Design for manufacturability (DFM) for CNC milling means shaping a part so that a round, rigid cutter can reach every feature in few setups, with tight tolerances only where the function needs them. The rules below cover inside corner radius, pocket depth, wall thickness, holes, threads, setups and tolerances, each with the reason behind it and its effect on cost.
What does DFM mean for CNC milling?
A milling machine removes material with a rotating cylindrical cutter that approaches along the spindle axis. Three facts follow from that, and every rule in this article comes from one of them. The cutter is round, so inside corners are round. The cutter has a finite length and bends under load, so deep and narrow features force slow cutting or special tools. The part has to be clamped, so every face the cutter cannot reach needs another setup.
Cost follows the same three facts: more machining time when the cutter must run light, more setups, more tooling and more inspection. This article describes cost effects in words, because their size depends on part, material and shop.
Unless a line says "calculation", the numbers below are guideline values from the design guides of Hubs and Protolabs, two CNC manufacturing services. They are not values from a standard, and a shop with different machines will draw its limits elsewhere. Read them as the point beyond which quoting becomes harder, not as the limit of any particular shop. Our audited network in Bursa covers CNC milling.
Which inside corner radius should you specify?
Rule 1: no sharp inside corners. Hubs recommends a vertical corner radius of at least one third of the pocket depth. It prefers a radius slightly above that value, for example by 1 mm, because the cutter then follows a circular path instead of a 90° turn and leaves a better surface finish. Protolabs states the same from the shop side: sharp inside corners are radiused by the process, and the resulting radius is the minimum tool radius.
The radius sets the largest cutter that can finish the corner, which is twice the radius at most. A smaller cutter at the same reach is far less stiff. For a cantilever with an end load, tip deflection is δ = F·L³ / (3·E·I), and for a solid round cutter I = π·d⁴ / 64. At a fixed reach L, deflection therefore scales with 1/d⁴.
Table 1. Corner radius, largest cutter and relative deflection, pocket 30 mm deep
| Corner radius R, mm | Largest cutter Ø (2 × R), mm | Depth ÷ cutter Ø | Relative deflection at equal force |
|---|---|---|---|
| 10 (⅓ of depth) | 20 | 1.5 | 1 |
| 6 | 12 | 2.5 | 7.7 |
| 3 | 6 | 5 | 123 |
| 1.5 | 3 | 10 | 1,975 |
Source: Ertaş Engineering calculation from δ ∝ L³/d⁴ with L = 30 mm (cantilever formula, Wikipedia; overhang rule, Mitsubishi Materials). Solid round tool, flutes and tool holder ignored. Hubs calls a cavity deep when its depth exceeds six times the tool diameter.
A shop makes up for the lost stiffness with light engagement, more passes and lower feed, so machining time on that corner rises. The cheapest fix sits on the drawing: a larger radius, or a shallower pocket. If a mating part needs a square corner, relieve the mating edge with a chamfer or radius rather than asking for a sharp corner in the pocket.
Rule 2: floor radius of 0.5 mm, 1 mm or none. Hubs lists these as the recommended values. Other floor radii can be machined with ball-end tools, which means another tool and another pass.
How deep can a milled pocket be?
Rule 3: keep the pocket depth at or below four times its width. Hubs gives this as the recommended value, and Protolabs gives the same figure for the cavity depth. Hubs calls a cavity deep when its depth exceeds six times the tool diameter, and says ratios up to 30:1 are possible with specialised tooling.
The reason is overhang. Mitsubishi Materials states that deflection is proportional to the cube of the overhang: with the same diameter, doubling the overhang gives eight times the deflection. A pocket 40 mm deep needs a cutter that reaches at least 40 mm out of the holder, however wide the pocket is.
Options when a pocket is too deep: widen it, split the part into two pieces that are joined afterwards, or move the pocket so that it is machined from the opposite face at a shallower depth.
How thin can a wall be?
Rule 4: make metal walls at least 0.8 mm thick. Hubs recommends 0.8 mm for metals and lists 0.5 mm as the minimum feasible value. Protolabs advises not to go below 0.5 mm and adds that thicker is better, since thin walls are less stiff and more prone to vibration.
A thin wall moves away from the cutter during the cut, so its finished thickness is hard to hold. If the wall carries a tolerance, the cost shows up as slow finishing passes and more rejected parts, not as extra material.
What limits apply to holes and threads?
Rule 5: hole depth of 4 × diameter. Hubs recommends a hole depth of 4 times the nominal diameter, lists 10 times as typical and 40 times as feasible. Holes deeper than the typical value need specialised drills, with a minimum diameter of 3 mm. Protolabs says holes much more than six diameters deep become a challenge. For accurate holes below 20 mm diameter, Hubs recommends standard drill sizes.
Rule 6: threads M6 or larger, length 3 × diameter. Hubs recommends M6 or larger: CNC threading tools cut threads down to M6 and machinists prefer them because they limit the risk of tap breakage, while taps and dies go down to M2. Hubs gives a minimum thread length of 1.5 times the nominal diameter and a recommended length of 3 times. It points out that most of the load on a thread is carried by the first teeth, up to 1.5 times the nominal diameter.
How do setups, tolerances and surface finish drive cost?
Rule 7: keep features on few faces. Protolabs describes 3-axis milling as cutting a part from up to six orthogonal sides. Hubs says rotating the part up to three or four times is often acceptable and anything above that is excessive. Each rotation is a new clamping with its own datum, so a position tolerance between features on two faces is harder to hold than one within a single face. Hubs lists 5-axis machining as a way to avoid multiple setups.
Rule 8: use the general tolerance and add individual tolerances only where function needs them. Our network works to ISO 2768-m as standard. For a 50 mm length, class m of ISO 2768-1 allows ±0.3 mm (range over 30 to 120 mm). A tolerance tighter than that on a feature calls for a light finishing pass and a measurement of that feature, so reserve it for bearing seats, sealing faces and locating features. ISO 2768-1:1989 is still the general tolerance standard for linear and angular sizes, and a revision project is listed. ISO 2768-2 was withdrawn in February 2021, see the ISO 2768 article. Geometrical tolerances follow ISO 1101:2017, confirmed in 2022, and fits follow ISO 286-1:2010, confirmed in 2026.
Rule 9: state roughness only where it matters. Surface texture on drawings is indicated to ISO 21920-1:2021, which replaced ISO 1302:2002. As of November 2026 ISO lists ISO 21920-1 as under revision, with a committee draft in progress, so check the edition on your drawing template. A roughness requirement on every face makes the finishing pass the default for the whole part. See Ra and Rz for the parameters.
Which DFM rules should you check before the drawing goes out?
Table 2. Guideline values for CNC milled metal parts and the cost effect of ignoring them
| Feature | Guideline value | Why | Effect on cost if ignored |
|---|---|---|---|
| Inside corner radius | ≥ ⅓ × pocket depth, slightly more preferred | Round cutter, small cutters bend | Light cuts, more passes |
| Floor radius | 0.5 mm, 1 mm or none | Standard cutters | Ball-end tool, extra pass |
| Pocket depth | ≤ 4 × width | Cutter overhang | Slow cutting, special tooling |
| Wall thickness, metal | ≥ 0.8 mm (0.5 mm feasible) | Stiffness | Slow finishing, scrap risk |
| Hole depth | ≤ 4 × diameter (10 × typical) | Drill length | Special drills, both sides |
| Thread | M6 or larger, length 3 × diameter | Thread tools | Tapping or another process |
| Setups | Up to 3–4 rotations | Clamping and datums | Handling time, position error |
| General tolerance | ISO 2768-m | Default finishing | Extra passes and inspection |
Source: Hubs design guide (corner radius, floor radius, cavity depth, wall, hole, thread, setups); Protolabs design guidelines (inside corners, hole depth, 3-axis sides); ISO 2768-1:1989. Cost column: Ertaş Engineering assessment.
Before a drawing goes out for quotation, go through three questions. Does any feature need a cutter smaller than the pocket depth suggests? Can a deep or thin feature be shortened, widened or thickened without changing function? Does every tolerance and roughness value sit on a feature that needs it? The technical drawing checklist covers the title block and format. DFM support is part of our design engineering service.
Frequently asked questions
- What is the smallest inside corner radius in CNC milling?
- It equals the radius of the cutter that finishes the corner, so there are no sharp inside corners. Hubs recommends a corner radius of at least one third of the pocket depth, and slightly more where possible, for example 1 mm more, so the cutter follows a circular path.
- How deep can a CNC milled pocket be?
- Hubs recommends a depth of up to four times the pocket width. It calls a cavity deep when the depth exceeds six times the tool diameter, and says ratios up to 30:1 are possible with specialised tooling.
- What is the minimum wall thickness for milled metal parts?
- Hubs recommends 0.8 mm for metals and lists 0.5 mm as the minimum feasible value. Protolabs advises not to go below 0.5 mm, because thinner walls are less stiff and vibrate under the cutter.
- Why do tighter tolerances make a milled part more expensive?
- A tight tolerance on a feature needs lighter finishing passes and more measurement than a feature held to the general tolerance. Specify ISO 2768-m for the whole drawing and add individual tolerances only on features that need them.
- How many setups are acceptable for a milled part?
- Hubs says rotating a part up to three or four times is often acceptable and anything above that is excessive. A 3-axis machine can reach up to six orthogonal sides, and each side needs its own clamping.
Sources
- Hubs, How to design parts for CNC machining (corner radius, cavity depth, walls, holes, threads, setups)
- Protolabs, Design guidelines for CNC milling (inside corners)
- Protolabs, 6 ways to optimize part design for CNC machining (hole depth, 3-axis sides)
- Protolabs, CNC machining design (wall thickness, tool access)
- Mitsubishi Materials, Flute length and overhang (deflection grows with the cube of overhang)
- Deflection (engineering), cantilever with end load: δ = FL³/(3EI) (Wikipedia)
- List of second moments of area, filled circle: πr⁴/4 = πd⁴/64 (Wikipedia)
- ISO 2768-1:1989, life cycle: published 1989-11-02, stage 90.92 since 2022-10-04, revision project listed (ISS, national ISO member)
- ISO 2768-1 linear tolerances, class m, over 30 to 120 mm: ±0.3 mm (AmesWeb table)
- ISO 2768-2:1989, life cycle: withdrawn 2021-02-04 (ISS, national ISO member)
- ISO 1101:2017, life cycle: confirmed 2022-10-03 (ISS, national ISO member)
- ISO 286-1:2010, life cycle: confirmed 2026-06-19 (ISS, national ISO member)
- ISO 21920-1:2021, life cycle: published 2021-12-20, previously ISO 1302:2002, stage 90.92 (to be revised) since 2025-10-07 (ISS, national ISO member)
- ISO 21920-1:2021, scope and replaced standard (AFNOR)
Questions on a drawing? sales@ertas.engineering