DFM for CNC Machining: The Rules That Actually Reduce Unit Cost

A part designed in CAD without manufacturing input looks clean on screen: sharp internal corners, a 0.8 mm wall, a 3 mm wide slot 25 mm deep, and a cosmetic surface on all six faces. Every one of those features is legal geometry. Together they turn a two-hour part into a six-hour part, and the quote reflects it before anyone explains why.

DFM is not a list of restrictions to argue about. It is the set of decisions that determine which cutter the machine can use, how fast it can move, how often the part must be re-fixtured, and how likely a thin wall is to sing and scrap the part.

The rule behind every rule

A rotating cutting tool has a diameter, a length and a stiffness. Everything else follows.

The diameter sets the smallest internal radius and the narrowest slot. The length sets how deep the tool can reach before it deflects, and stiffness falls with the cube of that length. The stiffness sets how much material can be removed per pass before chatter, which shows up as poor finish, poor tolerance and sometimes a broken tool inside your part.

When a feature forces a small, long tool, the machine slows down. A cutter at 4:1 length-to-diameter may run at a third of the feed rate of the same cutter at 2:1.

Internal radii and pocket depth

This is the largest cost lever on most parts, and it costs nothing to change.

Standardize on the cutters your supplier stocks. A shop running 6, 8, 10, 12 and 16 mm cutters will cut a 3 mm corner radius with a 6 mm tool, which is the smallest that is still efficient. A 1 mm radius forces a 2 mm cutter that cannot reach 20 mm deep without breaking.

A large radius changes the part, though. If a corner must be small for function, keep it small and accept the cost knowingly. If it is small only because nobody changed the CAD default, change the default.

Walls, floors and thin features

Thin walls are where parts are lost, not just slowed down. A wall below about 1 mm in aluminum deflects under cutting force, springs back after the tool passes, and ends up thinner in the middle than at the top.

Aspect ratio matters more than absolute thickness. A wall is comfortable to about 10:1 height-to-thickness, difficult from 10:1 to 20:1, and needs support or redesign beyond that. A 0.8 mm wall 8 mm tall is fine; the same wall 30 mm tall will move.

If a thin wall is functionally necessary, say so in the RFQ. The shop will plan around it with a support rib removed at the end, a light finishing strategy, or a stress relief before the final pass. That planning costs less than discovering the problem on the third part.

Holes, threads and small features

Drilling is fast until it is not. A hole up to about 4× its diameter is a standard peck-drilled hole; beyond that, chip evacuation and drill wander take over.

• Hole depth: 4:1 standard, 6:1 with care, 10:1 needs gun drilling.
• Hole diameter: below 1.5 mm, breakage risk rises and feeds drop.
• Hole entry: on a curved or angled surface, add a spot face, or the drill will deflect.
• Threads: M3 and above is routine; M2 works but is slow; below M1.6 expect special pricing and higher scrap.
• Thread depth: 1.5× diameter engagement in steel, 2× in aluminum, and no deeper than about 2.5× diameter in a blind hole so the tap has somewhere to go.
• Threads in thin walls: leave at least one full thread diameter of material around the hole.

Where a thread is only needed for occasional disassembly, a through-hole with a nut or a thread insert is often cheaper than a deep tapped hole in a difficult material. Thread milling suits titanium and hardened steel because it cuts a clean thread without a tap that can snap.

Undercuts, tolerances and text

Every setup carries fixed cost: workholding, work offset, proving the first part, and a datum transfer that adds error. Features that force extra setups include undercuts and internal grooves on turned parts, cross holes at an angle, and anything on the back face that cannot be reached from the front. If a back-side feature is unavoidable, add a flat that gives the vice something to hold and put a datum on it.

Tolerance follows a simple rule: tolerance only what functions. A drawing with ±0.05 mm general and three dimensions at ±0.01 mm is cheaper than the same part at ±0.02 mm everywhere and performs identically. Finish behaves the same way: Ra 3.2 µm is normal as-machined and costs nothing extra, Ra 0.8 µm needs a finishing pass with a smaller stepover, and Ra 0.4 µm usually means a separate polish or lap.

Engraved marking has its own minimums: character height around 3 mm so it survives anodizing, depth 0.2 to 0.3 mm, stroke width at least 0.4 mm. Fine detail in a logo will not survive coating.

What to fix first

If you change only three things, change these, in order: open the internal corner radii to at least one third of the pocket depth; reduce the number of setups by moving features onto accessible faces; and relax every tolerance that is not functionally required. Those three typically remove 15% to 30% of the unit price. Cosmetic changes, alloy substitution and stock-size optimization come after.

When we return a quote at JSHS, the DFM note names the features driving cost and prices each alternative, so you can decide with numbers rather than opinions. Send a drawing and ask for the DFM version alongside the as-drawn price.

Frequently asked questions

Does DFM change the part's function?

It should not. A good change preserves function and reduces cost. Where a change would affect function, such as enlarging a corner radius that carries a seal, the decision belongs to the designer, and the supplier should present the trade-off rather than make the change.

Is a 3 mm internal corner radius always acceptable?

For most pockets up to about 20 mm deep, yes. Beyond that, the 6 mm cutter becomes long and slow, and a 4 or 5 mm radius may be cheaper even though it removes more material.

Do these rules apply to turning as well as milling?

Many do: depth-to-diameter, wall thickness and thread rules carry over. Turning adds its own constraints around undercuts, groove width and boring bar reach, which is why a deep internal groove often means a second operation.

How much does a thin wall add to the price?

On an otherwise simple part, a wall at 0.8 mm instead of 2 mm can add 20% to 40%, because the shop must cut lighter, add finishing passes and accept higher scrap risk. Below 0.5 mm in aluminum, some shops will decline the work.