Engineering · DFM
DFM best practices for CNC machining.
The design rules specific to CNC milling and turning. Tool reach limits, pocket geometry, drill standards, thread depth recommendations, and where designers most commonly spec features that don’t need to be that hard.
01 · Pockets & corners
A pocket is a tool radius — plus everything else.
The single most common DFM issue we flag: square internal corners. Every endmill leaves a radius equal to its own radius. Specifying a true square corner forces a Wire EDM follow-op or an absurdly small endmill. Either drives cost up by 2–4×.
The fix is almost free: specify an internal corner radius. Even a generous radius (R 1–2× tool diameter) costs nothing — and lets us run a stiffer tool faster.
Internal corners
Specify R ≥ 0.060″ (1.5 mm)
Lets us run a 2 mm or larger endmill — standard tool, normal feeds. Tighter radii get exponentially more expensive.
Floor radii
Use bullnose tools
A small floor radius (R 0.030–0.060″) is essentially free with a bullnose endmill. Sharp floor edges require a thinner tool path or a follow-op.
Pocket depth
Depth ≤ 4× tool diameter
Standard endmill reach is roughly 4× the cutter diameter. Deeper pockets need extended-reach tools (slower, less rigid) or step-pocket designs.
02 · Tool reach
Deeper isn’t free.
A standard endmill reaches roughly 4× its diameter. Beyond that, deflection makes the tool walk and the surface chatter. Extended-reach tools exist — but they’re less rigid, slower, and more expensive.
Rule of thumb
A pocket 0.5″ deep should have walls and corners that allow at least a 0.125″ diameter endmill (4:1 reach). For a 1″ deep pocket, plan around a 0.250″ diameter tool minimum.
When you can’t avoid deep + small
We can run extended-reach carbide, ceramic-coated, or even Wire EDM as a follow-op. Talk to us early — geometry that looks innocent on a CAD model can require serious tool gymnastics.
03 · Holes
Standard sizes are essentially free.
Standard drill sizes (fractional, number, letter, metric standard) come off the rack. Non-standard sizes require a reamer, custom drill, or a milled hole — each adds setup time, tooling cost, and inspection complexity. For non-critical holes, snap to the nearest standard size and save real money.
| Series | Range | Common usage | Tolerance class |
|---|---|---|---|
| Number drills | #80 → #1 | Small holes (0.0135″ – 0.228″) | ±0.003″ |
| Letter drills | A → Z | Medium-small (0.234″ – 0.413″) | ±0.003″ |
| Fractional | 1/64″ → 1″+ | General use, 64ths | ±0.003″ – ±0.005″ |
| Metric | 0.5 mm → 25 mm | Increments of 0.5 or 0.1 mm | ±0.05 mm |
| Reamed | matched bore | Tight diameter & finish (e.g. for press-fit pins) | ±0.0005″ |
| Bored / interpolated | any size | Mill bores any custom diameter | ±0.001″ – ±0.0002″ |
Through > blind
Through holes are easier to chip-clear and inspect. Make a hole through the part if there's no functional reason for blind.
L:D ≤ 5
Standard drilling. Beyond 5:1, switch to peck cycles, gun drilling, or split the hole from both sides.
Cross-holes need flats
A drill on a curved surface walks. If you must cross-drill into a round, add a milled flat or counterbore at the entry.
04 · Threads
Tap depth: 1.5× diameter is enough.
More than ~1.5× diameter of engaged thread doesn’t add strength — the bolt fails before the threads strip. Spec’ing 3× full-depth threads in a blind hole just creates chip-clearance problems and risks tap breakage.
Drill depth ≥ tap depth + 1× diameter
Plain taps need clearance below the threads — for chips and to bottom out the tap. Spiral-flute / form taps reduce this requirement but don’t eliminate it.
Avoid bottoming taps unless required
Standard taps leave 2–3 incomplete threads at the bottom. If full thread to the floor is essential, call out a bottoming tap explicitly — it costs more.
Tap drill diameter matters
Don’t spec the major thread diameter as the hole — call out the minor (tap drill) diameter, or just leave it to us with the thread callout. Saves a step and prevents misreads.
Standard pitches first
UNC and metric coarse cover most needs. Specify UNF or metric fine only when shock load, vibration, or thin walls actually require it.
05 · Turning
Round parts have their own rules.
CNC turning is the cheapest way to make rotationally symmetric parts — but the design rules are different than milling. The big ones below.
L:D limits for slender parts
Length-to-diameter > 8:1 starts deflecting under cutting load. Use a tailstock, follow rest, or step up to Swiss-type (we run Tsugami) for very slender parts.
Tool radius leaves a fillet
Just like milling, the OD profile inherits a small radius wherever the tool meets a shoulder. Spec a sharp shoulder only when functional — and expect a follow-op to get there.
Internal vs external threads
External threads are easy and fast. Internal threads in small bores need careful tool selection and are slower. For tiny IDs, consider using a thread insert.
Knurling for grip features
Standard diamond and straight knurls can be applied during turning at minimal cost. Calling out a custom knurl adds a separate operation.
Bar pull-through and chuck clearance
If the part is bar-fed, the diameter must fit through the spindle bore. For chucked work, design at least 0.25″ (6.4 mm) of grip flange beyond the longest feature.
Live tooling combines ops
Modern lathes can drill, mill flats, mill cross-features, and tap in the same setup. Tell us early — we can often eliminate a whole second setup.
06 · Setup & datums
Each setup is real money.
Every time we re-fixture the part, two things happen: the clock runs (setup time + program load), and tolerance stack-up grows. A part designed to be machined in one setup is dramatically cheaper than the same part needing four.
Datum from a held face
If the drawing’s primary datum is on a feature we can’t hold (e.g. the inside of a pocket), we have to add a separate inspection setup. Pick a datum we can clamp to.
Group tight tolerances per setup
Two features held to ±0.001″ in one setup: easy. Same two features across separate setups: tolerance has to stack up against fixturing repeatability — much harder.
Symmetry kills setups
Mirror-symmetric features that look identical from front and back let us run them as a single program. Cosmetic asymmetry that's not functional often doubles cost.
Standard fixturing first
Vises, soft jaws, and machine-table fixtures are all common. A part designed around a standard 6″ machine vise is almost always cheaper than one needing a custom fixture.
Avoid 5-side requirements
If you need machining on all 6 sides, you've added at least 2 setups. If 4 of 6 is enough functionally, design that way.
Talk early on aerospace work
First-article inspection (FAI) per AS9102 adds setup overhead. Drawings designed around FAI requirements upfront save real time vs. retrofitting.
07 · Cosmetic
Tool marks aren’t defects — unless you say they are.
Standard CNC milling leaves visible tool marks. They’re directional, controllable, and routinely acceptable in functional applications. If a surface has cosmetic requirements, call them out explicitly — directional finish, no scratches, hand-finish, anodized matte, etc. Don’t leave it to interpretation.
For visual surfaces
- ·Specify finish direction (e.g. "linear, parallel to long axis")
- ·Call out Ra value (16 µin or below for cosmetic)
- ·Note any anodize / coat that follows
- ·Identify "show face" vs hidden faces
For functional surfaces
- ·Standard 63–125 µin Ra is almost always fine
- ·Direction usually doesn’t matter
- ·"As-machined" finish is the cheapest option
- ·Sharp burrs need a deburr op — call out edge condition explicitly
Up next
Wire EDM has its own DFM rules.
Wire EDM does the things milling can’t — sharp internal corners, hardened materials, high-aspect features. The full DFM reference for EDM is the next stop.
Send a STEP file for free DFM review.
We'll mark it up with the kind of suggestions on this page — and quantify the cost-reduction opportunities — usually back to you within one business day.
Quotes in 24 hours