CNC design considerations: the first 5 that decide cost

• 1
  Tolerance: buy accuracy only where it does work
• 2
  Tool access: the real limit on part geometry
• 3
  Walls, floors and the stiffness of the part itself
• 4
  Features that drive setup count: holes, threads and datums
• 5
  Finish, edge breaks and the last operation on the routing
• 6
  Five CNC design considerations and where each one bites

Tolerance is the first of the CNC design considerations because it sets the price of every other feature. A cutter holds a size by removing material in a controlled loop, and the loop has limits: thermal growth, tool deflection, spindle runout, fixture rigidity. Ask for ±0.005 mm across a 300 mm aluminium part and the shop must slow the passes, add finishing cuts and measure more often. Ask for ±0.1 mm and the same part may run in one setup at full feed.

The practical rule is to tolerance the function, not the drawing border. Put a tight callout on the bearing bore, the sealing face or the mating spigot, and leave everything else at general tolerance. A single title-block note such as 'general tolerance ±0.1 mm' covers the rest. On our machines the floor is ±0.005 mm (±0.0002 in), but that number only holds over the features you have chosen to control.

Stack-up matters more than any single dimension. Three parts each held at ±0.05 mm can consume 0.15 mm of an assembly gap before anything is bolted. Calculate the stack before you tighten individual tolerances, and widen the non-critical links. If a fit still looks risky, ask for a capability study on the critical feature rather than a blanket tightening.

Inspection follows the same logic. We inspect 100% of parts before shipment, with raw material checks, in-process monitoring and a final inspection, and reports are available on request. But you should decide on the drawing which dimensions need reported values and which only need a pass/fail check. Reporting every dimension on a 40-feature part adds cost without adding information.

A CNC machine removes material with a spinning cutter of finite length and diameter, so any feature the cutter cannot reach has to be made another way or not at all. Deep pockets are the classic case. A pocket 60 mm deep with a 6 mm end mill needs a long, thin tool that deflects and chatters, and the floor will not come flat. Keep pocket depth below roughly four times the cutter diameter where you can.

Internal corners behave the same way. A cutter leaves the radius of its own profile, so a square internal corner demands a broach, an EDM burn or a filed corner that you then have to clean up by hand. Design a corner radius at least one third of the pocket depth, and no smaller than the smallest sensible cutter for that cavity. External corners cost nothing; internal ones do.

Undercuts and side-entry slots break the rule entirely. A T-slot needs a cutter entering from the side, which means an open path to that face. If the feature sits on a closed face, the drawing usually needs a split part or a change of process. Five-axis work helps here: with 16 simultaneous 5-axis machining centers we can tilt the tool and reach faces that a three-axis setup cannot, at the cost of a slower cycle.

The check is simple. Trace the tool path in your head from the stock face inward. If the path crosses material, the feature needs another process. Build that check into the model before release, not into a conversation after the first article.

A thin wall is not a drawing problem, it is a vibration problem. As the cutter passes, the wall deflects away from the tool, springs back and leaves a taper or a chatter mark. Aluminium walls below about 0.8 mm and steel walls below about 1.2 mm start to need light finishing passes, support from the fixture, or both. Stay above those numbers unless the wall is short and well supported.

Floor thickness has the same floor limit but a different failure mode. A thin floor drums under cutting load and never sits flat. It also distorts when you unclamp it, because the internal stress released from the stock was being held straight by the vise. Keep floors at 1 mm or more for aluminium and 1.5 mm or more for steel where the part is not supported underneath.

Stock choice sets much of this. A part cut from 7075 plate behaves differently from the same part cut from 6061, and a casting behaves differently again because the skin is harder than the core. Materials we run daily include 6061, 2024, 5052, 6082, 7075, 303 and 316 stainless, 4140 and 4340 steel, Ti-6Al-4V, Inconel and PEEK. Each one changes the wall and floor numbers, so confirm them against the material rather than copying a rule from an aluminium part.

When the geometry forces a thin section, the answer is usually sequencing rather than redesign. Rough, stress-relieve, then finish. Leave material on the wall for the finishing pass, and hold the part on a face that will not be machined. That costs a setup, but it is cheaper than a scrapped batch.

Every face you machine from a new direction is another setup, and each setup adds position error and labour. A part that can be made in two setups is usually far cheaper than one that needs five. Group features on the faces you already have to reach, and put holes on the same face as the pocket they sit beside.

Hole depth is the most common cost trap. A drilled hole can run about three times its diameter deep before chip evacuation becomes unreliable; a tapped hole wants even less. Beyond that, the shop pecks, the drill wanders and the tap breaks. Specify thread depth and drill depth separately, and allow a cone at the bottom of blind holes for the drill point.

Threads should be called out by standard, not by pitch diameter. Metric and Unified threads are cut with a tap or a thread mill, and both want clearance at the entry. Add a chamfer or a countersink at the start of every tapped hole. For very hard materials such as Inconel or 440C, expect thread milling rather than tapping, which changes the cycle time but not the drawing.

Datums deserve the same discipline. Pick three orthogonal datum faces and dimension from them, not from the centre of a feature that will itself move. On a part with a true position callout, the datum scheme is the whole game: a poor choice makes a good part look out of tolerance, and a good choice lets a normal process capability pass the check.

Surface finish is specified as Ra and produced by a combination of tool, feed and pass count. As-machined aluminium sits around Ra 1.6–3.2 μm. A deliberate finishing pass reaches Ra 0.8–1.6 μm. Below that, Ra 0.2–0.8 μm, you are into fine finishing or a secondary process, and the cost rises with the area involved. Specify finish by zone on the drawing, not as one global note.

Edge breaks are a safety and assembly issue, not cosmetics. A sharp machined edge cuts gloves, damages mating parts and creates a stress riser on a loaded component. A 0.2–0.5 mm chamfer or a 0.3–0.5 mm radius on every external edge covers most cases. Note the edges you want left sharp, because a deburring pass touches everything it can reach.

Coating and plating go on last, but they change dimensions. Anodizing builds 5–25 μm per surface depending on the type, and hardcoat builds more. Electroless nickel, zinc and silver plating all add thickness. On a tight bore, that growth is the difference between a slip fit and a press fit, so tell the shop which surfaces must stay bare or be masked.

Laser marking is a finishing operation too, and it needs room. Minimum character height is 1.5 mm, and the mark should sit on a flat, machined face rather than a curved or as-cast surface. Put the marking callout on the model with a defined face, and keep it away from sealing faces and wear surfaces.