Design for CNC milling starts with one fact: end mills are round, so every inside corner, deep pocket, and thin wall carries a limit that the drawing should respect. This guide covers the three features that most often decide whether a milled part cuts cleanly or comes back for redesign: corner radii, pocket depth, and wall thickness. FM Machine Co. in Akron, Ohio wrote it for engineers who want fewer quote revisions and fewer surprises after the first part is cut.
Milling tools are cylindrical, so pocket corners always keep an internal radius. Most of the guidance below follows from that. The same thinking applies to lathe work, which the design for CNC turning guide covers.
Why do internal corners need a radius on a milled part?
A rotating cutter cannot make a square inside corner. The smallest radius a shop can cut in a corner is set by the cutter’s own radius, and a smaller cutter means a longer, thinner tool that bends under load. That is why a drawing with tight inside radii often gets a call from the shop: the only way to cut it is slowly, with a small tool that is prone to chatter and breakage.
Published design guides commonly suggest an inside corner radius of about one third of the pocket depth, with larger radii preferred, and the same radius on every inside corner where the function allows. A consistent radius lets the shop run one cutter through the pocket instead of changing tools. A radius slightly larger than the cutter radius also helps, because the tool keeps moving through the corner instead of dwelling in it.
When a sharp corner is a true requirement, such as a rectangular part that must seat in a pocket, a relief cut in the corner usually costs less than shrinking the radius. Whatever the choice, call out every inside radius on the drawing. A corner left undimensioned forces the shop to guess, and the guess may not match how the part assembles.
At the pocket floor, the edge between the floor and the wall is usually cut with a small radius or none. A large floor radius adds a ball-nose pass and extra time, so keep it only where the function needs it.
How deep can a pocket be before it causes trouble?
Pocket depth matters because depth means reach. The deeper the pocket, the longer the tool must stick out of the holder, and a long tool deflects, vibrates, and leaves a poorer finish on the walls. Chips are the second problem. In a deep, narrow pocket they have nowhere to go, and a cutter that recuts packed chips loses edge life quickly. How well chips clear also depends on machine layout, which the horizontal vs. vertical machining center guide explains.
Design guides often suggest keeping cavity depth to no more than about four times the cavity width. Past that point the shop can still cut the pocket, but the time and tool cost rise. If a design needs a deeper cavity, the options are a wider pocket, a shallower floor, stiffening ribs, or splitting the part so each piece has easier access.
Blind pockets are harder than through openings because chips have no exit and coolant cannot flush them out the far side. If the function allows an open or through design, the shop can cut it faster and with less risk to the tool.
How thin can a wall be and still hold tolerance?
Wall thickness limits are about stiffness, not just thickness. A thin wall flexes away from the cutter, which shows up as a tapered wall, a rough finish, or a wall that springs back after release and ends up out of tolerance. Height matters as much as thickness: a short wall of a given thickness behaves very differently from a tall one. A wall tied to ribs or curved geometry holds up better than a free-standing wall of the same height.
Published minimums vary by source, by material, and by wall height, so a single number does not transfer between parts. Ask the shop for a limit on your material and your wall height before the design is final. Tolerance and finish compound the problem, since a tight callout on a flexible wall adds light finishing passes and inspection time. The Ra and Rz guide explains which finish callouts add cost and which ones the function needs.
Features the tool cannot reach need a different process or a split part
Some features cannot be cut from the open side of a pocket at all. Undercuts, deep narrow slots, and features on faces that sit behind other geometry all depend on tool access, and access depends on the machine as much as on the design. A published equipment list, such as the FM Machine Co. equipment list, shows the travel of each machine, which tells you whether a part’s reach requirement is realistic before you send the drawing.
When a feature fails the access test, the choice is usually among three moves: redesign the feature so the cutter can reach it, split the part into two pieces that join after machining, or accept an added setup or a different process at higher cost. Each option has a price, so the earlier the question comes up, the cheaper the answer.
Where a part must be machined from more than one side, each additional setup adds handling and a chance for position error between faces. Features that must align across faces should be located from the same datums, so the shop can hold them in one setup when possible.
A radius, depth, and wall check before quoting prevents redesign
A short review of these features before the drawing goes out catches most of the problems that cause quote revisions. The table below lists the feature, what goes wrong in the shop, and the change to make on the drawing.
| Feature | What goes wrong | What to change on the drawing |
|---|---|---|
| Sharp inside corner | The shop needs a tiny cutter or sends the part back | Add a radius larger than the cutter radius, or add a relief at the corner |
| Deep, narrow pocket | A long tool deflects and chatters, and chips pack in the cavity | Widen the pocket, reduce the depth, or split the part |
| Tall, thin wall | The wall flexes during cutting and moves after release | Thicken or support the wall, and relax tolerance on it |
| Mixed inside radii | More tool changes and a longer cycle | Use one radius on inside corners where the function allows |
| Feature behind other geometry | The cutter cannot reach it without an extra setup or another process | Redesign for access, or split the part |
None of these changes loosens the function of the part. They give the cutter a path it can follow.
What should the drawing show for milled features?
A drawing that states the radius, depth, and wall dimensions clearly lets the shop quote the cut instead of interpreting it. These are the items that make the biggest difference:
- Every inside corner radius, with one radius used wherever the function allows
- Pocket depth and width, dimensioned so the ratio is visible
- Wall height and thickness for any thin or free-standing wall
- Datums that locate features on each face, so the shop can plan setups around the relationships that matter
- Finish callouts only on surfaces where the function needs them
- Material and quantity, since both change how the shop approaches the cut
Send the drawing with those details and request a quote through the quote form. The precision CNC machining services page lists the milling processes FM Machine Co. offers.