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.

Holes Design holes at standard drill sizes. Random dimensions like 0.378” require special tooling or interpolation. Standard sizes (letter, number, fractional, metric) cut faster and cost less.

Common standard drill sizes:

• Fractional: 1/4”, 5/16”, 3/8”, 1/2”, etc.
• Letter: A (0.234”) through Z (0.413”)
• Number: #1 (0.228”) through #80 (0.0135”)
• Metric: 3mm, 4mm, 5mm, 6mm, 8mm, 10mm, etc.

Threads Use common thread sizes. UNC (coarse) and UNF (fine) in standard sizes machine quickly. Unusual threads like 3/8-18 or M7x0.75 require special taps.

Most economical threads: #6-32, #8-32, #10-24, #10-32, 1/4-20, 5/16-18, 3/8-16, 1/2-13 (UNC sizes)

Corner Radii Internal corners require radius equal to the cutter radius. Standard end mills come in standard sizes. Specifying 0.093” radius forces purchase of a 3/16” end mill. Specify 0.125” (1/4”) or 0.0625” (1/8”) and standard tooling works.

Rule 2: Avoid Deep Pockets

Deep pockets require long tools that deflect, chatter, and cut slowly.

The 4:1 rule: Pocket depth should not exceed 4x the smallest width dimension. A 0.5” wide pocket should be no deeper than 2”.

What happens when violated:

• Long slender tools deflect, causing dimensional variation
• Feed rates must decrease dramatically
• Multiple passes with lighter cuts
• Possible tool breakage
• Special long-reach tooling may be required

Cost impact: Deep pockets can increase machining time 3-5x compared to shallow geometry.

Solutions:

• Redesign to reduce depth
• Open one side (slot instead of pocket)
• Increase pocket width to allow larger tool
• Accept radius in corners from larger tool

Rule 3: Limit Thin Walls

Thin walls flex under cutting forces, causing vibration (chatter) and dimensional problems.

Minimum wall thickness guidelines:

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

Below these thresholds:

• Special fixturing required
• Extremely light cuts necessary
• Multiple spring passes for accuracy
• High risk of distortion or scrap

Cost impact: Thin-wall machining can add 50-200% to part cost.

Solutions:

• Thicken walls where possible
• Add temporary support features (removed after machining)
• Accept wider tolerances on thin sections
• Consider alternative processes (wire EDM, sheet metal)

Rule 4: Eliminate Sharp Internal Corners

Rotating cutters cannot create sharp internal corners. Period.

Every internal corner will have a radius equal to the cutter radius. Specifying sharp corners forces secondary operations (EDM, broaching) that dramatically increase cost.

Best practice: Specify internal corner radius at least 1/3 of pocket depth. For a 0.75” deep pocket, use 0.25” corner radius minimum.

If you need smaller radii:

• Use stress-relief notches (small circular cuts at corners)
• Accept the cost of EDM operations
• Redesign mating parts to accommodate radius

Exception: External corners can be sharp—tools cut these naturally.

Rule 5: Specify Tolerances Only Where Needed

Tolerances tighter than ±0.005” trigger special handling, slower feeds, additional inspection, and higher cost.

Standard machining capability: ±0.005” (±0.127mm)

Cost multipliers for tighter tolerances:

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:

• Mating/interface dimensions
• Press-fit or close-fit features
• Sealing surfaces
• Bearing fits

Leave at standard tolerance:

• Non-functional dimensions
• Cosmetic features
• Clearance holes
• General envelope dimensions

Drawings plastered with ±0.001” on every dimension signal inexperience and guarantee high quotes.

Rule 6: Design for Standard Setups

Every setup (repositioning the part in the machine) adds cost: handling time, re-fixturing, realignment, and first-article verification.

Minimize setups by:

• Keeping features accessible from one direction
• Avoiding features on more than 3 faces if possible
• Designing one flat face for primary fixturing
• Including flat parallel surfaces for clamping

5-axis machining can access multiple faces in one setup but costs 3-5x more per hour than 3-axis. Design for 3-axis unless geometry demands otherwise.

Best case: All features machined from top with part fixtured on bottom.

Expensive case: Features on all six faces requiring multiple setups or 5-axis work.

Rule 7: Add Chamfers, Not Fillets (External)

External fillets require ball end mills and 3D tool paths. External chamfers use standard tools and simple 2D paths.

Fillet (radius on external edge): Requires 3D contouring, ball mill, slow cutting Chamfer (angled cut on external edge): Fast, simple, standard tooling

Unless the design specifically requires a rounded edge, specify chamfers for deburring. Standard 45° chamfers at 0.015-0.030” are quick and effective.

Exception: Internal fillets (in pockets) happen naturally from the tool radius—no extra cost.

Rule 8: Keep Thread Depths Reasonable

Deep threads risk tap breakage, the most dreaded shop floor failure.

Safe thread depth: 2x diameter for through holes, 1.5x diameter for blind holes.

A 1/4-20 thread should be no deeper than 0.5” (through) or 0.375” (blind).

Why it matters:

• Taps are brittle and break under excessive load
• Broken taps often require EDM removal ($$$)
• Deep blind holes trap chips, increasing breakage risk
• Thread strength doesn’t increase proportionally with depth

Full thread strength is achieved at approximately 1.5x diameter. Deeper doesn’t mean stronger—it just means 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 are simply impossible.

Check for:

• Undercuts: Internal features that can’t be reached straight-on
• Deep holes with features: Threads or counterbores deep in blind holes
• Intersecting features: Complex internal geometry
• Narrow slots: Require small fragile tools

Standard tool reach: 3-4x tool diameter without special tooling.

If your design requires reaching 3” deep with a 0.25” tool (12:1 ratio), expect problems and cost.

Rule 10: Consider Material Machinability

Material choice affects machining time by 2-4x. Design with material in mind.

Easy to machine (faster, cheaper):

• 6061 Aluminum
• 12L14 Steel (free-machining)
• Brass
• Acetal, UHMW, most plastics

Moderate:

• 7075 Aluminum
• 4140 Steel
• 303 Stainless
• Nylon, PEEK

Difficult (slower, more expensive):

• 316 Stainless
• 17-4 PH Stainless
• Titanium
• Inconel
• Hardened steels

Practical impact: The same part in 316 stainless might cost 2x what it costs in 6061 aluminum—partly material, mostly machining time.

Quick DFM Checklist

Before submitting drawings, verify:

• Holes at standard drill sizes
• Internal corner radii ≥ 1/3 pocket depth
• Pocket depths ≤ 4x width
• Wall thickness above minimums
• Tight tolerances only where functionally required
• Features accessible without multiple setups
• Thread depths ≤ 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.