CNC design basic skills: how to prepare a part for the shop floor

• 1
  Key takeaways
• 2
  Start with the CNC design basic skills that set the toolpath
• 3
  Tolerance strategy: spend accuracy where it matters
• 4
  Reduce setups and keep tool access open
• 5
  Threads, holes and small features
• 6
  Match material and finish to the function
• 7
  Step by step: a design review you can run yourself
• 8
  Practical limits by feature and material

A CNC machine removes material with a spinning cutter of fixed size. That single fact drives most design rules. Every internal corner carries the radius of the tool that cut it. Every pocket must be wide enough for the cutter body to enter, and every floor must be reachable along the Z axis. If a feature cannot be reached by a cylinder, it cannot be milled.

The practical limit is depth-to-diameter ratio. For end mills, 3× diameter is comfortable. Between 3× and 4× you need a reduced-neck tool and lighter passes. Past 4×, deflection grows fast, surface finish drops and the tool may snap. For drilled holes, 8× diameter is routine; beyond that we step-drill or use a gun drill.

Wall thickness matters as much as feature size. Thin walls vibrate under cutting load. In aluminum, 0.8 mm walls are stable if the part is supported. In stainless or titanium, keep 1.5 mm or more, because cutting forces are higher and spring-back causes chatter.

Design the part so the tool can approach from as few directions as possible. A part that can be machined from three sides is cheaper than one needing six. If a feature only exists to look good, ask whether it can be removed.

• 1
  Internal corner radiusAt least 1/3 of pocket depth, and never smaller than the cutter you can actually buy.
• 2
  Pocket depthKeep under 4× the smallest corner radius whenever the drawing allows.
• 3
  Floor radiusSpecify a corner radius instead of a sharp internal floor; sharp floors need EDM.
• 4
  Thin walls0.8 mm in aluminum, 1.5 mm in steel and titanium, or add ribs.

CNC holds ±0.005 mm in the right conditions, and we inspect 100% of parts before shipment. But tight tolerance is not free. It costs extra passes, temperature control and more inspection time. The design question is not how tight you can go, but which dimensions carry function.

Pick one primary datum surface that is flat and machined first, then a secondary and tertiary datum. Dimensions should chain from those datums, not from a cast or saw-cut face. When a drawing has no datums, the shop invents them, and two suppliers can produce two different parts that both pass the drawing.

Use general tolerance for everything else. A note like ISO 2768-m covers non-critical dimensions and removes dozens of tolerance callouts. Reserve the tight tolerances for mating bores, bearing seats, seal grooves and pivot holes.

Geometric callouts should be few and meaningful. Flatness on a sealing face matters. Flatness on a bracket that bolts to a rubber pad does not. Each GD&T frame adds a measurement step, so three well-chosen frames beat fifteen.

• 1
  Datum AThe first machined face; make it large and flat.
• 2
  General toleranceLet ISO 2768-m or an equivalent block tolerance handle the rest.
• 3
  Bearing and seal boresThese justify ±0.005 mm and Ra 0.2–0.8 μm.
• 4
  Cosmetic facesRa 1.6–3.2 μm as machined is usually enough.

Every setup means the part is unclamped, turned or flipped, and re-zeroed. That adds fixture cost, cycle time and stack-up error. A part designed for two setups instead of five can cut unit cost by a wide margin on small runs.

Design in a clamping allowance when the part is small or has no flat face. A 3 mm sacrificial tab on a bar, or a boss that is later milled off, gives the vise something to grip. Without it, the shop has to build a soft jaw or a vacuum plate, and that cost lands in your quote.

Undercuts and side-entry grooves are the usual blockers. A T-slot cutter can reach them, but only if the shank clears the wall above. Check the shank diameter, not just the cutter head. If the opening is narrower than the shank, the feature cannot be cut from that direction.

Harmonize hole sizes. Using M6, M8 and 6.5 mm holes on one plate means three tool changes and three drill cycles. Standardizing to two sizes saves machine time on every part in the run.

• 1
  Setup countTwo or three setups is normal; five or more is a red flag.
• 2
  Clamping tab3 mm sacrificial tab for small parts with no flat grip.
• 3
  Shank clearanceThe tool holder body needs clearance above the cutter.
• 4
  Tool countFewer unique hole diameters means fewer tool changes.

Blind tapped holes need a thread relief or a deeper drill. The rule we use: drill depth equals thread depth plus 0.5× diameter, and the tap needs a lead of about 3 pitches below the last full thread. An M6 thread 12 mm deep needs a drilled hole around 18 mm. Without that, the tap bottoms out and either breaks or leaves a partial thread.

Thread callouts should name the standard. M6 × 1.0 is clear. A note that just says M6 leaves pitch to the shop. For inch threads, specify UNC or UNF and the class. Class 2B is normal; class 3B needs gauging and costs more.

Micro features are possible but slow. Slots under 0.5 mm wide, holes under 1 mm, and text under 1.5 mm character height all need small carbide tools run at high spindle speed with light depth of cut. They break easily, so keep them away from deep pockets.

If a hole is only a clearance for a bolt, do not tolerance it tightly. A 6.6 mm hole for an M6 bolt is fine at ±0.1 mm, and boring it to ±0.02 mm just adds cost.

• 1
  Blind hole depthThread depth plus 0.5× diameter for drill, 3 pitches for tap lead.
• 2
  Thread reliefA shallow groove at the thread end prevents tap breakage.
• 3
  Minimum text height1.5 mm for laser marking; machined text needs 3 mm.
• 4
  Clearance holesKeep them loose; ±0.1 mm is enough.

Material choice changes the design limits. Aluminum 6061-T6 machines fast and holds thin walls well, which makes it the default for prototypes and enclosures. Stainless 304 and 316 resist corrosion but work-harden, so avoid rubbing cuts and keep feed per tooth high enough to stay under the hardened layer.

Titanium Ti-6Al-4V and Inconel are for high temperature or high strength needs. Expect slower cutting, more tool wear and shorter reachable depths. If the part does not need the strength, switching to 4140 steel or 7075 aluminum can cut both cost and lead time.

Surface finish interacts with tolerance. A Ra 0.2–0.8 μm bore usually needs a separate finishing pass or a reamer, and anodizing after that can shift the dimension by a few micrometres. If a bore must stay at ±0.005 mm after hardcoat anodizing, tell the shop before machining so the pre-plate size can be adjusted.

For laser marking, keep character height at 1.5 mm or more and place it on a flat milled face. Marking on a curved or as-cast surface gives uneven line width.

• 1
  6061-T6Best default for prototypes and thin-wall parts.
• 2
  316LMedical and marine; expect slower feeds.
• 3
  Ti-6Al-4VUse only where strength-to-weight justifies the cost.
• 4
  AnodizingHardcoat adds thickness; account for it on tight bores.