CNC machining design guide for electrical parts

Start with the blank, not the finished shape

A machined part is cut from a blank, and the blank sets the material cost, the number of setups and the amount of metal that becomes chips. A part designed as a rectangular housing from a plate may be cheaper as a turned body with a milled flat, and a part designed from a solid block may be cheaper as an extrusion with a light skim.

Ask what stock the supplier can buy. A near-net extrusion or a cast blank reduces machining time but adds a tooling cost and a lead time. A standard plate or bar is available immediately but removes more material. The crossover depends on volume, and it is worth checking before the geometry is frozen.

For copper and brass, the blank also matters for grain direction and for residual stress. A part machined from a heavily worked plate can distort when one face is removed and the balance of stress changes. Rough machine, stress relieve where the alloy allows, then finish.

Internal corners follow the cutter

A vertical internal corner cannot be sharper than the radius of the cutter that makes it. A 6 mm end mill leaves about a 3 mm corner radius. A drawing that calls a sharp internal corner forces either a smaller cutter, which is slower and more fragile, or an EDM operation, which adds cost and lead time.

• Set internal corner radii at or above one third of the pocket depth where possible. Deep, tight corners need a long, thin cutter that deflects.
• Use a standard cutter radius from the supplier's tool list rather than an arbitrary value. A 3 mm or 4 mm corner is easier to quote than 2.7 mm.
• Add a floor radius at the base of a pocket. A sharp internal base corner is a stress raiser and a difficult cut.
• Round external corners too. A sharp external corner is easy to machine but damages handling, insulation and plating rack contacts.
• Keep pocket depth below about four times the cutter diameter for a safe, productive cut. Beyond that, expect a smaller cutter, a longer cycle and more chatter risk.

Walls, floors and thin sections

A thin wall moves away from the cutter. As the tool passes, the wall deflects, the chip load changes and the surface shows chatter or a taper. In copper, the effect is pronounced because the material is soft and compliant. In aluminium, it is similar but the cutting forces are lower.

A working floor for a machined wall is about 0.8 mm for a stiff alloy and about 1.0 mm for copper at a moderate depth. Below that, the process needs light radial cuts, a support material, or a change of route to stamping or wire forming. These are starting points, not rules, because the height of the wall and the support at its base change the answer.

A thin floor behaves the same way. A floor under a pocket deflects when the cutter pushes on it, and the finished thickness varies across the part. Leave enough material for a finishing pass and support the floor from below where possible. If the floor is a sealing or contact face, machine it last.

Holes, threads and depth

A drilled hole is straightforward up to a depth of about three times its diameter. Beyond that, the drill wanders, the chip packs and the coolant struggles to reach the tip. A deep hole needs a peck cycle, through-tool coolant or a gun drill, and each of those adds cost.

A tapped hole needs a thread depth and a drill depth, and they are not the same. Leave at least three to five pitches of drill depth beyond the full thread so the tap can lead in and the chip can clear. A blind hole with no relief at the shoulder will not accept a fastener with a square end.

Small holes in copper are prone to burrs at breakout. A burr inside a bore that carries a cable will damage the insulation during assembly, and a burr on a contact face raises the resistance. Specify the deburr requirement and say which edges are functional.

Cross holes break into a main bore and leave a sharp intersection. That edge is hard to deburr and is a common crack initiation point under vibration. A small chamfer or a radius at the intersection, called out on the drawing, is cheaper than a manual rework step.

Every face is a setup

A three-axis machine can reach one face at a time. A part with features on four sides needs four setups, or a five-axis machine, or a fixture that indexes the part. Each setup re-establishes a datum and adds error.

Design the part so the critical features are on one face, or on faces that can be machined in one setup. If a bore and a mounting face must be perpendicular, put them in the same operation. If a hole pattern only needs clearance, put it on the cheaper face.

Count the setups before you count the features. A part with twenty features on one face is usually cheaper than a part with six features spread over three faces, because the setup cost dominates at low and medium volume.

Edges, burrs and electrical function

An electrical part has three edge requirements that a mechanical drawing often misses. First, any edge that touches insulation must be rounded or chamfered, because a sharp edge cuts through the insulation under vibration. Second, any edge on a current path must be free of burrs, because a burr is a thin section that heats and can arc. Third, any edge handled during assembly must be deburred for safety.

A typical callout is a 0.2 to 0.5 mm radius on external edges and a chamfer on a bore entry. The exact value depends on the part. State it once in a general note and add specific calls where the edge is functional. Do not rely on a generic 'deburr all edges' note, because it gives the inspector nothing to measure.

Plating changes the edge condition. A sharp edge receives a thicker deposit because the current density is higher there, and a burr can be encapsulated rather than removed. If the part is silver plated, the pre-plate deburr decides the plated edge.

Datums and tolerance discipline

Machining follows the datum. If the drawing nominates a datum that is not a real locating surface, the inspector and the machinist will use different references and the part will be argued about rather than accepted.

Choose the datum from the function. A part that mounts on a face and locates on a bore should use that face as the primary datum and the bore as the secondary. A part that plugs into a connector should use the mating face and the keyway. Then apply the tight tolerances only to the features that touch the mating part.

A general tolerance such as ISO 2768-m covers the rest. A drawing with every dimension at a tight tolerance is a drawing with no priority, and it will be quoted high because the supplier has to assume every feature is critical.

Material and finish choices

Copper is chosen for conductivity, brass for machinability, and aluminium for weight and thermal performance. Each brings a machining consequence. Copper galls and needs sharp tooling. Brass machines freely but may be restricted on lead content. Aluminium is soft, builds a built-up edge on a dull tool and can distort when a lot of material is removed.

Finishing is part of the design. Tin plating on copper gives a solderable, corrosion-resistant surface but adds thickness to threads and bores. Silver plating gives the lowest contact resistance but tarnishes and costs more. Anodising on aluminium adds a hard, insulating layer that must be masked at any earthing point.

State the finish, the thickness and the masked areas. A finish note that says 'tin plated' without a thickness leaves the supplier to choose, and the thread may not gauge after plating.