Design for Machining — Twelve Practical Rules
A part that looks perfect on screen may be unmakeable on the shop floor, or three times more expensive than it needs to be. Twelve rules that cut machining cost without costing function.
A cutting tool is a rotating cylinder. Every DFM rule follows from that one sentence.
1. Internal corners cannot be sharp
A cutter is round, so every pocket has rounded corners. Model a sharp corner and it either cannot be made, or it gets made by wire EDM at several times the cost.
Rule: make internal corner radii at least one third of pocket depth, and preferably match a standard tool: R3, R5, R6, R8.
A larger radius means a larger cutter, faster removal, lower cost. R2 in a 40 mm pocket forces the shop to clear the whole pocket with a 4 mm end mill.
2. Limit pocket depth
The longer the tool, the more it chatters and the less accurate it is.
Rule: pocket depth at most 3 to 4 times cutter diameter. A pocket 60 mm deep and 12 mm wide is effectively unmakeable.
3. Pocket floors are rounded, not flat
A ball-nose end mill does not leave a perfectly flat floor. If you need a flat floor, say so — the shop uses a flat-bottom tool. If you do not, model the floor radius.
4. Keep holes shallow
Rule: hole depth at most 4 times diameter with a standard drill. Beyond that you need special drills and peck cycles.
Also: avoid non-standard diameters. Ø10 is a standard drill; Ø10.3 needs reaming or boring.
5. Do not make threads blind and deep
A blind thread means the tap has to stop at the bottom — a broken-tap risk.
Rule: thread depth at most 2 to 3 times bolt diameter. An M8 thread deeper than 24 mm adds no strength; the bolt fails before the thread does.
And for a blind hole, leave 3 to 5 mm of extra depth past the thread for the tap to run out into.
6. Design in the clamping faces
The part has to be gripped somewhere. If every face is sloped or curved, the shop must build a fixture and that cost lands on your part.
Rule: provide at least two parallel flat faces, or one flat face plus a locating hole.
7. Minimise the number of setups
Every time the part is unclamped and re-fixtured, time is lost and error enters.
Rule: design holes and pockets on one or two faces wherever possible. A part needing machining from five sides costs five times one that finishes from one.
8. Eliminate undercuts
An undercut is a region the tool cannot reach from above. Making it needs special tooling, wire EDM or sinker EDM.
If genuinely required — a retaining-ring groove, say — use standard dimensions. If not, remove it.
9. Avoid thin walls
A thin wall chatters and deflects under tool pressure.
Rule: minimum wall thickness 0.8 mm for metal and 1.5 mm for plastic. More for tall walls.
10. Reserve tight tolerances for faces that work
This is the most expensive mistake. Every step tighter raises cost non-linearly. Read tolerancing properly.
11. Keep text and engraving simple
Engraving is milled and takes time. If a part number is needed, laser marking or stamping after machining is cheaper.
12. Start from standard stock sizes
If your part is 48 mm in diameter, the shop starts from 50 mm bar and turns 2 mm away. Design it at 50 and machine only where needed: less material, less time.
The same applies to sheet (standard thicknesses), tube (standard diameters) and profile.
A quick checklist before sending
- [ ] Do all internal corners have radii, and are those radii standard?
- [ ] Is no pocket deeper than 4× its width?
- [ ] Do all holes use standard drill diameters?
- [ ] Are thread depths sensible, with run-out space in blind holes?
- [ ] Is the part machined from at most two directions?
- [ ] Are there two flat faces to clamp on?
- [ ] Are tight tolerances only on working surfaces?
- [ ] Do the starting dimensions match available stock?
If you have a model you want reviewed before ordering, send it over. There are usually two or three small changes that take ten to thirty percent off the manufacturing cost without the part working any worse.