Design rules that make a CNC part cheaper
Most of the price of a machined part is decided before the RFQ is sent — by how many set-ups the geometry forces, how much material has to be removed, and how many tolerances are tighter than the function needs. These are the rules we apply when we review a drawing.
Geometry rules
Workable starting points for aluminum, steel and engineering plastics. They are not laws — but a part that breaks several of them needs a reason.
| Feature | Practical rule | Why it matters |
|---|---|---|
| Wall thickness | 0.8 mm minimum in aluminum, 1.0 mm in steel, 1.5 mm in plastics | Thinner walls deflect under cutting force and chatter, so the cut has to be slower |
| Internal corner radius | At least one third of the pocket depth, and never smaller than the cutter radius | Sharp corners need EDM; a 3 mm cutter cannot leave a 1 mm corner |
| Pocket depth | Up to 4× the cutter diameter | Deeper pockets need long, thin tools that cut slowly and drift |
| Hole depth | Up to 10× diameter for standard drilling | Beyond that you are into gun drilling or EDM, and the price changes |
| Blind hole bottoms | Flat-bottomed holes need a second tool; drill point is the default | Specifying a flat bottom on a deep hole adds an operation |
| Threads | M2 and above; thread depth 1.5–2× diameter | Small threads break taps and force slow cycles |
| Undercuts | Avoid on the main axis; use a relief groove if the function allows | Undercuts need special tooling or a second set-up |
| Thin floors and webs | 0.5 mm minimum, 1 mm preferred | Thin sections vibrate and spring back after the cut |
| Text and engraving | Use a standard cutter width and 0.2 mm minimum depth | Fine engraving with a 0.2 mm tool takes as long as the real features |
Tolerance and datum strategy
Tighten only what the function needs. A blanket ±0.02 mm on every dimension turns a straightforward part into an inspection project, and it does not make the assembly any better. Put the tight tolerance on the two features that actually locate the part, and let the rest sit at general tolerance.
GD&T communicates intent better than plus/minus, once the datum reference frame is real. Choose three mutually perpendicular faces that are machined in one set-up — if the datums can only be reached in different operations, the tolerance will be measured across setups and the stack-up will surprise someone. Position and profile callouts with a maximum material modifier also let the inspector use functional gauges instead of a full CMM program.
Finally, tell us which dimensions are critical. When a drawing has a hundred dimensions and no priority, everything gets inspected and nothing gets optimized. Two or three flagged CTQ features let us plan the routing, the fixtures and the inspection plan around them — usually at a lower piece price than a drawing where every tolerance is equally sacred.
Checklist before you send the RFQ
3D model in STEP, IGES or SLDPRT; 2D drawing in PDF, DWG or DXF with tolerances and GD&T; material and grade; surface finish and where it applies; quantity and whether it is a prototype or a repeat order; the date you need the parts in hand; and any documentation your quality team will ask for — first article, CMM data, material certificate, RoHS or REACH declaration.
Missing items do not stop the quote, but they change it. A quote issued without a finish or a tolerance requirement is a quote against assumptions, and the price moves when the assumptions change. Sending the complete pack once is faster than three rounds of clarification.
What comes back
A price, a lead time, and a short list of cost drivers with the changes that would remove them — a corner radius opened up, a tolerance relaxed, a pocket made through instead of blind, a datum moved to a face that is already machined. That review is free and it happens before you commit, which is the point at which design changes are still cheap.