Design for manufacturability (DFM) means designing a part so it can be made economically by the process that will actually make it. In custom metal parts, four decisions carry most of the cost: the tolerances you call out, the feature geometry that dictates tooling and the number of setups, the material, and the finish. Most of a part’s unit cost is committed the moment the drawing is released — a machinist can optimise the last slice of it, but nobody can machine away a geometry that forces a fifth setup. These changes cost nothing in CAD and are expensive or impossible once tooling is cut.
Why is cost locked in at design release?
Because geometry decides process, and process decides price. A quote is arithmetic — material, cycle time, setups, tooling, inspection, finishing and yield — and every line traces back to a decision made in CAD. A part quoted high usually means the drawing asked for expensive things without meaning to.
Which tolerances actually need to be tight?
Only the ones that control fit, function or a mating interface. A tight tolerance on every dimension is the most common and most expensive mistake in custom metal parts, because the shop cannot tell which dimensions matter and must plan to hold all of them.
Cost does not rise linearly as tolerance tightens; it steps. Tighter than the general tolerance means finishing passes at reduced feed, then better workholding, thermal control and tool-wear compensation, then grinding or lapping, with inspection escalating to piece-by-piece CMM measurement and scrap rising alongside. Industry guidance commonly treats about plus or minus 0.005 in (0.13 mm) as the no-cost baseline, each tighter band carrying a real multiplier.
Give the drawing a sensible general tolerance block — ISO 2768-m is the usual choice for milled and turned metal parts, and geometric tolerancing to ASME Y14.5 often costs less than a tight plus-minus box — then spend individual tolerances only where they are earned:
- Bearing seats, press fits and sliding interfaces
- Features that locate a mating part in an assembly stack
- Sealing faces and O-ring grooves
- Datums other features are measured from
- Anything a standard or certification requires
How do setups and workholding drive machining cost?
Every extra orientation the part must be re-fixtured in adds a fixture or soft jaws, re-established datums, a separate program and a first-article check — plus stack-up error, since two features cut in one setup sit far more closely to each other than two cut in different setups. So put features on as few faces as possible, and keep the ones that must be tightly related on the same face. Leave something to hold, too: parallel flats or a sacrificial clamping boss cost almost nothing, while geometry only a bespoke fixture can grip pushes non-recurring cost into a small batch.
Why do internal corners, pockets and deep holes cost extra?
Because milling cutters are round, a milled internal corner can never be sharper than the tool that cut it. A sharp internal corner means wire EDM, broaching or a secondary operation on a feature that would otherwise be free. Specify a radius matching a common tool size and slightly larger than the tool radius, so the cutter rolls around the corner rather than dwelling in it, which is where chatter and tool marks come from.
Depth is the other half. Reaching the floor of a deep pocket pushes the cutter further out of the holder, and an end mill behaves like a cantilever: deflection under a given side load rises with the cube of the unsupported length and falls with the fourth power of the diameter. A deep narrow pocket therefore needs a long thin tool at reduced feed, and the same metal takes several times longer to remove. Holes behave the same way — standard drills are comfortable to about four or five diameters, past which the cycle breaks into pecks for chip evacuation, and beyond roughly ten diameters the feature needs gun drilling.
How much metal, and which metal?
Thin walls deflect away from the cutter instead of cutting cleanly, so they need light finishing passes and careful fixturing, and they release residual stress unevenly when material comes off one side, leaving the part bowed.
The opposite problem is a part machined from solid that is mostly air. If nine tenths of the billet becomes chips, you paid for that metal, paid to cut it away and paid the cycle time — the cue to consider a near-net-shape forged or cast blank. Our comparison of investment casting with CNC machining, and our guide to hot versus cold forging, cover that crossover.
Machinability is a cost input too. On the scales shops work from, free-cutting brass and 6061 aluminium sit at the top, 303 stainless well below them, 304 and 316 lower again, Ti-6Al-4V near the bottom. A tougher alloy means lower surface speeds, longer cycles, more heat at the cutting edge and faster tool wear, so the gap between an aluminium part and the same part in titanium is driven far more by cycle time and tooling than by bar price.
Do your threads and holes use standard tooling?
Standard drill and tap sizes are free; a thread outside the common metric or unified series means a special tap, procurement lead time and a special gauge. Engagement beyond roughly one and a half diameters in steel, or two in aluminium, adds little joint strength because the first engaged threads carry most of the load, while deep threads add cycle time, tap wear and the risk of a broken tap in a nearly finished part. Blind holes also need clearance below the last full thread, so avoid threading to the bottom of one.
Which finish and cosmetic callouts are you paying for?
Every roughness and cosmetic requirement is an operation. An as-machined surface lands around Ra 1.6 to 3.2 µm with no special effort; better means extra finishing passes, grinding, lapping or hand work. Specify a cosmetic grade only on faces visible in the finished product, and mark which they are — an undefined requirement gets priced as if it applied everywhere.
Coatings also move dimensions. Plating adds thickness on top of the surface; anodising converts part of the base metal, so roughly half the coating builds outward, a hole shrinks, a pin grows, and threads are the usual casualty. Allow for the growth in the machined dimension or mask the feature, and say which on the drawing; our surface treatment guide goes further.
Will a prototype design still be right at volume?
Often not, and it diverges both ways. A design optimised for one-off machining is cut from solid, with generous radii and tolerances a careful operator can hit by hand. A volume design starts from a near-net-shape blank, consolidates features into fewer setups, and uses tolerances the process is statistically capable of holding.
Switching process between prototype and production is therefore a re-qualification, not a substitution: a part machined from plate and one machined from a forging differ in grain flow and material condition, and for load-bearing hardware the test evidence must be regenerated, as our article on the five risks in moving from prototype to production describes.
A manufacturability review to run before you release the drawing
- Is every tight tolerance on a feature that controls fit, function or a standard?
- How many setups does the geometry force, and can features move onto fewer faces?
- Does every internal corner radius match a standard tool at that pocket depth?
- Is any hole deeper than about five diameters, and does it need to be?
- What share of the billet becomes chips, and would a forged or cast blank be cheaper?
- Are all threads standard series, and is any deeper than about two diameters?
- Has plating or anodising growth been allowed for on fits and threads?
Working with Power Honour
Power Honour is a Taiwan-based OEM and ODM manufacturer with more than 30 years in precision metal parts and safety hardware, running CNC machining, forging, casting, stamping, heat treatment and surface treatment in-house under an ISO 9001 quality system. Because those processes sit under one roof, a review here can say not only how to machine a part more cheaply but whether it should be machined at all. Send a STEP file and a dimensioned drawing, and our engineers will return a DFM review alongside the quotation.