DFM Checklist: 25 Design Rules for CNC Machined Parts

Most CNC parts are expensive for design reasons, not machining reasons. A part that costs $48 to machine and one that costs $12 can have identical function — the difference is a handful of decisions made at the CAD stage. This is the DFM checklist we run through before quoting, and it is worth reading before you finalise any drawing.

The 25 Rules

Geometry and Features

1. Design internal corners to a standard tool radius. A corner sharper than the end mill that cuts it means EDM or hand finishing. Use R2, R3 or R4 — standard cutter radii — and say so.
2. Keep pocket depth under 4× the tool diameter where you can. Deeper pockets force long, slender tools that must run slowly.
3. Avoid pockets narrower than 2× the tool diameter. Below that, the tool deflects and finish suffers.
4. Do not specify a floor radius smaller than the corner radius. The tool has one radius; geometry that demands two means two operations.
5. Eliminate undercuts, or design them for 5-axis access. Undercuts needing special tooling are the second most common cost driver.
6. Keep walls above 0.8 mm for metal, 1.5 mm for plastic. Below that, chatter and distortion take over.
7. Add chamfers or fillets to all external edges. A 0.5 mm chamfer removes a manual deburring operation and is free to specify.
8. Avoid text and logos on vertical faces where possible. Engraving on a machined wall requires a separate small tool and a second pass; text on a flat face is cheap.
9. Engrave at 0.3 mm deep minimum, with a stroke width of at least 0.4 mm. Finer strokes clog and disappear.
10. Keep threaded holes to standard sizes. M3, M4, M5, M6, M8 and their UNC/UNF equivalents have tooling on the shelf.

Tolerance and Specification

11. Use the loosest tolerance that works. General tolerance of ±0.1 mm costs far less than a drawing peppered with ±0.02 mm.
12. Apply tight tolerance only to the features that need it — bearing bores, mating faces, seal grooves.
13. Do not dimension the same feature twice. Redundant dimensions create inspection disputes.
14. Use GD&T where datum control matters, not everywhere. Every extra datum and position callout adds inspection time. See our GD&T guide.
15. Specify surface finish only where needed, with a blanket note for the rest. "Ra 0.8 all over" is the most expensive two words in machining.
16. State the temper, condition and grade, not just the material name. "Aluminium" is not a specification.
17. Reference a standard for anything you have not drawn explicitly.
18. Allow for finishing processes. Anodising adds roughly 0.005–0.025 mm per surface and can close a tight bore; masking costs extra. Check our surface treatment notes.

Setup, Fixturing and Volume

19. Design in a way the part can be held. A part with no flat face and no clamping area needs a custom fixture that you pay for.
20. Minimise the number of faces that must be machined. Every new orientation is a new setup; three setups is where cost starts climbing steeply.
21. Machine from one side where possible. Multi-sided work needs re-fixturing and re-datuming, with tolerance stack-up risk.
22. Make parts in a batch. Setup cost is fixed; 100 pieces amortise it 100 times better than one.
23. Use standard stock sizes. A part sized to 62 mm when 60 mm bar is standard pays for the extra material plus the extra cutting.
24. Standardise across your product family. Same hole sizes, same corner radii, same fasteners — this lets a shop run family tooling and combined setups.
25. Send the 3D model, not just the PDF. A STEP or X_T file lets the CAM programmer work directly and reduces misinterpretation and re-quotes.

What DFM Saves in Practice

On a typical bracket, moving from a fully toleranced drawing to a DFM-reviewed one drops cycle time by 20–40% with no functional change. On aluminium enclosures, the biggest single saving is usually eliminating a fifth-axis setup by redesigning an undercut. On turned parts, it is often just switching from a special thread to a standard one.

The economics are worth stating plainly: a $60 engineering hour spent reviewing the design against this checklist routinely saves hundreds of dollars in production. That is why we do this review free on every RFQ rather than quoting the drawing as drawn.

Cost Drivers Ranked

Driver	Typical impact	How to reduce
Tolerance tighter than ±0.05 mm	High	Loosen what does not need it
Extra setups / orientations	High	Redesign to machine from fewer sides
Tiny internal radii, deep pockets	High	Use standard tool radii, reduce depth ratio
Surface finish below Ra 0.8 µm	Medium–high	Specify only critical faces
Exotic material	Medium–high	Confirm the alloy is genuinely required
Batch size of one	Medium	Order quantity, not single pieces
Custom fixturing	Medium	Add a clamping feature to the design
Hand deburring and finishing	Low–medium	Specify chamfers

How Renjiu Applies DFM

Every RFQ that reaches us gets a DFM review before the quote goes out: we flag tight tolerances that will not affect function, pockets that will force slow tooling, undercuts that will cost a setup, and finishes that will not survive the anodising you also specified. You get the flags, the reason, and the alternative — then you decide. Send models through our RFQ form, and pair this checklist with our RFQ checklist and the breakdown of what drives machined part price for the full picture.