Home / Guides / Design

Wall thickness, pocket depth and corner radius: the three numbers that price your part

August 18, 2026

If you only have ten minutes to make a machined part cheaper, spend them on three numbers: how thin the walls are, how deep the pockets are and how tight the internal corners are. Everything else on a normal part is secondary.

Wall thickness

A thin wall does not fail because the machine cannot cut it. It fails because it moves. Cutting forces push the wall away from the tool, it springs back after the cut and the dimension you measure is not the dimension the machine commanded.

Practical starting points:

Material	Comfortable	Possible with care
Aluminium	1.0 mm	0.5 mm
Steel and stainless	0.8 mm	0.4 mm
POM and nylon	1.5 mm	1.0 mm
PEEK	1.2 mm	0.8 mm

Plastics are on the thicker side of that table because they are softer and because heat builds up in the cut.

Two design moves buy a lot: add a small rib to stiffen a long thin wall, and avoid having a thin wall stand alone at full height. If the wall exists only to close a cavity, ask whether a cover plate would be cheaper than machining it in one piece.

Pocket depth

The limit is the ratio between depth and the diameter of the tool that has to reach the bottom.

• Up to 3 times tool diameter: normal, full speed
• 3 to 5 times: manageable, lighter passes
• 5 to 8 times: slow, and finish quality drops in the corners
• Beyond 8 times: specialist tooling, higher price, often a different quote altogether

The trap is that the tool diameter is set by your smallest corner radius, not by the pocket width. A 60 mm wide pocket with 2 mm corner radii has to be finished with a 4 mm cutter, so a 25 mm deep pocket is suddenly at six times diameter in the corners.

If the pocket is a weight reduction feature, open the corners up and the problem disappears.

Corner radius

Every internal vertical corner in a milled pocket has a radius. Your drawing can only choose which one.

Design rule that works: make the corner radius at least one third of the pocket depth, and keep one radius across the whole part.

Why one radius matters: each different radius is a different tool, a tool change, and sometimes a separate finishing pass. Three radii on a part is three times the finishing setup for no functional gain in most designs.

On floor corners, where the wall meets the bottom of the pocket, a sharp corner requires a square end mill and leaves a stress riser. A small floor radius from a bull nose cutter is stronger and faster. If your drawing shows a sharp floor corner, check whether it is functional.

The undercut question

Anything that cannot be reached from the direction the tool comes from is an undercut. Common examples are O-ring grooves inside a bore, snap features and re-entrant slots.

Undercuts are not impossible. There are T-slot cutters, lollipop cutters and dovetail cutters, and for internal grooves there are specialised tools. All of them mean another tool, another operation and a lower feed rate. Before you specify one, ask whether the part could split into two pieces that are each simple to machine, especially at low quantity where assembly labour is cheap compared with machine time.

A quick self check on your own model

1. Find the smallest internal corner radius. Multiply it by two. That is your smallest finishing tool.
2. Find the deepest pocket that has that radius. Divide the depth by the tool diameter. Over five, expect a premium.
3. Find the thinnest wall. Compare it with the table above.
4. Count the distinct corner radii. More than two on a simple part is usually accidental.
5. Look for anything the tool cannot see from the top or the bottom.

If all five are comfortable, your part will quote well anywhere. If two of them are not, that is exactly what to raise in your request, because a shop can often suggest a change that costs you nothing and saves real time.

What to do when the limits are in the way

Four moves that solve most thin wall and deep pocket problems without changing what the part does.

Add a sacrificial rib or tab. A small rib stiffens a thin wall during machining and is removed in a final light pass. Shops do this routinely, and saying you are open to it invites the suggestion.

Split the depth across two features. A deep narrow slot can sometimes become a shallow slot plus a through hole, which is two easy operations instead of one hard one.

Change the corner radius only where the tool has to reach deep. Corners near the top of the pocket can stay tight. It is the ones at full depth that set the tool.

Move the feature to the other side. Machining a pocket 20 mm deep from one side may be a 40 mm reach from the other. Which face the shop clamps is often negotiable, and it is worth asking.

Fixturing, the constraint nobody draws

A part has to be held. On thin or odd shaped parts, how it is held decides whether the tolerances are real:

• Leave clamping material where you can, especially on plates that will be finished on both sides
• Say which surfaces are cosmetic, so the shop knows where it must not leave clamp marks
• Expect soft jaws or a vacuum plate on thin parts, and accept that these add setup time on small orders
• Ask how the part will be held if you have a tolerance below ±0.02 mm on a flexible part. The answer tells you whether the shop has made this kind of part before

More of the same thinking is in the DFM checklist, and when your model is settled you can send it for quotes.

Questions we get on this

Keep reading

• What a DFM review actually changes, with the numbers
• Twelve design changes that take real money out of a machined part