CNC machining cost is mostly machine time and setups, and design decides both. Generous internal corner radii, pockets no deeper than a few cutter diameters, walls thick enough not to chatter, standard hole and thread sizes, and tight tolerances only where they matter are the rules that keep a milled part cheap. Each one lets the shop use larger, faster tools and fewer setups.
Key points
- Internal vertical corners always have a radius. Make it as large as the part allows, ideally about a third of the pocket depth or more.
- Keep pockets to about three or four cutter diameters deep. Deeper means slow, long-reach tools.
- Thin walls vibrate and deflect. Keep them above roughly 0.8 mm in metal and about 1.5 mm in plastic.
- Use standard drill and thread sizes, and limit thread depth to what the joint needs.
- Put a general tolerance on the drawing and tight tolerances only on functional features.
- Every extra side the part must be machined from is another setup, and setups cost real time.
Why design decides machining cost
A milled part is priced from three things: the stock it is cut from, the machine time to cut it, and the setups to hold it. The CNC machining cost guide explains each. Design touches all three, but machine time and setups most.
Machine time is about tools. A large cutter removes material fast and stays rigid. A small one removes little per pass and must move slowly. Most design rules for CNC milling are really ways of letting the shop use bigger tools for longer. That is what design for manufacturing means in machining.
Design rules at a glance
The values below are common rules of thumb, not limits. A capable shop can go beyond each of them, at a price.
| Feature | Rule of thumb | What breaking it costs |
|---|---|---|
| Internal vertical corners | Radius at least about one third of the cavity depth, and a little larger than the cutter radius | Smaller, slower tools and extra finishing passes |
| Pocket depth | Up to about 3-4 × the cutter diameter | Long-reach tools, slow feeds, chatter risk |
| Wall thickness | Metal above about 0.8 mm, plastic above about 1.5 mm | Light cuts, vibration, scrapped parts |
| Hole diameter | Standard drill sizes | A drill becomes a milled hole or a special tool |
| Hole depth | Up to about 4 × diameter is routine; around 10 × is feasible | Peck drilling, special drills, run-out |
| Thread engagement | About 1.5 × the nominal diameter for most joints | Time spent tapping thread that carries no load |
| Undercuts | Standard T-slot or dovetail cutter sizes, or avoid | Special cutters, extra setups |
| Floor-to-wall corners | Fillet radius matching a standard ball or bull-nose cutter, or a sharp edge | Ball-nose finishing passes |
| Tolerances | General tolerance everywhere; tight only on functional features | Slow passes, extra inspection, rejects |
| Text | Engraved rather than embossed, in a simple font | Embossed text means machining away everything around it |
Internal corners: why every pocket has a radius
An end mill is round, so every internal vertical corner it cuts has a radius at least as large as the cutter’s. Drawing a sharp internal corner does not make one; it makes the shop ask, or pick a tiny tool.
Two rules help:
- Make the corner radius slightly larger than the cutter radius. If the corner radius equals the cutter radius exactly, the tool wraps around the corner, engagement spikes and it chatters. A little extra radius lets the tool arc through the corner smoothly.
- Scale the radius with depth. A common guide is at least a third of the pocket depth, because a cutter that reaches deep must have a matching diameter to stay rigid.
If a mating part really needs a square corner, use a relief in the corner (sometimes called a dog-bone) or, for a truly sharp corner, a process such as EDM. On the edges between floor and wall, a fillet is optional: a sharp floor edge is cheap with a flat end mill, and a fillet is cheap only when it matches a standard cutter.
Pockets, walls and floors
Deep, narrow pockets are slow. The tool must be long enough to reach, a long tool bends, and a bending tool must take light cuts. Keep pocket depth to a few cutter diameters, open pockets to one side where you can, and make the narrowest part of the pocket wide enough for a rigid tool.
Thin walls and thin floors vibrate as they are cut, which leaves chatter marks and makes dimensions drift. The shop compensates with light passes and support, which is time. Taller walls need to be thicker; the minimum wall thickness guide compares machining with other processes.
Holes and threads
Use standard drill sizes wherever a hole does not need a precise fit, and standard reamer sizes where it does. A non-standard diameter becomes a milled hole, which is slower. Through holes are easier than blind holes; a blind hole made with a drill has a conical bottom, so specify a flat bottom only when it is needed.
For threads, use standard sizes and specify the thread length the joint needs. Beyond about 1.5 times the diameter, extra engagement adds little strength in most metals. Leave a little unthreaded depth at the bottom of a blind hole so the tap does not bottom out and break.
Tolerances and finish
Tight tolerances are the most expensive thing on a drawing that costs nothing to write. A general tolerance class covers most features; tighter values belong only on fits, locating faces and sealing surfaces. Use GD&T where the relationship between features matters more than any single size. The tolerances and cost guide shows how cost climbs as the band narrows.
The same goes for surface roughness. A standard as-machined finish is usually fine for non-functional faces. Specify a finer finish only where a seal, a bearing or the look demands it.
Setups and accessibility
Every face that needs machining from a new direction is another setup: the part is unclamped, turned and re-fixtured, and its position re-found. Design features to be reached from as few directions as possible, and give the part a flat face or a parallel pair the shop can clamp. Workholding that is easy to design is cheap to run.
An undercut cannot be reached from above at all and needs a special cutter or another setup. When a part genuinely needs many directions, 5-axis machining may be cheaper than many 3-axis setups; see 3-axis vs 5-axis machining.
Worked example: checking a pocket and a thread
Worked example: applying the rules to one feature set. The rules are rules of thumb; the arithmetic is exact.
A housing has a pocket 60 × 40 mm, 24 mm deep, drawn with 3 mm internal corner radii, and four M6 tapped holes.
| Check | Calculation | Result |
|---|---|---|
| Recommended corner radius | 24 mm ÷ 3 | at least 8 mm |
| Cutter for the drawn 3 mm radius | Diameter below 2 × 3 mm | 5 mm cutter, for example |
| Reach of that cutter | 24 mm ÷ 5 mm | 4.8 diameters: long reach, slow |
| Cutter for an 8.5 mm radius | Diameter below 2 × 8.5 mm | 16 mm cutter |
| Reach of that cutter | 24 mm ÷ 16 mm | 1.5 diameters: rigid, fast |
| Useful M6 thread length | 1.5 × 6 mm | about 9 mm |
| Tap drill for M6 coarse | Standard size | 5.0 mm |
Changing the corner radius from 3 mm to 8.5 mm lets a 16 mm cutter clear the whole pocket, instead of a 5 mm cutter working near five diameters deep. If the 3 mm corner is needed for a mating part, a 16 mm cutter can rough the pocket and a small tool can finish only the corners.
Getting a design quoted
Send a STEP file with the drawing, so the shop gets exact geometry and units; the STL vs STEP vs 3MF guide explains why a mesh is a poor input for machining. The CNC milling technology page covers the process itself.
Quotometry prices CNC milling and turning today, and checks several of the rules above before it prices: internal radii against the smallest end mill, deep pockets and holes, undercuts and thin walls, read from a STEP model. A mesh upload carries no features, so it goes to the shop’s review.
Questions people ask
Why can't a CNC mill make a sharp internal corner?
Because the cutter is round. An end mill leaves a radius equal to its own radius in every internal vertical corner. Smaller radii need smaller tools, which cut slower and reach less deep. A truly sharp internal corner needs a different process, such as EDM, or a relief cut into the corner. Design the largest radius the part allows.
How deep can a CNC pocket be?
As a common rule of thumb, pockets up to about three to four times the cutter diameter machine without special tooling. Deeper is possible with long-reach tools, but they deflect, chatter and must cut slowly, so cost rises quickly. If a deep pocket needs small corner radii as well, the cost rises faster still.
How long should a tapped thread be?
For most steel and aluminium parts, thread engagement of about 1.5 times the nominal diameter carries most of the load the fastener can take; much beyond about three times adds little strength and costs time. In a blind hole, drill a little deeper than the thread so the tap has room at the bottom.
What tolerance should I put on a CNC drawing?
Apply a general tolerance to the whole drawing, such as a class from ISO 2768, and specify tighter tolerances only on the features that need them: bores for bearings, locating faces, mating surfaces. Every tighter tolerance adds machining care and inspection, so a drawing full of tight numbers costs far more than one with tight numbers where they matter.
Quotometry prices every part from your own machines and rates, on your website, in seconds.