CNC machining design: how geometry decides cost and yield

• 1
  What CNC machining design actually controls
• 2
  Wall thickness, radii and the limits of the cutter
• 3
  Hole depth, thread choice and tapping limits
• 4
  Tolerances, datums and inspection reality
• 5
  When to use 3-axis, 4-axis, 5-axis or mill-turn
• 6
  Material choice changes the design rules
• 7
  CNC machining design limits by feature

CNC machining design is the practice of shaping a part so a rotating cutter can reach every surface, a fixture can hold it while that happens, and a probe or CMM can measure the result. The machine does not read intent. It follows the toolpath, and the toolpath is limited by tool diameter, tool length, and the angle the spindle can reach.

Design decisions set three numbers early: cycle time, scrap risk, and the tolerance you can actually hold. A pocket with a 2 mm corner radius in a 40 mm deep slot forces a long, thin tool. That tool deflects, so the machinist has to slow the feed, take lighter passes, and may still miss the corner. Change the radius to 4 mm and the same pocket runs with a stiffer tool at a higher feed rate.

The same logic applies to datum choice. If a drawing calls a bore concentric to a surface that no longer exists after the first op, the shop has to build a soft jaw or a fixture to recreate it. That is real cost, and it shows up as a line item, not as a magic trick.

None of this means the part has to be simple. It means every feature should have a reason, and the reason should survive a conversation with the person holding the chip pan.

• 1
  Tool accessCan a standard end mill reach the feature without a long, thin tool?
• 2
  WorkholdingIs there a flat, rigid surface the vise or fixture can grip?
• 3
  MetrologyCan the tolerance be measured on the finished part, not on the setup?

Thin walls are the most common source of chatter and scrapped parts. On aluminium 6061, walls below 0.8 mm start to deflect under normal cutting forces; on stainless 304 or 17-4PH, keep walls at 1.2 mm or more. On titanium TC4, 1.5 mm is a safer floor. The numbers are not absolute, but they tell you when to expect the shop to ask for a change.

Internal corners are the second issue. A cutter is round, so every pocket corner carries the radius of the tool. If the drawing shows a sharp 90° internal corner, the shop either leaves a radius anyway or burns hours with a small tool and a lot of pecking. Specify the largest acceptable corner radius and let the shop pick the tool that fits it.

Deep pockets bring length-to-diameter ratio into play. A 10 mm end mill cutting a 50 mm deep pocket is running at 5:1, which is workable with a stub or reduced-neck cutter at lower feed. At 10:1 the tool becomes a spring. If the pocket must be that deep, either open the corners or split the feature so it can be machined from both sides.

Floor radius matters too. A sharp internal floor corner needs a flat-bottom tool with a corner radius, and the radius left behind is dictated by that tool. If your design needs a true square floor, say so early, because it may require EDM or a different process.

• 1
  Aluminium 6061Minimum wall around 0.8 mm for stable cutting.
• 2
  Stainless 304 / 17-4PHKeep walls at 1.2 mm or thicker to control deflection.
• 3
  Titanium TC4Treat 1.5 mm as the practical floor without special support.

Hole depth is a ratio problem. A standard twist drill can reach about 4 times its diameter before chip evacuation becomes unreliable. Around 8 times diameter, peck drilling and through-tool coolant are needed. Past 10 times diameter, the shop will likely drill from both ends or use a gun drill, and the price reflects that.

Threads have a similar rule. Cut threads in aluminium and stainless are standard. In titanium and Inconel, thread milling is often the better call because it produces a cleaner profile and avoids tap breakage, which is expensive when it happens inside a finished part.

Thread depth should be at least 1.5 times the nominal diameter for steel and stainless, and 2 times diameter for aluminium, where the material is softer. A 6 mm thread in aluminium wants roughly 12 mm of engagement. Shorter engagement strips under load, and the failure happens in the field, not on the bench.

For blind holes, add a small flat-bottom allowance or specify a drill point angle. If the drawing calls a blind hole with a flat bottom, the shop has to use an end mill, which changes the cycle time. One note on the print saves a round of questions.

• 1
  Depth to diameter4:1 is routine, 8:1 needs pecking, 10:1 needs a special plan.
• 2
  Thread engagement1.5× diameter in steel, 2× diameter in aluminium.
• 3
  Thread millingPreferred for titanium and high-nickel alloys.

A tolerance is a promise about the finished part, and it has to be measurable. The general tolerance on a drawing should match what the part needs, not what looks impressive. Hanging a ±0.005 mm callout on a non-functional surface adds inspection time and scrap risk without improving the assembly.

Datums should come from surfaces that exist after the first operation and that the fixture can actually locate. If the datum is a curved surface, the shop will build a dedicated nest. That is fine for a 10,000 part run and wasteful for a prototype. For prototypes, choose a flat face or a bore as the primary datum.

Inspection follows the same logic. A true position callout of Ø0.05 mm MMC on a hole pattern is measurable with a CMM and a functional gauge. The same callout without the MMC modifier is harder to verify and slows the run. Adding MMC where the assembly allows it is one of the cheapest DFM wins on a drawing.

GreatLight inspects 100% of parts before shipment, with raw material checks, in-process monitoring and a final inspection. Reports are available on request. That covers the process, but the tolerance still has to be reachable by the machine and the tool.

• 1
  General toleranceSet it to the assembly need, not the machine limit.
• 2
  Datum choiceUse flat faces or bores for prototypes and short runs.
• 3
  MMC modifierIt makes hole-pattern inspection faster and cheaper.

Most prismatic parts with features on one or two faces run well on a 3-axis machine. The part sits in a vise, the cutter comes from above, and the shop flips it once for the back side. This is the cheapest route, and it holds ±0.005 mm on well-supported features.

Add features on four sides and a 4-axis mill with a rotary table saves setups. The part rotates around one axis, so a single program reaches multiple faces and the positional error between operations drops. This suits shaft-like parts, manifolds and brackets with side holes.

Simultaneous 5-axis work is for contoured surfaces, deep angled pockets and features that a straight tool cannot reach. GreatLight runs 16 simultaneous 5-axis machining centers, plus 12 four-axis mills, 27 three-axis machines and 16 mill-turn centers. The right choice is the one that reaches the feature with the stiffest tool, not the one with the most axes.

Mill-turn centers handle parts that combine turning and milling, such as a shaft with cross holes or a flange with an eccentric bore. Doing both on one machine removes a setup and protects concentricity. If your part has a turned diameter and a milled slot, mill-turn is usually the shortest path.

• 1
  3-axisOne or two faces, vise-friendly, lowest cost.
• 2
  4-axisFour-sided features, fewer setups, good position control.
• 3
  5-axisContours and deep angled features a straight tool cannot reach.
• 4
  Mill-turnTurned and milled features on one part, one setup.

The same geometry behaves differently across materials. Aluminium 6061 and 7075 cut fast and hold thin walls, but 7075 is more prone to stress relief movement after heavy material removal. Stainless 304 work-hardens, so light rubbing passes are worse than a firm cut. Titanium TC4 conducts heat poorly, so the cutter runs hot and tool life drops.

For high-volume parts, material cost and machinability both matter. ADC12 die casting aluminium is a different process, but a design that transitions from machined prototype to die cast production should keep wall thickness and draft in mind from the start.

GreatLight machines aluminium 6061, 6061-T6, 2024, 5052, 5083, 6063, 6082, 7075 and ADC12; stainless 303, 304, 316, 316L, 420, 430, 431, 440C and 17-4PH; steels including 1018, 1045, 4130, 4140, 4340 and A36; copper and brass grades such as C101, C110, C36000 and beryllium copper; titanium TA1, TA2 and TC4, plus Inconel and magnesium AZ31B / AZ91D; and plastics including ABS, PC, POM, PEEK, PA and carbon fibre.

If a material is on the edge of the process, that is a conversation, not a rejection. The earlier it happens, the cheaper the outcome.

• 1
  Aluminium 7075Expect some movement after heavy stock removal.
• 2
  Stainless 304Avoid light rubbing cuts; they work-harden the surface.
• 3
  Titanium TC4Heat stays in the cutter, so feeds and speeds matter more.