How to Design Parts for CNC Machining

• 1
  Key takeaways
• 2
  Why design parts for CNC machining starts with the cutter
• 3
  How to design parts for CNC machining with sane tolerances
• 4
  Wall thickness, ribs and features that survive cutting force
• 5
  Fixturing, datums and design parts for CNC machining that hold still
• 6
  Material and finishing choices when you design parts for CNC machining
• 7
  A step-by-step DFM workflow
• 8
  Design limits by feature and material

A CNC mill removes material with a round tool. That single fact drives most of the rules in this article. Sharp internal corners cannot be cut by a rotating end mill, because the tool has a radius. If your model shows a square internal corner, the shop has to add a corner relief, change the tool, or run a secondary EDM operation. All three add cost.

The practical approach is to model the corner radius you are willing to accept. For a pocket 20 mm deep in aluminium, a 3 mm corner radius is normal and cheap. A 1 mm radius needs a smaller, less rigid tool, so the shop must slow the feed rate and take lighter passes. The cut still works, it just takes longer.

The same logic applies to the floor of a pocket. A flat-bottom end mill leaves a sharp internal edge at the wall-floor junction, which is fine. A ball nose tool leaves a scalloped floor, which may need a finishing pass if the surface is functional. Decide which faces are sealing surfaces and which are just clearance.

One more cutter constraint: tool length. A pocket 5× deeper than its width needs a long, slender tool that deflects under load. Keep depth-to-diameter ratios at or below 4:1 for aluminium and 3:1 for stainless steel where you can. If the geometry demands more, expect the shop to use a reduced feed rate or a smaller stepover.

• 1
  Internal corner radiusMatch it to a standard end mill: 1, 2, 3, 4, 6 or 8 mm.
• 2
  Pocket depthKeep depth under 4× the tool diameter for aluminium.
• 3
  Floor finishFlat floors machine faster than contoured ones.

Tolerance is the single biggest cost lever in a machined part. General tolerances of ±0.1 mm are easy to hold on most features. Tightening a feature to ±0.01 mm means the operator must check it, the machine must be thermally stable, and the inspection report must prove it. That work is real, and it shows up in the quote.

Map each tolerance to a function. A bearing bore that locates a shaft needs a tight fit, often ±0.005 mm or an H7 reamed hole. A cover plate that only keeps chips out can sit at ±0.2 mm with no consequence. When every dimension on the drawing carries the same tight tolerance, the shop has to treat the whole part as critical.

Watch for tolerance stack-up across a chain of features. If three dimensions each carry ±0.05 mm and they add up to a critical gap, the accumulated error can reach ±0.15 mm. Sometimes it is cheaper to tighten one datum and loosen the rest than to tighten all three.

Surface finish follows the same pattern. As-machined faces run Ra 1.6–3.2 μm and need no extra operation. A sealing face at Ra 0.8–1.6 μm takes a finishing pass. Below Ra 0.8 μm, the shop may need to polish or lap, which is a separate step and a separate cost line.

• 1
  General features±0.1 mm covers most non-critical dimensions.
• 2
  Mating bores±0.005 mm or an H7 fit for locating features.
• 3
  Cosmetic facesRa 1.6–3.2 μm as machined, no extra pass.

Cutting force pushes the workpiece around. Thin walls have little stiffness, so they spring away from the tool and then snap back, leaving a tapered or chattered surface. In aluminium, keep unsupported walls at 0.8 mm or thicker. In stainless and titanium, go to 1.5 mm or more, because those materials cut with higher forces.

If a design needs a thin wall for weight, add a rib or a temporary boss that the shop can machine away later. A 2 mm rib standing 10 mm tall adds stiffness without adding much mass. Tell the shop which features are temporary, or they may leave them in.

Holes have their own rules. A drilled hole is normally 1× diameter deep per peck, and standard drills reach about 5× diameter before the shop switches to a parabolic or gun drill. A hole 10× diameter deep in stainless steel is a special operation, not a routine one. Spot-face the entry if the hole must sit on a curved surface.

Blind holes need a drill point at the bottom. A flat-bottom hole requires an end mill, which costs more. If the hole is for a thread, allow the tap to run past the thread length. Add 3–5 mm of clearance at the bottom so the tap does not bottom out and break.

• 1
  Aluminium walls0.8 mm minimum unsupported.
• 2
  Steel and titanium walls1.5 mm minimum unsupported.
• 3
  Standard drill depthUp to 5× diameter before special tooling.
• 4
  Threaded blind holesAdd 3–5 mm of run-out below the thread.

A part must be held while it is cut. How you hold it depends on the shape you designed. A block with flat faces and parallel sides is easy to clamp in a vise. A thin curved shell with no flat surface needs a custom soft jaw or a vacuum fixture, and that fixture is a cost item.

Add clamping features when the geometry is awkward. Two small tabs on the outside of a housing let the shop bolt the part to a plate, machine the whole profile, then cut the tabs off in a final pass. The tabs cost a few minutes to remove and save the cost of a custom fixture.

Datums matter as much as clamps. Pick three orthogonal faces for your primary, secondary and tertiary datum and call them out on the drawing. If the shop has to guess which face locates the part, two setups will not agree with each other, and the part will fail inspection for reasons that have nothing to do with the machine.

For complex parts, a five-axis center can machine five sides in one setup. That removes the re-clamping error between operations. It is not always the cheapest route for a simple part, but for a part with features on several faces, one setup often wins on total cost.

• 1
  Simple blocksStandard vise, no fixture cost.
• 2
  Thin shellsAdd tabs or use a vacuum plate.
• 3
  Multi-face partsConsider five-axis for one-setup machining.
• 4
  AlwaysCall out datum A, B and C on the drawing.

Material choice sets the baseline for tool life, cycle time and achievable finish. Aluminium 6061 machines fast and takes a good finish, which is why it dominates prototypes and brackets. Stainless 304 is tougher and work-hardens, so the shop must keep the tool moving and avoid dwelling. Titanium Ti-6Al-4V needs slower speeds and more coolant, and it costs more per hour on the machine.

Pick the material for the end use first, then check machinability. A part that must resist corrosion may need 316L even though 6061 would machine faster. A part that sees high temperature may need Inconel, which is slow to cut and should be designed with generous radii and shallow pockets.

Plan the finish before the geometry is frozen. Anodizing adds 5–25 μm per surface depending on the type, which changes the size of a bore or a thread if those features are anodized. Mask critical bores, or cut them undersize so the coating brings them to print. Hardcoat anodizing builds more than clear anodizing, so the allowance is different.

Laser marking has a minimum character height of 1.5 mm. If you need a serial number or a logo on the part, leave a flat area at least that tall for the mark. Marking on a curved or rough surface gives an uneven result and may not read under the scanner.

• 1
  Prototypes and brackets6061-T6 aluminium is the default.
• 2
  Corrosion resistance316L stainless, but expect slower cutting.
• 3
  High temperatureInconel, with generous radii and shallow pockets.
• 4
  Anodized threadsMask or cut undersize for the coating build.