Plain-language guides to precision CNC manufacturing

Search

CNC Design Guidelines for Engineers

cnc design guidelines

Wondering whether your part will machine cleanly and affordably? These cnc design guidelines boil down to generous internal radii, walls of at least 0.8 mm in metal, shallow cavities and tolerances only where they matter.

Design item Typical guideline
Minimum wall thickness, metal 0.8 mm recommended (0.5 mm absolute minimum)
Minimum wall thickness, plastic 1.5 mm recommended (1 mm absolute minimum)
Internal corner radius At least one third of the cavity depth
Cavity depth No more than four times the cavity length
Thread length No more than three times the hole diameter
Default tolerance when none is given ±0.1 mm

The figures above come from the JLCCNC design guideline, last updated on Aug 20, 2025, and the Protolabs Network guide to cutting CNC costs. Shops set their own limits and figures can change, so check the source before you rely on them.

Why tool geometry drives every CNC design rule

CNC machining removes material from a solid block with rotating cutting tools. According to JLCCNC, standard tools such as end mills and drills have a cylindrical shank and a limited cutting length. Nearly every rule below follows from those two traits.

The Protolabs Network design guide sorts the restrictions into three groups:

  • Tool geometry: the cutter’s shape transfers to the part, so internal corners always have a radius, however small the tool.
  • Tool access: the cutter approaches from above, so features it cannot reach cannot be machined, with undercuts as the exception.
  • Tool reach: deep features need extended-reach tools, which increase chatter and lower the achievable accuracy.

The same guide points out that no industry-wide standards exist for CNC design. Treat every number in this guide as a starting point, then confirm it with the shop that will cut your part.

Your model becomes toolpaths before it becomes a part. If you want to see the instructions a machine runs, read g-code basics; for the programs that write them, see cam software for cnc. A Xometry Europe guide republished on Wevolver names HyperMill and Mastercam as CAM packages that generate efficient toolpaths and minimize setup changes.

Internal corners and radii

Because milling cutters are round, a perfectly sharp internal corner is not possible. JLCCNC explains that smaller corners need thinner tools, which means longer machining times, more fragile cutters and higher cost.

The usual rule is a corner radius of at least one third of the cavity depth. Yijin Solution gives a worked example: a 12 mm deep pocket needs at least a 4 mm radius, with R0.5 mm as the recommended minimum for any corner. The Protolabs Network cost guide goes slightly larger, advising 5 mm or more for a 12 mm deep cavity so an 8 mm tool can run at higher speeds.

When a drawing carries no corner instructions, JLCCNC machines internal corners from a depth-based formula: radius R = (H/10) + 0.5 and tool diameter D = H/5, in millimetres. A 30 mm deep cavity therefore gets R 3.5 mm and a 6 mm tool. The table shows how tool diameter sets the minimum radius in the same guide.

Tool diameter Minimum internal radius
⌀ 2.0 mm R 1.5 mm
⌀ 4.0 mm R 2.5 mm
⌀ 6.0 mm R 3.5 mm
⌀ 8.0 mm R 4.5 mm
⌀ 10.0 mm R 5.5 mm
⌀ 12.0 mm R 6.5 mm

The Protolabs Network cost guide adds three habits that keep cutters efficient:

  • Use the same radius on all internal edges to eliminate tool changes.
  • At the cavity floor, apply a small radius of 0.5 or 1 mm, or none.
  • Specify a corner radius slightly larger than the cutter radius to reduce tool load and cost.

If a mating part truly needs a square corner, add reliefs or undercuts to the cavity instead of shrinking the radius, as the Protolabs Network guide advises. JLCCNC notes that spark erosion with copper electrodes can produce sharp corners, but at higher cost. Because tool diameter sits behind every radius decision, read end mill selection next.

cnc design guidelines Part model
A seated person views a yellow three-dimensional model on a computer screen.

Wall thickness and cavity depth

Thin walls need multiple passes at low cutting depths, so they vibrate, deform and break easily, JLCCNC warns. Its recommendation is 0.8 mm for metal (absolute minimum 0.5 mm) and 1.5 mm for plastic (absolute minimum 1 mm). HLH Rapid explains that plastics need more material because they are more prone to warping from residual stresses and softening as temperature rises.

Other guides add useful limits:

  • RapidDirect treats a wall of 0.508 mm (0.020 in) or less as highly susceptible to breaking and suggests a height-to-thickness ratio of 3:1.
  • The same RapidDirect guide recommends a draft angle of 1 to 3 degrees on high walls to improve machinability.
  • The Xometry Europe guide on Wevolver says walls below the minimums may need specialized fixturing or reduced cutting speeds.

For a deeper treatment of the topic, read the cnc wall thickness guidelines. To see how cutting parameters change around fragile features, read speeds and feeds.

Cavities are limited by the cutter’s reach. JLCCNC says end mills work best when cutting depth is two to three times the tool diameter, so a 12 mm mill can safely make a cavity up to 25 mm deep. Cutting at five times the diameter or more brings tool deflection, difficult chip removal and tool breakage.

Published limits on overall cavity depth differ, as this list shows:

  • Protolabs Network: no more than four times the feature length, meaning the largest dimension in the XY plane.
  • JLCCNC: limit depth to five times the length (maximum size on the XY plane) to minimize cost.
  • Xometry Europe on Wevolver: keep depths within a 3:1 depth-to-width ratio.
  • RapidDirect: an absolute maximum of four times the tool diameter.

Where the figures disagree, the lowest one is the safest default until your shop confirms its own limit. If a cavity must go deeper, RapidDirect suggests redesigning the part as two pieces that bolt together.

Holes, threads and engraved text

Holes are cut with a drill bit or an end mill. HLH Rapid recommends standard diameters for high-accuracy holes under 20 mm, and says holes up to 10 times the diameter are possible but should be limited to four times the diameter. RapidDirect is stricter at 3:1 for standard holes and adds 25% to the depth of blind holes for chip accumulation.

For threads, JLCCNC recommends designing to standard major and minor diameters and describing the thread parameters fully in the order. Base-hole size matters: for M3×0.5 the standard base hole is ⌀ 2.5 mm, and a base hole drawn at ⌀ 3 mm is too large for tapping.

Thread length rules from three sources agree closely:

  • JLCCNC: keep thread length to no more than three times the hole diameter, and leave an unthreaded length of at least half the hole diameter at the end of a blind hole.
  • HLH Rapid: most thread load is taken by the first few teeth, up to 1.5 times the nominal diameter.
  • Yijin Solution: a thread depth of 2 to 3 times the thread diameter, because deeper threads add machining time and shorter ones risk insufficient pull-out strength.

For fuller coverage of drilling and tapping choices, read cnc thread and hole design.

Choose engraved over embossed text, because engraving removes less material. HLH Rapid recommends engraved details at least 0.8 mm deep and 0.5 mm wide, with a font height of at least 5 mm and a sans serif typeface.

cnc design guidelines Design workstation
A person works at two monitors displaying colorful technical models.

Tolerances, setups and drawings

Smaller tolerances cost more because they take longer to produce and inspect. JLCCNC applies ±0.1 mm when no tolerance is given and requires an annotated 2D drawing for anything else. Defaults differ by shop: HLH Rapid quotes ±0.05 mm for metals and ±0.2 mm for plastics, controlled to ISO 2768.

Yijin Solution lists precision tolerances of ±0.01 to 0.05 mm and warns that they need slower feeds, more passes and higher inspection cost. Reserve them for critical features. For the symbols that define those features, read gd&t basics.

Every extra setup adds time and positional error. Yijin Solution suggests keeping all features reachable within four setups or fewer and designing stable three-point datum surfaces so the part does not need a custom fixture. The Protolabs Network design guide recommends aligning holes, cavities and vertical walls to one of the six principal directions.

How the part is clamped follows from those datums, so cnc workholding is the natural companion topic.

HLH Rapid asks for a 2D technical drawing alongside the 3D model whenever the design includes any of these:

  • Threads
  • Tolerances
  • Surface finish specifications
  • Other notes

Surface finish also needs a number. Yijin Solution gives as-machined Ra 1.6 to 3.2 µm, with finish passes reaching Ra 0.4 to 0.8 µm.

What should you check before sending a design to a shop?

Machining time is often the primary cost driver, according to the Protolabs Network cost guide. Tight tolerances and hard-to-machine features such as very thin walls can add special tooling, stricter quality control and extra operations at lower cutting speeds. Material cost matters too, since raw price and machinability both influence the quote.

Run through this checklist before you release a drawing:

  1. Internal corner radii are at least one third of the cavity depth, with one radius reused wherever possible.
  2. Walls meet the metal or plastic minimum.
  3. Cavity depth stays within the strictest published ratio your shop accepts.
  4. Holes use standard sizes, and threads are short with standard base holes.
  5. Tight tolerances appear only on critical features.
  6. A 2D drawing carries the threads, tolerances and finish notes.

The Xometry Europe guide on Wevolver lists signs that a part is complex and needs extra planning:

  • Features smaller than 2.5 mm, which demand specialized tooling.
  • Large parts, typically over 1000 mm, which require specialized equipment.
  • Depth-to-width ratios greater than 3:1, which can cause tool deflection.

Several flags on one part is a cue to simplify it or break it into modular sections that are machined separately and assembled later, as the same guide suggests. HLH Rapid notes that CNC can cost more than other methods such as 3D printing. When no cutter can reach a feature, read 3d printing for manufacturing to see where additive methods fit. For the bigger picture of the process these rules belong to, read precision cnc machining.

cnc design guidelines Geometric model
A laptop on a desk displays an angular model against a blue background.

Frequently asked questions

What is the minimum wall thickness for CNC parts?

Show answer

Both JLCCNC and HLH Rapid recommend at least 0.8 mm for metals and 1.5 mm for plastics. JLCCNC lists absolute minimums of 0.5 mm for metal and 1 mm for plastic.

What internal corner radius should you use?

Show answer

Aim for a radius of at least one third of the cavity depth. Yijin Solution gives 4 mm for a 12 mm deep pocket, while the Protolabs Network cost guide suggests 5 mm or more for the same depth.

Why do shops publish different limits?

Show answer

The Protolabs Network design guide states that no industry-wide specific standards exist, and that machine and tool makers keep expanding what is possible. Cavity depth shows the spread, because the guides listed earlier each give a different ratio.

How long can a threaded hole be?

Show answer

Keep the thread to no more than three times the hole diameter, per JLCCNC. In a blind hole, leave an unthreaded length of at least half the hole diameter at the bottom.

What tolerance applies if a drawing does not specify one?

Show answer

JLCCNC makes parts to a standard tolerance of ±0.1 mm or higher, while HLH Rapid uses ±0.05 mm for metals and ±0.2 mm for plastics. Ask your shop for its default before you assume one.