Design for Manufacturability: 10 Rules for Cost-Effective CNC Parts

Design decisions lock in 70% of manufacturing cost before machining even begins. The same functional part can cost $50 or $150 depending on how it’s designed. These ten rules address the most common cost drivers we see in customer drawings—fix these, and your quotes will drop.

Rule 1: Respect Standard Tool Sizes

Every non-standard dimension requires a non-standard tool, adding cost and lead time.

When designing holes, specify standard drill sizes whenever possible. Random dimensions like 0.378” require special tooling or circular interpolation, both of which add time and cost. Standard sizes in fractional increments (1/4”, 5/16”, 3/8”, 1/2”), letter sizes (A through Z, covering 0.234” to 0.413”), number sizes (#1 through #80), and metric increments (3mm, 4mm, 5mm, and up) all cut faster and cost less because every shop has these tools ready to go.

Thread selection follows the same logic. UNC and UNF in standard sizes machine quickly with readily available taps. Unusual threads like 3/8-18 or M7x0.75 require special taps that may not be in stock. The most economical choices are the workhorses: #6-32, #8-32, #10-24, #10-32, 1/4-20, 5/16-18, 3/8-16, and 1/2-13.

Internal corners require radius equal to the cutter radius, so standard end mill sizes matter here too. Specifying a 0.093” radius forces purchase of a 3/16” end mill that might not be on hand. Specify 0.125” (1/4”) or 0.0625” (1/8”) and standard tooling works immediately.

Rule 2: Avoid Deep Pockets

Deep pockets require long tools that deflect, chatter, and cut slowly. The 4:1 rule provides the guideline: pocket depth should not exceed 4x the smallest width dimension. A 0.5” wide pocket should be no deeper than 2”.

When this rule gets violated, problems cascade. Long slender tools deflect under cutting forces, causing dimensional variation across the pocket floor. Feed rates must decrease dramatically to prevent tool breakage. Multiple passes with lighter cuts become necessary. Tool breakage becomes a real risk, and special long-reach tooling may need to be ordered.

The cost impact is substantial—deep pockets can increase machining time 3-5x compared to shallow geometry. When faced with a deep pocket requirement, consider redesigning to reduce depth, opening one side to create a slot instead of a pocket, increasing pocket width to allow a larger and stiffer tool, or accepting a larger radius in corners from the larger cutter.

Rule 3: Limit Thin Walls

Thin walls flex under cutting forces, causing vibration (chatter) and dimensional problems. The minimum wall thickness varies by material.

Material	Minimum Wall
Aluminum	0.040”
Steel	0.030”
Plastics	0.060”
Stainless	0.030”

Below these thresholds, special fixturing becomes necessary to support the walls. Extremely light cuts spread machining time considerably. Multiple spring passes may be needed for accuracy as the wall flexes away from the tool and springs back. The risk of distortion or scrap increases significantly.

Thin-wall machining can add 50-200% to part cost. When possible, thicken walls in the design, add temporary support features that get removed after machining, accept wider tolerances on thin sections, or consider alternative processes like wire EDM or sheet metal fabrication.

Rule 4: Eliminate Sharp Internal Corners

Rotating cutters cannot create sharp internal corners. This is geometry, not capability—no amount of money changes it.

Every internal corner will have a radius equal to the cutter radius. Specifying sharp corners forces secondary operations like EDM or broaching that dramatically increase cost and lead time. The best practice is to specify internal corner radius at least 1/3 of pocket depth. For a 0.75” deep pocket, use 0.25” corner radius minimum.

If your design genuinely requires smaller radii, options include stress-relief notches (small circular cuts at corners that create clearance), accepting the cost of EDM operations, or redesigning mating parts to accommodate the radius that machining naturally produces.

External corners are the exception—tools cut these naturally, so sharp external corners add no cost.

Rule 5: Specify Tolerances Only Where Needed

Tolerances tighter than ±0.005” trigger special handling, slower feeds, additional inspection, and higher cost. For detailed guidance on tolerance selection, see our CNC machining tolerances guide.

Standard machining capability sits comfortably at ±0.005” (±0.127mm). Tighter tolerances multiply costs.

Tolerance	Cost Impact
±0.005”	Baseline (1.0x)
±0.002”	1.3-1.5x
±0.001”	1.5-2.0x
±0.0005”	2.5-4.0x

Apply tight tolerances only to dimensions that actually require them: mating and interface dimensions where parts must fit together precisely, press-fit or close-fit features, sealing surfaces, and bearing fits. Leave everything else at standard tolerance: non-functional dimensions, cosmetic features, clearance holes, and general envelope dimensions.

Drawings plastered with ±0.001” on every dimension signal inexperience and guarantee high quotes. Experienced designers know that most dimensions don’t need tight control to achieve functional requirements.

Rule 6: Design for Standard Setups

Every setup—repositioning the part in the machine—adds cost through handling time, re-fixturing, realignment, and first-article verification of the new orientation.

Minimize setups by keeping features accessible from one direction, avoiding features on more than three faces when possible, designing one flat face suitable for primary fixturing, and including flat parallel surfaces that provide good clamping reference.

Five-axis machining can access multiple faces in one setup, but it costs 3-5x more per hour than 3-axis work. Design for 3-axis unless geometry genuinely demands otherwise. The best case is all features machined from the top with the part fixtured on the bottom. The expensive case is features on all six faces requiring multiple setups or 5-axis capability.

Rule 7: Add Chamfers, Not Fillets (External)

External fillets require ball end mills and 3D tool paths with slow, careful contouring. External chamfers use standard tools and simple 2D paths.

For deburring external edges, specify chamfers unless the design specifically requires a rounded edge. Standard 45-degree chamfers at 0.015-0.030” are quick to machine and effective at removing sharp edges.

Internal fillets are the exception—they happen naturally from the tool radius and add no cost. It’s only external radii that require the expensive 3D contouring operations.

Rule 8: Keep Thread Depths Reasonable

Deep threads risk tap breakage—the most dreaded shop floor failure because broken taps are extremely difficult to remove.

Safe thread depth is 2x diameter for through holes and 1.5x diameter for blind holes. A 1/4-20 thread should be no deeper than 0.5” in a through hole or 0.375” in a blind hole.

Taps are brittle and break under excessive load. Broken taps often require EDM removal at significant cost, as drilling them out risks damaging the threads. Deep blind holes trap chips, increasing breakage risk further. And here’s the key insight: thread strength doesn’t increase proportionally with depth. Full thread strength is achieved at approximately 1.5x diameter. Going deeper doesn’t make the connection stronger—it just makes manufacturing riskier and more expensive.

Rule 9: Provide Adequate Tool Access

Machinists can only cut what tools can reach. Features in restricted areas require special tooling or may simply be impossible to manufacture.

Standard tool reach runs 3-4x tool diameter without requiring special long-reach tooling. If your design requires reaching 3” deep with a 0.25” tool (a 12:1 ratio), expect problems and significant cost increases.

Watch for undercuts that can’t be reached from any straight-on approach, threads or counterbores deep in blind holes, complex intersecting internal geometry, and narrow slots that require small fragile tools. Each of these features either requires special tooling, secondary operations, or design revision.

Rule 10: Consider Material Machinability

Material choice affects machining time by 2-4x for the same geometry. Design with material machinability in mind.

Easy-to-machine materials cut faster and cost less: 6061 aluminum, 12L14 free-machining steel, brass, and most plastics like acetal and UHMW. Moderate materials include 7075 aluminum, 4140 steel, 303 stainless, nylon, and PEEK. Difficult materials that run slower and cost more include 316 stainless, 17-4 PH stainless, titanium, Inconel, and hardened steels.

The practical impact is significant. The same part in 316 stainless might cost 2x what it costs in 6061 aluminum—partly due to material cost, but mostly due to dramatically longer machining time.

Quick DFM Checklist

Before submitting drawings, verify:

• Holes at standard drill sizes
• Internal corner radii at least 1/3 pocket depth
• Pocket depths at most 4x width
• Wall thickness above minimums
• Tight tolerances only where functionally required
• Features accessible without multiple setups
• Thread depths at most 2x diameter
• External edges chamfered, not filleted
• No undercuts or internal features requiring special access
• Material selected considering machinability

We Review Your Designs

NextGen Components provides DFM feedback on every quote. When we see cost drivers in your design, we’ll point them out—along with alternatives that maintain function at lower cost.

Have a design you want reviewed before finalizing? Send it to our team and we’ll identify optimization opportunities.