On this page
Design for manufacturability (DFM) means designing a part so it is easy, quick and cheap to make, without losing anything it needs to do. It matters because the design decides most of the cost: once the drawing is released, the material, the process, the number of setups and the tolerances are largely fixed. A change on screen costs minutes; the same change after tooling is made costs weeks.
General principles
- Know the process before you model. A part designed for machining looks different from the same part designed for sheet metal, casting or moulding. Decide early.
- Simplify the shape. Every extra feature is extra time. Ask whether each one does a job.
- Use standard features and parts: standard hole sizes, thread sizes, bend radii, fasteners and stock sizes.
- Tolerance only what matters. Tight tolerances and fine finishes multiply cost; apply them only to functional features.
- Choose an easy material that the process and suppliers handle well. Free-machining steel and 6082 aluminium machine much faster than stainless steel.
- Reduce setups. Put features on as few faces as possible, so the part can be made in one or two clampings.
Design for assembly (DFA)
Parts cost money to make, but they also cost money to handle, fit and fasten. Fewer parts mean fewer drawings, less stock, less assembly time and fewer things to go wrong. For every part, ask: does it move relative to the others? Does it need to be a different material? Does it need to come apart for service? If the answer to all three is no, it can probably be combined with a neighbouring part.
- Replace screws with snap fits, hinges with living hinges or bent tabs, and welded brackets with one bent part where loads allow.
- Make parts self-locating (tabs, slots, chamfers and dowels) so they can only go together one way.
- Make parts symmetrical where possible, or clearly asymmetrical, so they can’t be fitted wrongly.
- Assemble from one direction, ideally from the top down.
- Use the same fastener size throughout, so one tool does every job.
Process rules
Machined parts
- Give internal corners a radius slightly larger than a standard cutter (for example R3 for a 5 mm cutter), and avoid sharp internal corners entirely.
- Keep pocket depth below about four times the cutter diameter, and hole depth below about five times the drill diameter.
- Use standard drill, reamer and thread sizes; give blind tapped holes extra drilled depth beyond the thread.
- Add flat spot faces where a drill or a bolt head meets a sloping or curved surface.
- Avoid thin walls (below about 1 mm in aluminium) that chatter while cutting.
Sheet-metal parts
- Use an inside bend radius at least equal to the sheet thickness, and the same radius on every bend.
- Make flanges at least about four times the thickness long, so the press brake can grip them.
- Keep holes at least 2t + R from a bend (t = thickness, R = bend radius), or they stretch into ovals.
- Make holes at least as wide as the sheet is thick, so the punch doesn’t break.
- Add bend reliefs where a bend ends at an edge, to stop tearing.
Moulded and cast parts
- Keep walls uniform; core out thick sections and add ribs instead.
- Add draft to every face parallel to the mould opening (0.5–2° for plastics, 1–3° for castings).
- Avoid undercuts that need side actions, or design them to release with a flexible snap.
- Round all corners: an inside radius of about half the wall thickness.
3D-printed parts
- Orient the part so the main loads run along the layers.
- Keep overhangs within about 45° of vertical, or design in chamfers to avoid supports.
- Leave 0.2–0.3 mm clearance for fits, and use inserts for threads that are used often.
Worked example: checking a sheet-metal bracket
A bracket is folded from 2 mm steel sheet. The design has a 1 mm inside bend radius, a 6 mm flange and a ⌀6 mm hole whose edge is 3 mm from the bend. Check it against the sheet-metal rules.
Step 1: bend radius. The minimum is about t = 2 mm. The design’s 1 mm is too tight for mild steel and may crack on the outside of the bend. Change it to 2 mm.
Step 2: flange length.
The design’s 6 mm flange is too short for the press brake. Make it 8 mm.
Step 3: hole distance from the bend. With the new 2 mm radius:
The hole is only 3 mm from the bend, so it would distort. Move it to 6 mm, or cut it after bending.
Step 4: hole size. ⌀6 is larger than the 2 mm thickness, so it can be punched. ✓
None of the three changes affects how the bracket works, but together they avoid cracked bends, a flange the press can’t form and an oval hole, any of which would scrap parts.
Getting manufacturing input early
The best DFM check is a conversation. Send the 3D model to the machinist, fabricator or mould maker while the design can still change, and ask what would make it cheaper or more reliable to make. In CAD, sheet-metal and mould tools flag many problems automatically: flat patterns that won’t unfold, bends too close to holes, missing draft and thick sections.
Key points
- The design fixes most of a part’s cost; check manufacturability before the drawing is released.
- Fewer parts, standard features and one-direction assembly save more than any process tweak.
- Every process has its own rules: inside radii for milling, bend radius and flange length for sheet metal, uniform walls and draft for moulding.
- Tolerance and finish only the features that need them.