Design for machining: which features quietly double the cost of a CNC part?

What should a design for machining review check before a part goes out for quote?

Check five things in order: how many directions the tools must approach from, whether every pocket and corner can be reached by a standard cutter, whether holes and threads are standard sizes, whether walls are stiff enough to cut, and whether tight tolerances sit only on features that need them.

The order matters because the early items decide the later ones. Setup count is set by geometry, and it also decides which features end up toleranced to each other across two clampings, which is where tight position tolerances get expensive. Tool access decides cycle time. Hole and thread sizes decide whether the job runs on tools already in the magazine. The table below is the working checklist; the sections after it explain the rows that cause the most trouble. The values are rules of thumb that most shops recognize, not limits from a single standard, so treat them as the point where a conversation with the supplier should start.

How do you count the setups a part really needs?

Count every direction a tool has to come from, then count each one as a separate clamping unless the shop can show it reaches that face another way. Most of the savings available in design for machining come from reducing that count.

On a three-axis mill, a block with features on the top face and holes on one side is two setups. Add a tapped hole on the bottom and a cross-hole on the end and it becomes four, each with its own fixture, indicating step and first-piece check. Every transfer also adds error between features cut in different clampings, so a tight position tolerance between a top-face bore and a side-face hole costs much more than the same tolerance between two holes on the same face. If those features must relate tightly, try to put them on the same face, or reference them to a datum that both setups can pick up, as described in the guide on concentricity, runout and position.

Turned parts have their own version of the count. A round part whose features all lie on its axis comes off a lathe in one cycle; a flat, an off-axis hole or a slot across the diameter either needs live tooling or a second operation on a mill. A useful habit is to mark up a print with one color per approach direction before sending it out. Faces that carry only one small feature are the first candidates to eliminate or move.

Five-axis machining reduces clampings, but it is not free: the machine time is more expensive and fewer shops offer it. Design so that a three-axis shop can make the part in two or three setups, and treat five axes as an option rather than a requirement unless the geometry truly needs simultaneous motion.

Which features silently double the cost of a machined part?

The features that can double a part’s cost are rarely the hard ones the designer noticed. They are small defaults that force a special tool, an extra setup or full inspection on every dimension.

• Sharp inside corners in pockets, drawn that way because the CAD sketch defaulted to them. They force EDM, a deviation request or a quoting question.
• A tight title-block tolerance applied to every dimension. A general note such as ISO 2768-m covers non-critical sizes without a tolerance on each one (the “K” often added for geometry comes from ISO 2768-2, withdrawn in 2021 and replaced by ISO 22081); see the cost of tight tolerances.
• A fine roughness symbol in the title block instead of on the seal or bearing face that needs it. Every surface then gets a finishing pass.
• One small feature on an otherwise empty face, such as a single tapped hole on the back, which adds a whole clamping.
• Non-standard threads or odd hole sizes that need their own tools and gauges.
• Thin, tall walls or thin floors under a deep pocket, which deflect while being cut and need slow spring passes to hold size.
• Engraved or raised text machined into the part when a pad-printed or laser mark, or no mark, would do.
• “Break all sharp edges” left undefined, or every edge given its own radius. The edge note guide shows how to bound it.
• Cosmetic requirements on hidden faces, which turn a functional part into one that has to be handled and inspected like a visible one.

None of these change the function of most parts. That is the point of the checklist: each one costs money, and the designer rarely meant to pay for it.

What should a supplier’s design for machining review send back?

A useful review comes back as a marked-up copy of your own drawing and a short written list of changes that lower cost or risk, each one optional. It should also say plainly when a feature is outside what the shop runs.

At Saola, drawing review produces a marked-up copy of the customer’s drawing and a short written list of DFM notes, both described on the quality page. Round bar and tube parts run on the CNC lathes at our lead CNC plant, and parts that need heavy off-axis milling or pocketing are routed to CNC milling at the same plant rather than forced onto a lathe, as the CNC turning page states. Milling here is mainly the second operation on castings, not general billet machining, and simultaneous five-axis machining is not offered on any process. If a design depends on five-axis access, the review will say so instead of quoting around it. The milling page also lists drawing changes that cut machining cost on castings: one datum scheme on both the casting and machining drawings, which keeps the work to one setup, and bores sized to standard reamer and boring-bar diameters, which avoids a custom tool or a slower interpolated cut.

Whichever supplier quotes the part, compare the notes that come back against this checklist. A review that only repeats the price without naming a single feature has not looked at the geometry.