CNC Machining Design Guidelines: DFM Rules with Real Numbers

Wall thickness and tall features

Thin walls are the most common source of chatter, deflection and scrap. The cutting force pushes the wall away, so the finished dimension and surface finish suffer. Recommended values are:

These values assume a low height-to-thickness ratio. As a wall gets taller relative to its thickness (roughly above 3:1), increase the thickness or add supporting ribs, because a tall, thin wall behaves like a cantilever and flexes. Keep wall thickness as uniform as possible to avoid uneven material removal.

Holes and pockets

• Use standard hole diameters. Holes that match standard drill and reamer sizes are cheaper than sizes that need boring or end-milling to a non-standard number.
• Limit depth to about 4× diameter. Within this ratio holes and pockets are reliable; deeper features need long tools, pecking and slower feeds. Deep holes up to around 10:1 are possible with the right equipment but should be flagged in DFM review.
• Design flat-bottomed pockets carefully. Drills leave a conical bottom; a flat bottom requires an end mill. Keep pocket depth within about 4× the tool diameter and leave internal corner radii (see below).
• Provide a starting surface and avoid holes that meet at sharp angles inside the part, where tool engagement becomes unstable.

Internal corners and radii

Because cutting tools are cylindrical, internal corners always retain a radius equal to at least the tool radius. Designing a sharp internal corner forces a secondary operation such as sinker EDM or broaching. Practical guidance:

• Give internal corners a radius that matches a standard tool, commonly R3–R6 for general pockets, and keep radii consistent.
• A larger radius allows a larger, stiffer tool, which cuts faster with less deflection; a good target is a radius around one-eighth to one-quarter of the pocket depth.
• External edges can be sharp (they are easy to produce) but a small break-edge or chamfer removes burrs and is safer to handle.

Threads

• Specify standard threads — metric such as M6×1.0 or imperial such as 1/4-20 UNC — with the class (e.g. 6H) and depth. Non-standard or custom threads are expensive.
• Don't thread to the bottom of a blind hole. A tap cannot produce a full thread to the very end; allow about half a diameter of unthreaded length plus a drill point. A practical tapped depth is within about 3× the thread diameter.
• For very small or delicate threads, consider a threaded insert (e.g. helicoil) in soft aluminium and plastics to improve durability.

Tolerance and surface finish

Tolerance is a cost dial. A common default is around ±0.125 mm (±0.005 in) for non-critical features, or a general standard such as ISO 2768-mK. Holding features tighter than about ±0.025 mm requires slower feeds, specialist tooling and temperature-controlled inspection, which can add 20–50% or more. Apply tight tolerances only to features that actually mate, seal or locate, and use GD&T (flatness, perpendicularity, true position) where the relationship between features matters. Similarly, don't over-specify surface finish: Ra 3.2 suits structural faces, Ra 1.6 common mating faces, and Ra 0.8 or finer for sealing and bearing surfaces. See our full tolerance and finish guide.

Undercuts, draft and machine access

• Avoid internal undercuts where possible; they need special tools or separate setups. If an undercut is essential, dimension it clearly so a standard slot or dovetail tool can reach it.
• Think in setups. Every re-clamping adds time and stacks alignment error. Design the part so the most features can be reached from as few sides as possible; multi-sided complex parts are often best done in one 5-axis setup.
• Raised or recessed text should be at least about 0.5 mm deep/high and use a bold, simple font; raised text is usually preferred because it removes less material.
• Choose the material and finish for function — aluminium and brass machine quickly and cheaply; reserve harder alloys and premium finishes for where they earn their cost.

DFM checklist before you request a quote

• Walls at/above recommended thickness, uniform and with ribs if tall.
• Standard hole sizes; depths within ~4× diameter; flat-bottomed pockets noted.
• Internal corner radii provided; no sharp internal corners.
• Standard threads with class and depth; clearance at blind-hole bottoms.
• Tight tolerances and fine finishes only on functional features.
• Undercuts avoided or clearly dimensioned; minimal setups.
• 3D model (STEP/IGES) plus 2D drawing with callouts, material and quantity.

We run a DFM review on every enquiry and flag anything that adds cost or risk before production, so you can adjust the design early. Upload your model for a free review and a quote within 24 hours.

Frequently asked questions

What is the minimum wall thickness for CNC machining?

For metals about 0.5 mm minimum, 0.8 mm recommended; for plastics about 1.0 mm minimum, 1.5 mm recommended. Thin walls vibrate and deflect, causing chatter and scrap.

What is the standard CNC tolerance?

A common default is about ±0.125 mm, or ISO 2768-mK. Tighter than ±0.025 mm raises cost, so call it out only on functional features.

How deep can a machined hole or pocket be?

Keep within about 4× diameter for reliable results; deeper features need special tooling. Around 10:1 is possible with suitable equipment.