Minimum Wall Thickness

When designing CNC machined metal parts, a minimum wall thickness of around 0.03 in (≈0.8 mm) is a safe baseline. For plastics, start at ≥ 0.06 in (≈1.5 mm) to reduce warping and clamping deformation in thin-wall machining.

If you need to go thinner:

Add ribs, shorten unsupported spans, or switch to a more rigid material.
For cosmetic thin shells, consider sheet metal or molding depending on volume and tolerance needs.

Very thin walls should always be reviewed with your machining supplier before finalizing drawings — in our engineer-reviewed quotations, thin-wall machining is one of the first checks we perform. Request a quote.

5.2

Hole Diameter, Depth & Spacing

Hole drilling guidelines and standard tool compatibility

For standard drilled holes, most CNC shops are comfortable with minimum diameters around 2.5–3.0 mm; anything below this enters micro-machining territory and drives cost. Smaller holes increase sensitivity in chip evacuation, tool life, and peck drilling time.

Rules of thumb:

Minimum hole diameter ≥ 2.5–3.0 mm for general CNC milling/turning.
Hole depth about 5–8× diameter for standard drills.
Between-hole spacing ≥ 1–1.5× diameter to avoid thin webs.
Hole center to free edge ≥ 1.5–2× diameter to reduce breakout.

For very small or deep holes, review gun drilling, EDM, or process changes during DFM instead of assuming standard drilling cycles.

5.3

Deep Cavities & Blind Pockets

Deep cavity and blind pocket depth guideline

Blind pockets or deep cavities should be no deeper than 3× the tool diameter (3×D). Beyond that, extended-length tools lose rigidity, increasing chatter, tolerance drift, and poor surface finish.

Better options when depth is constrained:

Open one or more walls so the cutter can enter from the side.
Split the part into two components and assemble (bolts/dowels).
Use stepped levels so each level stays within the 3×D guideline.

In short, pockets within 3×D are cheaper, more repeatable, and easier to inspect than deep cavities that push tool reach to the limit.

5.4

Internal Corners / Fillets

Internal corners and fillets sized to end mill radius

Sharp internal corners are difficult or impossible with standard end mills. Use internal radii ≥ tool radius. Example: a 6 mm end mill needs at least a 3 mm internal fillet.

Typical end mill size → minimum fillet radius:

Tool Ø	Tool Radius	Recommended Min. Fillet
3 mm	1.5 mm	≥ 1.5–2.0 mm
6 mm	3.0 mm	≥ 3.0–3.5 mm
10 mm	5.0 mm	≥ 5.0–6.0 mm

When in doubt, err on the side of larger internal radii and mark only corners that must be sharp for function.

5.5

Undercuts and Special Features

Special features often increase setups and fixturing

Undercuts and hidden grooves often require non-standard tools (T-slot, keyseat, side-and-face cutters) plus custom fixtures—raising cost and quote uncertainty versus standard end mills/drills.

Guidelines:

Avoid hidden internal undercuts; open features for standard tool access.
Keep depth/width within common cutter sizes if unavoidable.
Consider splitting into multiple components then bolting/doweling together.
Flag undercuts clearly in drawings and 3D models for accurate RFQ.

5.6

Tolerance Strategy

Default to ±0.005 in (≈±0.13 mm) unless tighter values are function-critical. Over-specifying tolerances increases machining time, setup complexity, and inspection effort.

Tolerance tiers (typical targets):

Tier	Typical Band	Use For
General	±0.10 mm	Non-critical features, general geometry.
Precision fit	±0.05 mm	Sliding fits, aligned faces, mating features.
Critical / reamed	±0.01–0.02 mm	Bores, dowel holes, CTQ features with gauges.

When releasing drawings:

Tighten only on CTQ features that impact function/fit.
Add GD&T only where it adds clarity.
Use a drawing legend to state default tolerance bands.

5.7

Threads & Threaded Hole Design

Threads and threaded hole depth guideline

Keep effective thread length within 2–3× hole diameter and allow run-out in blind holes. Deeper threads rarely add strength but do add time and tap-break risk.

Good practice:

Use correct tap drill size and add a chamfer/countersink.
Provide bottom relief so the tap doesn’t bottom out.
Prefer through threads over blind threads when possible.

Use standard ISO metric or UNC/UNF sizes and standard tap-drill charts. Reference.

5.8

Text, Logos and Markings

Engraving and marking should be on accessible, stiff surfaces

Engraved text/logos can add cycle time if too small or intricate. Keep geometry simple and place markings on flat, accessible faces.

Good practices:

Prefer engraved over raised lettering.
Use simple sans-serif fonts; avoid thin strokes/script.
Min text height ~5 mm, depth 0.3–0.5 mm for typical engraving.
Consider laser marking for strict branding.

5.9

Avoid Slender / Narrow Features

Avoid slender ribs and narrow features to reduce deflection

Slender ribs and narrow tabs deflect under cutting loads, causing chatter, marks, and dimensional drift.

Practical thresholds:

Keep rib height-to-thickness ≤ 8:1.
Keep ribs/tabs ≥ 1.0 mm thick in metals, ≥ 1.5 mm in plastics.

5.10

Minimize Setups & Flips

Reduce setups and flips for better accuracy and lower cost

Each flip or re-clamp introduces positional uncertainty. Fewer setups reduce cost, lead time, and alignment risk.

Design actions:

Unify datums so critical faces/holes share the same reference.
Arrange key features to be reachable in one clamping.

When parts genuinely need multi-sided geometry, 5-axis CNC machining often balances flexibility and accuracy.

5.11

Standard Tool / Cutter Compatibility

Standard cutter compatibility improves CNC DFM and quote stability

Designing around standard cutter and drill sizes is one of the simplest CNC DFM moves: it keeps your CNC machining design guide aligned with real shop tooling.

Common metric tap / drill matches:

Thread	Nominal Ø	Tap Drill (approx.)
M3 × 0.5	3.0 mm	2.5 mm
M6 × 1.0	6.0 mm	5.0 mm
M8 × 1.25	8.0 mm	6.8 mm

5.12

Surface Finish & Post-Processing

Surface finish and post-processing should be planned with tolerances

Surface finish requirements affect machining time and cost. Very low Ra may require slower cutting, extra finishing passes, or secondary processes.

Guidelines:

General machined surfaces: Ra 3.2–6.3 μm is typical and economical.
Sealing/sliding faces: Ra 0.8–1.6 μm often needs dedicated finishing.

5.13

Material-Specific CNC Design Considerations

Material affects minimum walls, radii, and depth guidelines

Guidelines shift depending on whether you machine aluminum, stainless/tool steels, or plastics—mainly in wall thickness, fillets, and pocket depths.

Typical trends:

Aluminum: thinner walls and more aggressive cutting.
Stainless/tool steels: thicker sections, larger fillets.
Plastics: thicker walls (≈1.5 mm+) to reduce warping.

Design Feature	Baseline Rule	Cost Risk	Quote Accuracy Risk	Inspection Risk	Escalate to DFM?
Thin Walls	Metal ≥0.8mm / Plastic ≥1.5mm	High	Medium	High	Yes
Deep Pockets	Depth to Diameter Ratio < 3:1	High	High	Medium	Yes
Tight Tolerances	Default ±0.13mm (Limit to CTQ)	High	High	High	Yes
Multi-face Geometry	Minimize setup (Datum transfer risk)	High	High	High	Yes
Internal Radii	Fillets ≥ Tool Radius (R > 3mm)	Medium	Medium	Low	Usually

Design Principle	Priority / Type	Recommendation (in/mm)	Cost Impact	Rationale & Decision Logic
Wall Thickness	Recommended Baseline	$\ge 0.03$ in ($\approx 0.8$ mm) for metals; $\ge 0.06$ in ($\approx 1.5$ mm) for plastics.	High	Ensures rigidity and tool stability. Feasibility varies by material stiffness and wall height; thin unsupported sections increase scrap and inspection risk.
Pocket Depth	Recommended Baseline	Depth $\le 3\times$ tool diameter ($3\times$D).	High	Long tools suffer from poor rigidity and vibration. Deep cavities should be reviewed for 5-axis CNC machining for deep cavities to maintain accuracy.
Internal Corner Radius	Recommended Baseline	Fillet radius $\ge$ tool radius.	Medium	Industry standard baseline to ensure tool stability and reduce cycle time. Larger radii minimize tiny-cutter dependency and tooling instability.
Tolerance Guidelines	Critical when Specified	$\pm 0.005$ in ($\approx \pm 0.13$ mm) default.	High	Practical baseline to balance cycle time, tool wear, and inspection load. Review tolerance feasibility for machined features for tighter CTQ bands.
Threaded Hole Length	Recommended Baseline	Thread length $\le 2-3\times$ nominal diameter.	Medium	Longer threads add cycle time and tap-break risk without extra strength. Use as a practical programming baseline for consistency.
Minimize Setups / Flips	Recommended Baseline	Minimize unique machining orientations.	High	Extra setups increase alignment risk and inspection burden. Review when fewer setups justify 5-axis to maintain datum continuity.

Common Mistake	Why It’s a Problem
Too-thin wall thickness	Designing walls below about 0.03 in (≈ 0.8 mm) for metals or 0.06 in (≈ 1.5 mm) for plastics causes deformation, tool deflection, and vibration during cutting. Thin walls are harder to clamp, more likely to chatter, and increase scrap.
Sharp internal corners instead of fillets	Standard end mills cannot machine perfectly sharp internal angles. Forcing tiny corner radii requires very small tools, slow feed rates, or secondary processes like EDM. Fillets improve tool access, tool life, and stress distribution.
Overly tight tolerances on all features	Specifying tight tolerance bands everywhere (for example ±0.01–0.02 mm on non-critical geometry) drastically increases machining and inspection time. Only CTQ features should use the tightest bands; general surfaces work well with ±0.05–0.10 mm.
Deep pockets beyond 3× tool diameter	Going beyond the 3×D depth guideline forces the use of long, slender tools that vibrate, leave poor surface finish, and struggle to hold tolerance. It often requires special tooling and extra passes, driving up cost and cycle time.
Slender or fragile structures	Thin ribs or unsupported sections are prone to breaking or distortion. High height-to-thickness ratios cause deflection under cutting loads, leading to chatter marks, dimensional errors, or broken tools. Additional supports or redesign are usually required.
Non-standard hole or slot sizes	Using hole diameters or slot widths that do not match standard drill or cutter sizes forces custom tooling, reaming, or interpolation with small tools. This increases machining time, setup work, and lead time for tool procurement.
Too many setups or scattered features	Placing critical features across many different faces or requiring multiple orientations increases the number of setups and part flips. Every re-clamp introduces alignment error, adds fixture cost, and lengthens cycle time. Grouping key features into fewer datums is almost always more economical.
Abrupt wall thickness transitions	Sharp changes in section thickness concentrate internal stress and can cause distortion during machining, heat treatment, or anodizing. Smooth tapers or filleted transitions distribute stress more evenly and help parts remain stable.

Feature	✕ Poor Design	✓ Optimized Design
Wall Thickness	0.5 mm — too thin for most metals, leads to deflection under clamping and cutting forces.	≥ 0.8 mm — ensures structural integrity, stable clamping, and reliable machinability.
Internal Corners	Sharp 90° internal angles that are difficult or impossible to machine with standard end mills.	3 mm radius fillets that match common tool radii, improving tool access, life, and surface finish.
Pocket Depth	12 mm depth machined with a 3 mm tool (4× tool diameter), causing vibration and poor finish.	9 mm depth with the same 3 mm tool (3× tool diameter), staying within the stable 3×D guideline.
Tolerances	±0.001 in on all features — excessive and expensive for non-critical geometry.	±0.005 in on non-critical features, tightened to ±0.002 in only where truly needed.
Machining Outcome	High cost, poor yield, increased tool wear, and slow production due to unstable cutting conditions.	Efficient, cost-effective machining with reduced tooling stress, better first-pass yield, and shorter lead time.

DFM Practice	Description
Validate Geometry Early	Ensure wall thickness, radii, hole sizes, and pocket depths match standard CNC tooling and fixturing capabilities. This validation happens as soon as RFQ files are received, before pricing is confirmed.
Mark Challenging Features	Highlight risky features in CAD and drawings (deep pockets, thin walls, tight GD&T, critical fits) so shops can focus on them during quoting and process planning, rather than discovering them on the machine.
Define Non-Machinable Zones	Identify regions that cannot be accessed with standard tools or reasonable setups and either redesign those areas, switch processes (e.g. EDM), or clearly mark them as out of scope before PO placement.
Incorporate Machinist Feedback	Share early design files with CNC partners and adjust models based on their recommendations for toolpaths, datums, and clamping. This is where many cost and quality improvements are captured during the 24–48 h DFM review.
Use Iterative Design Loops	Promote short, focused design–feedback loops between engineering and manufacturing. Small geometry changes (radii, tolerances, setups) can move parts from “difficult and expensive” into a stable, repeatable machining window.

Frequently Asked Question	Answer
What is the minimum wall thickness for CNC-machined parts?	For most CNC-machined parts, a practical minimum wall thickness is about 0.03 in (≈ 0.8 mm) for metals and 0.06 in (≈ 1.5 mm) for plastics, which keeps walls stiff enough for clamping, reduces chatter during cutting, and helps parts remain stable during cooling and finishing. Thinner walls may be possible in low-load or cosmetic areas, but they should be discussed with your machinist and may require ribs, shorter spans, or alternative processes such as sheet metal or molding.
How deep can I make a pocket or cavity in CNC design?	As a rule of thumb, limit blind pocket or cavity depth to about 3× the cutting tool diameter; going deeper than this quickly reduces tool rigidity, increases vibration, and makes it harder to hold tolerances and surface finish. If deeper features are required, consider opening one side of the pocket, using stepped depths, or redesigning the part into multiple pieces that can be machined separately and then assembled.
What tolerances are standard for CNC machining?	A general CNC starting point is about ±0.005 in (≈ ±0.13 mm) for most features, with tighter bands reserved for critical fits or gauged dimensions, which may be held around ±0.002 in (≈ ±0.05 mm) or better depending on the process. Applying tight tolerances everywhere increases cycle time and inspection effort. Mark CTQ features clearly and keep non-critical geometry at more relaxed values such as ±0.05–0.10 mm.
Why are internal fillets important in CNC design?	Internal fillets are important because standard end mills cannot cut perfectly sharp internal corners; providing a radius equal to or larger than the tool radius allows proper tool access, reduces cutting stress, and improves surface finish. Larger internal radii also allow the use of stiffer, larger-diameter tools with higher feed rates, which reduces machining time and extends tool life.
Can I design threaded holes of any depth?	No. Threaded length is usually most effective at about 2–3× the nominal hole diameter; beyond this, extra thread depth adds machining time but provides very little additional strength or pull-out resistance in most materials. Design blind holes with a small unthreaded run-out at the bottom so taps do not bottom out, and consider through threads wherever possible because they are easier to machine and clean.
Are non-standard hole sizes a problem?	Yes—specifying hole diameters or slot widths that do not match standard drill and cutter sizes often requires custom tools, reaming, or interpolation with small end mills, all of which increase cycle time, setup complexity, and sometimes tooling cost. Whenever possible, align hole sizes with common drills and tap-drill charts so shops can use off-the-shelf tooling and standard programs.
What happens if I include thin, unsupported features?	Thin, unsupported features such as slender ribs, tabs, or tall narrow walls tend to deflect, vibrate, or even break during machining, which can lead to chatter marks, dimensional errors, and higher scrap or rework rates. If such features are functionally required, add local thickening, gussets, temporary support tabs, or alternative processes to keep machining stable and predictable.
What are good rules for CNC hole spacing?	For most CNC machining, keep at least 1–1.5× hole diameter between holes and 1.5–2× diameter from a hole center to a free edge. This avoids thin webs, breakout, and clamping issues, and makes it easier to maintain tolerances and surface finish around the hole pattern.
How does surface finish affect CNC machining cost?	Tighter surface finish requirements typically add machining time and sometimes extra processes. General machined surfaces around Ra 3.2–6.3 μm are economical; moving to Ra 0.8–1.6 μm may require slower cutting parameters, additional finishing passes, or secondary operations. It is best to reserve very fine finishes only for sealing faces or surfaces where they truly matter.

Injection Molding

CNC Machining

Sheet and Tube Fabrication

Additive Manufacturing

Quick RFQ Risk Table for CNC Part Design

Tool Access, Cutter Geometry, and Cycle-Time Limits

Setup Count, Datum Transfer, and Dimensional Risk

Material Stiffness and Part Stability During Machining

Wall Thickness Guidelines

Pocket Depth and Long-Tool Risk

Internal Corner Radius and Tooling Limits

Hole Diameter, Depth, and Edge Distance

Threads, Bottom Relief, and Tapping Limits

Slots, Ribs, Tabs, and Deformation Risk

Deep Cavities, Compound Angles, and Hard-to-Reach Features

Single-Setup Machining and Better Datum Continuity

When 5-Axis Adds Cost Without Real Benefit

What is a realistic default tolerance for CNC machining?

Which features should carry tight tolerances?

When CMM, FAI, or Special Inspection Planning Is Required