the single biggest cost driver after material. A part that machines in one op from one side is cheap. Add a second side and the price climbs, because the part must be flipped, re-zeroed, and inspected again. Add a fourth side and the price climbs again.

Design for as few faces as possible. Put all critical features on one face or on two opposite faces. If a feature must sit on a third face, ask whether it can be moved to a face already being machined. Often it can, with a small change to the housing or bracket geometry.

Five-axis machining removes some of this constraint. A simultaneous 5-axis center can reach five faces in one setup, so undercuts and angled holes no longer need separate fixtures. We run 16 simultaneous 5-axis centers and 16 mill-turn centers for exactly this reason. But 5-axis time costs more per hour than 3-axis, so it pays off when the part is complex, not when it is simple.

For long parts, we machine up to 4,000 mm on the largest travel. Parts beyond that need to be split or designed as weldments. Keep that limit in mind early, before the drawing is frozen.

Aluminum 6061-T6 is the default for most machined parts. It cuts fast, holds tolerance well, and takes anodizing cleanly. 7075 is stronger but galls more and costs more. 2024 machines well but has poor corrosion resistance unless it is alodined or painted. For marine or wet environments, choose 5052 or 5083.

Stainless 303 is the easiest to machine and is fine for shafts and fittings. 304 and 316 are tougher and work-harden, so they need slower feeds and more rigid setups. 17-4PH gives high strength after heat treatment and is common in aerospace and medical work. All of these machine to ±0.005 mm on critical features when the setup is right.

Titanium and Inconel are a different story. Ti-6Al-4V (TC4) has low thermal conductivity, so heat stays in the cut and tools wear fast. Inconel is worse. Design walls and floors thicker for these alloys, and expect longer cycle times. If the part does not need high-temperature strength or a high strength-to-weight ratio, aluminum or steel will be cheaper and faster.

Plastics behave differently again. POM and PEEK hold tolerance well; ABS and PP flex and can melt if the cutter dwells. For plastic parts, add generous radii and avoid thin, unsupported sections. Carbon fibre is abrasive and wears tools quickly, so it needs carbide or diamond tooling.

• 1
  General purpose6061-T6 aluminum
• 2
  High strength aluminum7075, 2024
• 3
  Corrosion resistance316L stainless, 5052 aluminum
• 4
  High temperatureTi-6Al-4V, Inconel

Send a STEP or IGES file plus a 2D drawing with the tolerance block, datums, and finish callouts. If the drawing and the model disagree, the drawing wins. We check both during the DFM review and flag any conflict before quoting.

Our DFM review comes back within 12 hours with the quote. It lists features that will be slow or risky, and suggests changes. We do not charge for this review, and we do not share your files. An NDA is available if you need one on file.

Production can start within 24 hours of a signed order. Standard parts ship in 3–5 days. There is no minimum order quantity, so a single prototype and a 10,000-part run go through the same process. Every part is inspected before shipment, with reports on request.

The goal of all this is simple: catch the design issues before the first chip is cut. A 2 mm radius change on a drawing costs nothing. The same change after a fixture is built costs days.