CNC Machining Design Guidelines
A part can look perfect in CAD and still be slow, expensive or risky to machine. These are the design rules our engineers recommend most often, and each one is cheap to apply before production starts.
CNC machines remove material with rotating cutting tools, so the shape of the tool, its length and the way the part is clamped all limit what can be made. At RpProto we review CAD files for CNC machining every day, and the same small design issues come up again and again. Following the guidelines below gives you better accuracy, shorter lead times and a lower part cost.
1 Check part size against the machine envelope
Check the envelope early for large parts
Every CNC machine has a limited work envelope, which is the maximum size of part it can hold and cut. 3-axis mills generally offer a larger working area than multi-axis machines, so very large parts with many angled features can be harder to plan.
Tip: If your part is large, tell us early. Splitting it into two sections that are assembled afterwards is sometimes cheaper than machining it in one piece.
2 Keep features on as few faces as possible
Fewer setups = lower cost
Each time a part must be unclamped, flipped and re-aligned, you pay for extra setup time and extra chances for small positioning errors. A part with holes, pockets and slots on just one or two faces is much cheaper than one with features on all six sides.
Tip: Align holes and pockets in the same direction wherever the function allows. If angled features are unavoidable, 5-axis machining can reach them in a single setup, though the machine time is more expensive.
3 Design internal corners with a radius
Internal radius ≥ 1/3 of cavity depth
A rotating cutter is round, so it cannot cut a perfectly sharp inside corner. Every internal corner will have a radius, and the smallest possible radius is set by the tool diameter.
- Make internal fillets as large as your design allows. A bigger radius lets us use a bigger, stiffer tool, which cuts faster and gives a better finish.
- Use the same radius for all internal corners where possible. One tool can then cut them all without changing.
- Make the radius slightly larger than the tool radius. This lets the tool move smoothly around the corner instead of stopping and leaving marks.
If your design truly needs a sharp inside corner, for example to fit a square mating part, add a small relief cut (a “dog-bone” notch) in the corner, or let us know and we will suggest an alternative.
4 Keep wall thickness sensible
Metal ≥ 0.8 mm | Plastic ≥ 1.5 mm
Thin walls vibrate and bend under cutting forces. This causes poor surface finish, dimensional errors and sometimes broken walls. Plastics are softer and can flex or warp, so they need thicker walls than metals.
Keep tall thin walls in proportion as well. As a rule of thumb, wall height should not exceed about 10 times its thickness.
Tip: If you need a thin wall for weight reduction, add ribs or increase the thickness near the base to stabilize it.
5 Limit cavity depth
Depth ≤ 4 × width
Deep, narrow pockets need long cutting tools. Long tools bend and vibrate (chatter), which hurts accuracy and surface quality. If a deeper pocket is essential, make it wider, or use a stepped profile so that shorter tools can reach the bottom.
6 Choose standard hole and thread sizes
Hole depth ≤ 10 × diameter
Holes that match standard drill bit sizes are fast and inexpensive to produce. Non-standard diameters must be cut with an end mill, which takes longer.
- Use standard metric or imperial diameters wherever possible.
- Deeper holes are possible with special drills, but they add cost.
- For threads, standard sizes are best. In most cases a thread length of about 2 to 3 times the diameter provides full strength, so extra thread depth rarely adds value.
- A drilled blind hole ends in a cone shape. A flat bottom requires an end mill, so only specify one if the design really needs it.
7 Handle undercuts carefully
T-slots about 3–40 mm wide | Dovetails at 45° or 60°
Undercuts are features that standard tools cannot reach from above, such as grooves inside a bore or T-slots. They need special tools and extra setup. Dovetail undercuts work best at standard angles, because matching cutters are readily available.
Where possible, redesign the feature so it can be cut from the open side. Otherwise, using standard slot widths and angles keeps costs down.
8 Add text and logos the smart way
Engrave rather than emboss
Engraved text is quicker and cheaper than embossed text, because embossing means removing all the material around the letters. Choose a simple, clean sans-serif font, and avoid very thin strokes or tiny sizes. Fine decorative lettering can be hard to cut cleanly, especially in harder metals. If your logo is small or detailed, send us the file first and we will confirm the minimum size we can machine.
9 Specify tolerances only where they matter
Tight tolerances on critical features only
Tolerances are one of the biggest cost drivers in CNC machining. Tighter tolerances mean slower cutting, more inspection and a higher chance of scrap.
- Apply tight tolerances only to critical features, such as bearing seats, press fits or sealing surfaces.
- Leave non-critical dimensions on the general tolerance. See our CNC machining tolerances.
- Add a drawing with critical dimensions marked. Without one, we machine to the standard general tolerance.
A good habit is to ask of each tolerance, “What function does this protect?” If you cannot answer, the tolerance can probably be relaxed.
10 Pick a material that machines well
Machinability shapes what you can design
Material choice affects what you can design. Aluminum 6061 cuts quickly and cleanly and holds tolerances well, so it supports thinner walls and finer features at lower cost. Harder materials such as stainless steel or titanium cut more slowly and wear tools faster, which often means larger radii, more generous wall thickness and higher cost. Plastics like POM and ABS machine easily, but they can flex and expand with temperature, so they need thicker walls and more realistic tolerances.
If you are unsure which material is best, tell us how the part will be used and we will recommend options.
11 Share your files for a DfM review early
Send STEP + 2D drawing
The cheapest time to change a design is before it is machined. Send your 3D model (STEP is ideal) and a 2D drawing marking critical dimensions, threads and surface finish. Our engineers will flag problems and suggest practical changes.
Quick reference table
| Feature | Recommended guideline |
|---|---|
| Internal corner radius | Larger is better; ≥ 1/3 of cavity depth |
| Minimum wall thickness | Metal ≥ 0.8 mm; plastic ≥ 1.5 mm |
| Cavity depth | ≤ 4× cavity width |
| Hole depth | ≤ 10× hole diameter |
| Thread length | About 2–3× diameter |
| T-slot width | About 3–40 mm |
| Dovetail angle | 45° or 60° |
| Text | Engrave rather than emboss; simple sans-serif font |
Design checklist before you send your files
- Are all internal corners rounded, and consistent where possible?
- Are walls thick enough for the material?
- Are pockets and holes within the depth ratios above?
- Do hole and thread sizes match standard tools?
- Are features aligned to minimize setups?
- Are tight tolerances limited to critical features?
- Did you include a drawing for threads, tolerances and surface finish?
Work with RpProto
We machine prototypes and production parts in aluminum, steel, stainless steel, brass, titanium and engineering plastics. Upload your CAD file and our engineers will review it, flag any risks and suggest improvements.
Request a quote