Wall thickness and fillet design are among the most impactful decisions you make for a CNC part. Too thin and the part deforms during machining, cracks under load, or costs 3x more due to slow feeds and special tooling. Get these right and you save money on every order.
The table below shows the absolute minimum and the recommended wall thickness for common CNC materials. "Minimum" means it can be done but with higher scrap risk and slower machining. "Recommended" is the sweet spot for reliable production at reasonable cost.
| Material | Absolute Minimum | Recommended | What Happens If Too Thin |
|---|---|---|---|
| Aluminum (6061, 7075) | 0.5 mm | 1.0 mm | Chatter during finishing, wall pushes away from cutter, dimension out of tolerance. Thin aluminum walls vibrate and produce poor surface finish. |
| Steel (1045, 4140) | 0.8 mm | 1.5 mm | Tool deflection at 0.5 mm is severe with steel. Walls bow inward. Harder steels amplify this — tool rubs instead of cuts. |
| Stainless Steel (304, 316) | 0.9 mm | 1.5 mm | Stainless work-hardens rapidly. Thin walls overheat, warp, and may crack. Tool wear accelerates dramatically. |
| Titanium (Ti-6Al-4V) | 1.0 mm | 1.5 mm | Titanium has low thermal conductivity — heat builds up in thin sections causing thermal warping. Extremely slow feeds required. |
| Copper & Brass | 0.5 mm | 0.8 mm | Soft material helps — copper can go quite thin. But very thin copper walls are fragile during handling and may bend before assembly. |
| Engineering Plastics (Delrin, Nylon, PEEK) | 0.4 mm | 0.8 mm | Plastics deflect under cutting force. Thin walls flex away from the tool, producing inconsistent dimensions. PEEK is stiffer but costs 10x more. |
Beyond the absolute minimum, several ratios and relationships govern good wall design. Follow these to avoid surprises during manufacturing.
| Rule | Guideline | Why It Matters |
|---|---|---|
| Wall-to-feature height ratio | Wall thickness should be at least 1/5 of the adjacent feature height (wall standing up from the base) | A tall thin wall acts like a cantilever beam. A 10 mm tall wall needs at least 2 mm thickness to resist deflection from cutting forces. |
| Unsupported wall height | Max unsupported height = 8× wall thickness (aluminum), 5× wall thickness (steel) | Beyond this ratio, the wall vibrates during machining. Either thicken the wall or add ribs for support. |
| Uniform wall thickness | Keep walls within 20% of each other's thickness on the same part | Uneven walls cause differential cooling in heat treatment and uneven stress relief, leading to warpage. |
| Corner transition | Gradual transitions between thick and thin sections | Abrupt thickness changes create stress concentrators. Add a fillet or taper when transitioning between sections of different thickness. |
| Rib design | Rib thickness = 0.6× wall thickness; rib height ≤ 5× rib thickness | Thick ribs create sink marks on the opposite surface (in castings) and add machining time (in CNC). Keep ribs thin and well-filleted. |
| Cost impact of thin walls | Walls at minimum thickness: +30–80% machining time vs. recommended thickness | Thin walls require reduced feeds, spring passes, and often multiple setups with specialized tooling. The cost penalty is significant. |
Every CNC end mill is cylindrical, which means it cannot cut a sharp internal corner. The smallest internal corner radius you can achieve equals the tool radius. This is one of the most fundamental constraints in CNC machining, and ignoring it is one of the most common design mistakes.
Tool geometry: An end mill with a 6 mm diameter has a 3 mm corner radius. It physically cannot produce an internal corner smaller than R3. To get a smaller radius, you need a smaller tool — which means slower machining, more passes, and higher cost.
Stress concentration: Sharp internal corners are stress concentrators. Under cyclic loading, a sharp corner is where fatigue cracks initiate. Adding even a small fillet (R0.5 mm) dramatically reduces stress concentration. In aerospace and structural applications, fillets are not optional — they're critical for part life.
Tool life: A sharp internal corner forces the tool to decelerate, pause, and change direction — all of which increase tool wear. Filleted corners let the tool maintain a smooth arc path, extending tool life and improving surface finish.
| Tool Diameter | Corner Radius | Recommended Internal Fillet | Cost Level |
|---|---|---|---|
| φ16 mm (5/8") | R8 mm | R8 mm or larger | Standard (lowest cost) |
| φ10 mm (3/8") | R5 mm | R5 mm or larger | Standard |
| φ6 mm (1/4") | R3 mm | R3 mm or larger | Standard |
| φ4 mm (5/32") | R2 mm | R2 mm or larger | Moderate |
| φ3 mm (1/8") | R1.5 mm | R1.5 mm or larger | Moderate |
| φ2 mm | R1 mm | R1 mm or larger | Higher |
| φ1 mm | R0.5 mm | R0.5 mm | Premium (slow, fragile tool) |
| < φ1 mm (wire EDM or specialized) | R0.2 mm | R0.2–R0.5 mm | Very high cost (special process) |
Every step down in fillet radius means a smaller, slower tool and more machining passes. The relationship is not linear — halving the fillet radius can more than double the cost of that feature.
| Fillet Radius | Relative Cost of Feature | Reason |
|---|---|---|
| R3–R6 mm | 1.0x (baseline) | Standard end mill, fast material removal |
| R1–R2 mm | 1.3–1.5x | Smaller tool, more passes, slower feed rate |
| R0.5 mm | 1.8–2.5x | Fragile tool, very slow feed, frequent tool changes |
| < R0.5 mm | 3.0–5.0x | May require wire EDM or specialized tooling |
External corners are the opposite of internal corners — the tool can easily reach them, so sharp external edges are technically possible. However, leaving sharp edges on a machined part is almost always a bad idea in practice.
The industry standard edge break is 0.5 mm (0.020") chamfer or radius on all sharp edges unless otherwise specified. Many machine shops apply this automatically as a default deburring operation. This is included in the cost and should not require a special note.
| Edge Treatment | When to Use | Notes |
|---|---|---|
| 0.5 mm chamfer (default) | Most parts, all edges unless noted | Standard deburring. Included in base price. Safe to handle, protects from burrs. |
| 0.5 mm radius | Edges that will be handled frequently or sealed against a gasket | Radius is gentler than chamfer for sealing surfaces and user-contact edges. |
| No edge break (sharp) | Cutting edges (knives, blades), matching surfaces requiring line contact | Must be explicitly called out on the drawing. Increases handling risk and injury potential. |
| Large radius (R2+) | Ergonomic parts, cosmetic exterior surfaces | Requires a specific tool path. Costs slightly more than standard edge break. |
Chamfer is cheaper and faster to apply — a single pass with a chamfer mill or even a spot drill handles it. Chamfers also make assembly easier because they guide mating parts into position.
Radius (fillet on external corner) is preferred when the edge contacts a seal, O-ring, or human hand. Radii distribute stress better and look better on cosmetic parts. However, they require a ball-nose end mill or a specific radius tool, which adds a tool change.
Draft angles (a taper applied to vertical surfaces to allow part removal from a mold) are primarily a concern for casting, forging, injection molding, and sheet metal forming. CNC machining does not require draft angles — the tool cuts freely in all directions and there is no mold to pull the part from.
However, there are a few CNC-specific situations where draft or taper matters:
| Feature | When Draft/Taper Matters | Guideline |
|---|---|---|
| Tapered holes | For taper pins, dowel alignment, or self-locking fits | Specify taper angle (e.g., 1:50 for metric taper pins) and use a boring bar or taper reamer. |
| Conical features | Valve seats, nozzle profiles, countersinks | Standard countersink angles: 60°, 82°, 90°, 120°. Custom angles require specialty tooling. |
| CNC from cast blank | When machining a part that starts as a casting | The casting itself needs draft, but the CNC machining removes it. Account for draft when calculating stock allowance. |
| Deep pockets | Very deep pockets (>4× diameter) may develop slight taper from tool deflection | If taper must be avoided, use a spring pass (light finishing cut with no material removal intent). |
When an end mill cuts a pocket, the corners where the wall meets the floor will have a radius equal to the tool's corner radius. This is the floor radius, and it's one of the most common sources of confusion on engineering drawings.
A standard flat end mill has a small corner radius (typically R0.5–R1.0 mm even on a 10 mm tool). A bull-nose end mill has a larger corner radius (R2–R6 mm). A ball-nose end mill has a radius equal to half the tool diameter.
The floor radius in your pocket will always equal the tool's corner radius. If you want a flat floor (R0), you need a flat end mill with sharp corners — and those only exist in smaller sizes. For a large pocket with a truly flat floor, you need to use a smaller tool to clean out the corners, which adds machining time and cost.
| Floor Radius | Tool Required | Relative Cost | Notes |
|---|---|---|---|
| R3–R6 mm | Bull-nose end mill (φ10–16 mm) | 1.0x (baseline) | Fastest material removal. Large radius is no problem for most applications. |
| R1–R2 mm | Standard flat end mill | 1.0x | Most end mills have R0.5–R1 corner as standard. This is the typical floor radius you get. |
| R0.5 mm | Small flat end mill or corner radius end mill | 1.2–1.5x | Requires a cleanup pass with a smaller tool. Adds one tool change and extra machining time. |
| R0.2–R0.3 mm | Small end mill + careful toolpath | 1.5–2.0x | Fragile tool, slow feed. Multiple spring passes needed to achieve dimensional accuracy. |
| R0 (sharp corner) | Wire EDM or lapping | 3.0–5.0x | Impossible with standard end mills. Requires wire EDM or manual lapping. Rarely worth the cost. |
The table below summarizes how different design decisions for walls, fillets, and radii affect machining cost. Use this as a quick reference when reviewing your design before sending it to manufacturing.
| Design Feature | Standard Specification | Tight / Difficult Spec | Cost Multiplier |
|---|---|---|---|
| Wall thickness (aluminum) | ≥ 1.0 mm | 0.5–0.8 mm | 1.3–1.8x |
| Wall thickness (steel) | ≥ 1.5 mm | 0.8–1.2 mm | 1.4–2.0x |
| Internal fillet radius | R3–R6 mm | R0.5 mm or smaller | 1.8–3.0x |
| Floor radius in pocket | R1–R3 mm | R0 (sharp) | 3.0–5.0x |
| Edge break | 0.5 mm chamfer (default) | Sharp edges (no break) | 1.0x (but higher handling risk) |
| External radius | Sharp or 0.5 mm break | Large cosmetic radius (R5+) | 1.1–1.3x |
| Deep pocket aspect ratio | Depth ≤ 4× width | Depth > 6× width | 1.5–2.5x |
| Tall thin wall | Height ≤ 5× thickness | Height > 8× thickness | 1.5–2.0x |
These are the wall thickness and fillet errors we see most often in customer drawings. Avoid these and your parts will be cheaper, stronger, and faster to produce.
| # | Mistake | What Happens | Correct Approach |
|---|---|---|---|
| 1 | Specifying R0 internal corners | Impossible with standard end mills. Machinist must use wire EDM or ask for design change. Delays the project. | All internal corners must have a fillet radius ≥ R0.5 mm. Match to standard tool sizes (R1, R1.5, R2, R3). |
| 2 | Unequal fillet radii on the same feature | Requires multiple tool changes. Adds setup time and cost. | Use one fillet radius per pocket feature wherever possible. Standardize to a single tool radius across the part. |
| 3 | Very thin walls adjacent to thick sections | Thin wall warps or deflects during machining due to stress from the adjacent thick section. Dimensional non-conformance. | Keep wall thickness uniform. Add gradual transitions between thick and thin sections. |
| 4 | Deep pockets with small floor radius | Requires a long, thin tool that deflects. Poor surface finish, inaccurate dimensions, broken tools. | Increase floor radius proportionally to pocket depth. Deep pockets should have larger floor radii. |
| 5 | No edge break specified | Shop applies default 0.5 mm break — usually fine, but if you needed sharp edges, the part is already made wrong. | If sharp edges are required, call them out explicitly. If not, add "BREAK SHARP EDGES 0.5 mm MAX" to the drawing notes. |
| 6 | Calling out draft angle on a CNC part | Confuses the machinist. Draft is for cast/molded parts. CNC can cut taper, but "draft" implies a mold. | Specify the actual taper angle as a dimensional callout (e.g., "1:50 taper" or "2° included angle"), not "draft." |
| 7 | Fillets smaller than tool radius available for the feature depth | A 20 mm deep pocket with R0.5 corners requires a 1 mm tool that's too long and flexible. Tool breaks or deflects. | Rule of thumb: tool reach should not exceed 8× tool diameter. For deep pockets, use larger fillet radii. |
| 8 | Ignoring anodize/paint thickness on thin walls | Wall is at 0.6 mm nominal, anodize adds 25 μm per side (0.05 mm total), now it's 0.7 mm — but tolerance stack-up eats the rest. | Account for surface treatment thickness in your wall calculation. Add 2× coating thickness to minimum wall spec. |
| 9 | Sharp floor corners (R0) on sealed pockets | O-ring or sealant cannot seat properly in a sharp corner. Leak path forms. | Specify R0.5–R1.0 minimum floor radius for any pocket that will hold a seal, gasket, or O-ring. |
| 10 | Wall thickness not called out explicitly | Wall thickness is a derived dimension — it depends on pocket depth and pocket floor position. Ambiguity leads to disputes. | Call out minimum wall thickness directly on the drawing as a critical dimension, especially for thin walls. |