Design for manufacturing

Why it matters

Most of a product's cost is locked in during design, long before anyone cuts metal. A feature that takes a designer ten seconds to draw can add a second machine setup, a special tool or a scrapped mould. Design for manufacturing (DFM) means designing parts that are easy to make well, and design for assembly (DFA) means making them easy to put together. Good DFM does not make parts worse; it removes cost and risk that add nothing to function.

DFM for CNC machining

• Inside corner radii. Milling cutters are round, so pockets always have radiused inside corners. Give inside corners a radius a little larger than a standard cutter radius (for example, R3.5 mm when a 6 mm cutter is used) so the tool does not have to stop in the corner.
• Pocket depth. Deep, narrow pockets need long tools that deflect and chatter. A common rule of thumb is to keep pocket depth within about 3 to 4 times the cutter diameter.
• Standard hole sizes. Use standard drill and tap sizes. Specify thread depth rather than threading to the bottom of a blind hole, and give tapped holes room for the drill point.
• Minimise setups. Every time the part is flipped or re-clamped costs time and adds error. Put features on as few faces as possible.
• Wall thickness. Very thin walls vibrate and bend during cutting. In metals, walls under about 1 mm are difficult; plastics need more.
• Tolerance only what matters. Use a general tolerance note (such as ISO 2768-m) for everything else.

DFM for sheet metal

• Keep bend radii at or above the material thickness for most steels and aluminium, and use the same radius throughout so one tool does all bends.
• Keep holes at least about 2 times the thickness away from bends, or they distort.
• Add bend reliefs where a bend meets an edge to stop tearing.

DFM for injection moulding

• Uniform wall thickness. Thick sections cool slowly, causing sink marks, voids and warping. Core out thick regions and use ribs instead.
• Draft. Add a draft angle (often 1 to 2 degrees, more for textured surfaces) to walls in the direction the mould opens so the part releases.
• Ribs are typically about 50 to 60 % of the wall thickness they join to avoid sink on the other face.
• Avoid undercuts that need side actions in the mould, or design snap fits that can be moulded simply.

DFA in brief

• Fewer parts. Ask of each part: does it move relative to its neighbours, does it need a different material, or does it have to come apart for service? If not, it might be combined with another.
• Fewer fastener types. One screw size throughout means one driver and fewer mistakes.
• Self-locating features (pins, tabs, chamfers) and mistake-proofing (poka-yoke): parts that only fit one way.
• Top-down assembly so gravity helps.

Worked example: improving a machined bracket

A first design of an aluminium bracket has:

1. A rectangular pocket 40 mm deep with sharp inside corners.
2. Tapped holes on four different faces.
3. Every dimension at ±0.01 mm.
4. Two M5 and two M6 tapped holes.

Improvements:

1. Add R5 inside corner radii (a little larger than the 4 mm radius of an 8 mm cutter) and, if function allows, reduce the pocket depth to 24 mm so a standard 8 mm cutter stays within about 3 times its diameter.
2. Move the holes onto two opposite faces, so the part needs two setups instead of four.
3. Keep ±0.01 mm only on the bore that locates a bearing; put the rest under a general tolerance note.
4. Use four M6 holes, so one tap and one screw size cover the assembly.

Each change is small; together they can cut machining time substantially. The best way to confirm is to ask a machinist or get quotes before and after: many online manufacturing services give instant quotes and automated DFM feedback.

Talk to the people who make it

Machinists, toolmakers and moulders know what is easy and what is expensive. Showing them a design early, and asking "what would make this easier to make?", is one of the most valuable habits an engineer can build. Their workshops are also hazardous places: visit with permission, wear the required PPE and never touch machines you have not been trained and authorised to use.

Common mistakes

• DFM at the end. By the time a design is "finished", changes are expensive.
• Copying a part designed for another process. A machined design rarely moulds well.
• Cutting cost by removing function. DFM keeps the function and removes the waste.
• Ignoring inspection. A feature you cannot measure is a feature you cannot accept.

Recap

• Design inside corners, pocket depths, holes and walls for the tools that will make them.
• Sheet metal: consistent bend radii, holes away from bends, reliefs.
• Moulding: uniform walls, draft, thin ribs, no unnecessary undercuts.
• DFA: fewer parts, fewer fastener types, self-locating, mistake-proof.

Try it

On the Do tab, review a part design against a DFM checklist and redesign it in CAD or on paper.