Designing for CNC Common mistakes that cost time & money — and how to avoid them
CNC routing is capable and cost-effective, but it runs on a specific set of rules that CAD software quietly ignores. Miss them and you’re absorbing rework costs and wasted material. Get them right and parts come out correct the first time, at the price you quoted.
Tolerances that are too tight, or inconsistently applied across a part, are reliably expensive. For wood, MDF, acrylic, and plastics, standard CNC routing tolerances sit around ±0.2–0.5 mm. Aluminium can hold ±0.1 mm — but achieving that means slower feeds, more tool changes, and the cost adds up fast.
The Mistake
- ±0.05 mm called out uniformly across an entire part
- Only one or two features actually need that precision
- Fabricator charges for tight-tolerance setup across every dimension
- Machining time and cost increase with no functional benefit
The Fix
- Identify functionally critical features: mating faces, press-fit holes, alignment pins
- Specify tight tolerances there only — let everything else sit at ±0.3 mm
- This single change can cut machining time by 20–30% on complex parts
- Call out tolerances explicitly in the drawing, not just the file
A CNC router uses a spinning cylindrical tool. Physics prevents it from cutting a perfectly sharp internal corner — it will always leave a radius equal to half the tool diameter. Design a square internal pocket for a mortise joint, press-fit bracket, or inlay without accounting for this, and the parts won’t go together.
A small circular relief at each corner, diameter matched to the tool. Functional and straightforward to machine — slightly visible on the finished part.
Similar principle to dogbone but positioned along one edge. Less noticeable in assembled work where appearance matters.
For aesthetic parts, an undercut hides the relief while maintaining fit. Requires a discussion with your machinist before the design is locked.
Which approach suits your part depends on whether the corner is structural, concealed, or on show. Raise it with your fabricator before committing to the design — it’s a short conversation that prevents a full remake.
CNC routing involves real physical forces. A spinning bit moving through timber or acrylic creates lateral loads, vibration, and heat. Thin walls and small protruding features that look fine in a render are sometimes the first thing to snap, deflect, or tear out.
Sheet Materials
- MDF / Plywood — min wall 3 mm, min feature 4 mm
- Acrylic — min wall 3 mm, min feature 5 mm
- HDPE / Delrin — min wall 2 mm, min feature 3 mm
- These shift with feature height and fixturing
Metals
- Aluminium — min wall 1.5 mm, min feature 3 mm
- Tall thin walls amplify vibration — add gussets or fillets at the base
- Material switch (acrylic → Delrin) often gives rigidity without redesigning
- If below these numbers, talk to your fabricator before the job runs
The material determines machinability, surface finish, edge quality, structural performance, and what post-processing is even possible. These mismatches come up regularly.
Machines beautifully, but swells and falls apart with moisture. Use exterior-grade plywood or HDPE for anything exposed.
Cast machines better, holds tighter tolerances, and is less prone to stress cracking. Extruded is cheaper but problematic for precision parts.
6061 is the default for structural CNC parts. 5052 is suited to forming. Using 5052 for machined features produces poorer surface finish and faster tool wear.
Hardwoods with interlocked grain — some NZ native species among them — can tear out along edges. Consider grain direction relative to toolpath early.
A well-designed part can still cause delays if the files aren’t set up properly for CNC. These are the most common problems we see on incoming jobs.
Toolpaths need closed geometry. Open paths produce errors or unexpected cuts. Close all vectors before sending.
Stacked geometry sends the tool over the same path twice, adding time and risking overheating. Strip duplicates as part of your pre-submission check.
Always specify material thickness in the drawing notes — not just in the file. Where thickness affects fit, it’s critical information.
When a fabricator is running multiple jobs simultaneously, ambiguity turns into mistakes. Include material and spec in the filename or a callout sheet.
Files at 1:10 or sent in the wrong unit (mm vs inches) are more common than most designers expect. Confirm units and include a known reference dimension.
Run through this before sending any CNC job. None of these items takes more than a few minutes — all of them are considerably cheaper to fix before the part is cut.
Geometry
- Internal corners have dogbone, T-bone, or undercut fillets
- Wall thickness and feature widths checked against material minimums
- DXF/DWG vectors closed and duplicates removed
- File units confirmed — mm preferred
Drawing & Notes
- Critical tolerances called out; non-critical dimensions relaxed
- Material specified and appropriate for the application
- Material thickness called out in drawing notes
- Post-processing requirements noted (painting, anodising, tapping)
None of the mistakes covered here are difficult to fix — they just require knowing what to look for before the file leaves your desk. GeoSaffer’s team in Auckland includes DFM review as part of the quoting process. Ten minutes looking at your file upfront is worth considerably more than dealing with a remake later.
Get a quote or send your file for review →