DFM for CNC Machining: Design Rules for Lower Part Cost

DFM for CNC machining is the set of geometry and drawing decisions that decide how many setups a part needs, which tools can reach its features, and how tight its tolerances must be. The headline numbers: a standard commercial part holds ±0.13mm (±0.005in) on linear dimensions without effort, while calling ±0.025mm (±0.001in) on every feature adds 20 to 50 percent and ±0.013mm (±0.0005in) can double the cost. Walls under 1.5mm deflect under cutting force, a round tool cannot cut an inside corner sharper than its own radius, and a drilled hole past 4 diameters deep starts to wander. Each limit is a design decision made before the file is sent, not a shop problem solved after.

This page carries the process-specific rules for CNC. The general principles shared with sheet metal and additive are covered on the design for manufacturing page. Here the focus is CNC depth: setup and orientation thinking, corner, wall, hole, and pocket rules with numbers, what tolerances cost, how material choice shifts every rule, and a worked example that takes a bracket from three setups to one.

What DFM changes on a machined part

Setups, tool reach, and tolerance drive the price

A machined part is priced from three things before anyone looks at material. First, setups: every flip, rotation, or fixture change stops the machine while an operator re-clamps and re-indicates datums, so a part that machines complete in one vise grip is nearly always the cheapest version of itself. Second, tool reach: a rotating cutter is a cylinder, so it cannot produce sharp internal corners, reach under overhangs in a 3-axis setup, or mill a corner tighter than the tool itself. Third, tolerance: precision is paid per feature, through slower feeds, finer tooling, and added inspection, so a blanket tight band taxes the whole part for the sake of a few functional features.

Walk the design against those three costs in order. Count the setups the geometry forces, check every feature against the tool reach limits, and only then set tolerances feature by feature, with the general class carrying everything that is not functional. A short CAD review at this stage removes the re-quotes and the DFM feedback loop.

Orientation is the cheapest win

Ask one question early: can every machined feature be reached from a single clamp orientation? If yes, the part needs one program, one setup, and one datum set that inspection reuses. If no, each extra orientation brings its own clamp marks, its own re-indicating time, and a fresh chance to stack error into the part.

Orientation also decides workholding. A rectangular part grips in a plain vise, the fastest holding there is. Parts with no parallel faces need soft jaws or a fixture plate, both of which add setup cost, and thin or tall parts clamp poorly because vise pressure bows a thin plate while cutting force pushes a tall wall.

The file package a shop can quote from

Send a STEP file for the 3D geometry plus a 2D drawing for everything the model cannot say: critical dimensions with their tolerances, thread callouts with standard, size, class of fit, and depth, surface finish notes, and the datum scheme the machinist will clamp to. Threads in a model are cosmetic cylinders unless the drawing specifies them.

State units, material, and the general class

Three fields prevent the most expensive quoting failures. State the units in the file, the title block, and the filename, because a millimeter-versus-inch mix-up scales the part by 25.4 times. State the material with temper, 6061-T6 rather than bare aluminum. Declare the general tolerance class in the title block, for example ISO 2768-mK, so every untoleranced dimension has a defined band instead of an argument. The CAD file formats page covers the format detail, and GD&T follows ASME Y14.5 or the ISO 1101 series.

Design rules with numbers

These are the CNC geometry limits stated as design targets. Check every feature against them before sending a file.

Inside corners and pocket radii

A milling cutter is round, so every internal corner it produces carries a fillet at least as large as the tool radius. The floor is 0.2 to 0.5mm with small precision tooling, and standard practice sizes pocket corners to a 0.8mm radius endmill, tightening to 0.5mm only where the design forces it. A sharp 90 degree internal corner is not a milled feature: it needs EDM or a redesign that adds a radius.

Larger radii are cheaper, not sloppier. A 2mm corner accepts a stiffer endmill that removes material faster, while a 0.5mm corner forces a 1mm tool that must run slow and shallow to survive. In deep pockets the radius becomes structural, because tight corners there mean a long, thin tool that chatters.

Wall thickness and deep pockets

Set structural walls at 1.5mm or thicker. Walls under 1.5mm deflect under cutting force, which hurts both accuracy and finish, and the shop recovers with light finishing passes, special fixturing, or both. The 0.5 to 1.0mm band is viable only for small non-critical details, an emblem edge or a shallow rib. Per-process wall and feature floors across every process sit on the minimum wall and feature sizes page.

Deep pockets are the common trap because they create thin walls as a side effect: a pocket milled between two thin walls leaves them unsupported for the full depth, and cutting force on one face pushes each wall while the tool finishes the other. Give deep pockets generous internal radii and size walls up from the 1.5mm rule in proportion to their height. Chamfers follow the same logic at small scale: 0.5 to 1.0mm is standard, 0.2 to 0.5mm is the precision end, and below about 0.2mm the feature needs special tooling for no functional gain.

Holes, depth ratios, and threads

Drilled holes behave when they respect one ratio: depth to diameter at 4:1 or less. Past that a standard twist drill loses straightness and size, and chips pack the flutes. Gun drilling reaches 10:1 for true deep holes, at a cost adder of 50 to 100 percent. Blind holes need at least 2 diameters of depth for the drill tip geometry, and through holes are preferred wherever the design allows, because chips and tap lead exit freely.

Threads carry their own rules, treated in full on the drilling, tapping, and threading page. The DFM-relevant parts: standardize on common UNC, UNF, and metric sizes, end blind threads well short of the hole bottom so the tap has chip space, and treat tapered threads as a 30 to 50 percent adder over straight threads, specified only where a seal demands it. Put the thread standard, size, class of fit, and depth on the drawing, per the thread standards reference.

Undercuts and features a 3-axis setup cannot reach

An undercut is any surface the tool cannot reach cutting straight down the spindle axis. A 3-axis setup cannot machine one, so the part moves to 4-axis or 5-axis equipment, which adds roughly 200 to 500 percent over 3-axis machining, or it takes a special tool run slow. Internal keyways add 20 to 40 percent through broaching. Undercuts, keyways, and sharp internal corners are the three geometry classes that push parts onto more expensive equipment, and redesigning around them is usually cheaper: open a slot to the surface, or convert the feature to one a straight tool reaches.

Workholding and the shape of the blank

Design the part for the vise it will sit in. A blank with two parallel faces grips in a plain vise, and parts without parallel faces need soft jaws or a fixture, which adds a setup before cutting starts. For thin parts, plan the clamping direction so vise pressure does not bow a finished surface, and use tabs or extra stock at the clamp points that stay as-cut or machine away last. Stock size is a DFM decision too: a blank thick enough that one face can ship sawn and non-critical removes a facing operation, as the worked example shows.

Material choice shifts every rule

Machinability sets feeds, speeds, tool life, and the tolerance a feature can hold. Aluminum 6061 is the default: it machines freely, holds about ±0.025mm (±0.001in), and its one quirk, buildup on the tool edge, is handled with polished carbide tooling and flood coolant. Carbon steel 1018 machines at about 70 percent of free-machining brass and holds the same band, and brass C360 is the 100 percent machinability benchmark.

Stainless 304 and 316 run near 45 percent of that benchmark speed, hold about ±0.05mm (±0.002in), and work-harden under dull or slow tooling, so they demand sharp tools, low speeds, and positive rake geometry. Titanium Ti-6Al-4V conducts heat poorly, so heat concentrates at the tool edge, and it needs carbide tooling, low speed, heavy feed, and flood coolant to hold about the same ±0.05mm. The DFM consequence: the same geometry costs more and holds looser in stainless or titanium than in aluminum or steel, so tight features in those alloys deserve a second look. Alloy ratings are covered on the material machinability page.

Tolerances and what precision costs

General defaults before specific callouts

Let the general class do most of the work. For machined metals, ISO 2768-1 fine class gives ±0.05mm for sizes from 0.5 to 3mm and 3 to 6mm, ±0.10mm for 6 to 30mm, and ±0.15mm for 30 to 120mm, with medium class roughly double those values as the general default. ISO 2768-2 grade K adds about 0.05mm flatness on short features and 0.2mm circular run-out, and angular features hold ±1 degree at the standard level. Declaring the class in the title block governs every untoleranced dimension at once, and it prices as routine work, because it is.

Then tolerance the exceptions. A mating bore, a locating hole pattern, or a sealing face gets an explicit value sized to what the material and feature can hold: hole position reaches ±0.08mm as standard practice and ±0.025mm at the precision end, and GD&T flatness and parallelism typically run 0.001 to 0.005 inch (about 0.025 to 0.13mm), specified per ASME Y14.5 so inspection is repeatable. The machining tolerances guide covers the standards in full.

The cost ladder

Every rung below is a real cost adder observed in commercial machining, and most parts that quote high carry two or three of them at once. Read it as a list of things to remove, not a menu to order from. The pattern in every row is the same: tighter bands, deeper holes, and extra operations each add machine time, tooling, or inspection somewhere in the job. The steepest rungs are the multi-axis and deep-hole rows, which is why orientation thinking and hole depth limits come first in any DFM pass.

Pre-send checklist

Run this list against the model and drawing before requesting a quote. It takes minutes and catches the issues that otherwise surface as a re-quote or a DFM email.

• Every machined feature is reachable from one clamp orientation, or the extra setups are a deliberate, costed choice.
• Inside corner radii are at least 0.8mm, or 0.5mm at the precision floor, and larger where pockets are deep.
• Structural walls are 1.5mm or thicker; nothing functional sits in the 0.5 to 1.0mm band.
• Drilled holes stay within 4:1 depth to diameter, blind holes are at least 2 diameters deep, and through holes are used where possible.
• Threads are standard sizes, blind threads end short of the hole bottom, and thread standard, class, and depth are on the drawing.
• No undercuts, internal keyways, or sharp internal corners unless the design cannot work without them.
• Tolerances: general class declared in the title block, explicit values only on functional features, GD&T on datums and mating interfaces.
• Material with temper stated, units in the file, filename, and title block, stock size chosen so a non-critical face can ship as-cut.

Worked example: a bracket from three setups to one

A sensor mounting bracket in 6061-T6 aluminum, 90 by 60 by 20mm, shows the chain end to end. The first version has a shallow pocket and two counterbored mounting holes on the top, three M4 tapped holes in the bottom face, and two 6mm cross-holes through the side walls. That geometry forces three setups: top work in a vise, a flip for the bottom taps, then soft jaws standing the part on edge for the cross-holes. Every flip adds handling and re-indicating, the cross-holes stack datum error across setups, and the soft jaws are a fixture cost unique to this part.

The redesign targets one orientation. The M4 tapped holes become 6mm clearance holes drilled from the top, a 3.3:1 depth ratio against the 20mm thickness that sits inside the 4:1 limit, counterbored for the fastener heads so the bracket now bolts through into the base it mounts on. The 6mm cross-holes move to the top face as blind holes 14mm deep, a 2.3:1 ratio that clears the 2-diameter floor and stays inside the 4:1 limit while doing the same locating job from above. The pocket corners open from 0.5mm to 2mm so a stiffer endmill finishes them in fewer passes, and the bottom face is declared non-critical at the general class and ships as the sawn stock face, which removes the flip entirely.

The result machines in one vise grip from sawn bar stock: one program, one datum set measured the same way inspection will check it, no soft jaws, no re-indicating. Both brackets do the same job, and the one-setup version is cheaper at any quantity this bracket is likely to run, because the work moved off the machine and into an hour of CAD.