Why pockets, walls and undercuts decide manufacturability
Most CNC milling time on prismatic parts is spent clearing pockets and finishing walls. Geometry that looks fine in CAD—deep cavities, paper-thin ribs, hidden undercuts—can multiply setups, force tiny cutters or make a feature impossible without EDM. This checklist-style guide covers the design rules that keep pockets, thin walls and undercuts manufacturable on ordinary 3-axis and 5-axis mills.
Pockets: start from the cutter
A pocket is an internal cavity cut by an end mill. The tool is a rotating cylinder (or a ball/bull-nose variant), so every internal vertical corner inherits a radius no smaller than the tool radius. Sharp internal corners in the solid model are not free; they imply a tiny tool, slow cycle time or a secondary process.
Corner radius
- Make internal corner radii larger than the planned tool radius when you can; slightly oversized radii cut faster and leave a better finish
- Avoid "sharp" internal corners unless function truly requires them (for example a square insert seat), and then expect EDM, broaching or a very small tool
- Outside corners can be sharp; that is easy for an end mill
Pocket depth versus tool diameter
A practical comfort zone for many materials is a depth of roughly three to four times the tool diameter for efficient roughing, with finishing passes afterward. Deeper pockets are possible but need longer tools, reduced feeds and more careful strategies. If a pocket is both deep and narrow, redesign: widen the opening, split the depth across sides or machine from opposite faces.
Floor and wall finish
Specify surface finish only where it matters. A pocket floor that never shows can stay at a standard machined finish. Walls that seal or guide need explicit callouts. Floor radii (fillets where the wall meets the floor) should match a realistic tool corner radius; a zero floor fillet forces a sharp corner tool or an extra pass.
Thin walls: stiffness rules the cut
Thin walls deflect under cutting forces. Deflection causes chatter, taper, stepped walls and scrap—especially in aluminum with tall ribs and in titanium or plastics with low stiffness relative to the cut.
Starting thickness guidelines
Exact limits depend on material, height, support and tooling, but useful design habits are:
| Situation | Design habit |
|---|---|
| Short ribs in aluminum | Keep thickness comfortable relative to height; avoid foil-like sections |
| Tall unsupported walls | Thicken, add ribs, or machine alternately from both sides |
| Matching thin walls on both sides of a pocket | Leave stock and finish in a balanced sequence; avoid hitting final thickness in one heavy pass |
| Plastic thin walls | Be more conservative; heat and clamping distort easily |
If weight is the goal, lighten with patterned pockets and consistent wall thickness rather than one heroic membrane.
Height-to-thickness thinking
As a mental model, treat a wall like a cantilever. Doubling height without increasing thickness multiplies flexibility. When a wall must be tall and thin for function, add gussets, shorten spans between supports or allow the shop to leave sacrificial ribs until final finishing.
Cosmetic thin walls
Anodized or painted thin edges chip and look uneven. If cosmetics matter, thicken visible edges slightly or break sharp edges with a consistent chamfer or radius.
Undercuts: when the tool cannot see the feature
An undercut is a feature that is hidden from the spindle direction of a given setup— for example a groove on the far side of a wall, a T-slot, or a side pocket shadowed by an overhang. 3-axis mills need a clear line of sight along Z for standard end mills. Undercuts need one of:
- A second setup (flip or re-clamp the part)
- A 5-axis tilt to bring the feature into view
- Special tooling (lollipop cutters, keyseat cutters, custom form tools)
- A separate process such as wire EDM or sinker EDM
Design out undercuts when you can
Ask whether the undercut is required for function or only inherited from a cast/molded mindset. Many undercuts on machined parts can become open slots, through features or assemblies of two simpler parts.
When undercuts stay
- Provide clear access dimensions and state the functional need
- Prefer standard groove widths that match common cutter widths
- Avoid deep, blind undercuts with tiny openings
- Consider splitting the part on the undercut plane and fastening or bonding afterward
Multi-setup and 5-axis effects
Features on opposite faces need either two setups or a 5-axis strategy. Each re-clamp stacks location error between features. If a bore on one face must align tightly with a pocket on another, machine them in one clamping when possible or establish clear datums and inspection plans.
5-axis positioning helps reach angled ports and reduces setups for housings, but it does not remove the need for corner radii and sensible wall thickness. It also does not make a true undercut free if the tool still cannot fit.
Checklist before you release the model
Pocket checklist
- Internal corner radii ≥ planned tool radius (and preferably larger)
- Depth-to-width ratio is not extreme without a process note
- Floor fillets match a real tool
- Non-functional floors are not held to cosmetic finishes
Thin-wall checklist
- Wall thickness is consistent with height and material
- Unsupported spans are broken up or gusseted
- Cosmetic edges are slightly forgiving
- Plastics and titanium get extra conservatism
Undercut checklist
- Every undercut has a reason
- Access exists for a standard or named special tool
- Alternative: two-piece design or EDM is acknowledged on the drawing notes if required
Drawing and model hygiene
- Contiguous solids without accidental micro-gaps
- Hole and pocket bottoms modeled as they should be machined (not cartoon sharp)
- Tolerances on walls that can flex are realistic
- Stock size and primary datums are obvious
Interaction with finishing
Anodizing, plating and powder coat add thickness and can bridge fine details. Thin walls and tight pockets change dimensionally after coating. Call out whether dimensions apply before or after finish, and mask threads and precision bores as needed. Deep narrow pockets are harder to coat uniformly; design open enough for the finish process when cosmetics or corrosion protection matter inside the cavity.
Common mistakes
- Modeling sharp internal corners "to clean up later" and never cleaning them up
- Specifying 0.5 mm walls 30 mm tall in aluminum for weight without a machining plan
- Leaving T-slots or hidden grooves with no tool access story
- Stacking ±0.02 mm on a flexible thin wall
- Forgetting that a pretty rendered fillet of R0.1 mm implies a Ø0.2 mm tool
- Designing pockets that trap chips with no exit path in deep cavities
A quick redesign pattern
When a part fails the checks above, try this sequence:
1. Enlarge internal radii and open the pocket mouth
2. Thicken or gusset the thinnest tall walls
3. Convert undercuts to through features or split parts
4. Move tight tolerances to stiff datums
5. Only then escalate to 5-axis, EDM or exotic tooling
That order usually recovers schedule and cost before special processes are needed.
Next steps
Upload the model and highlight any walls or cavities that must stay thin or undercut for function. The reviewing engineer can suggest radius and thickness changes, flag features that need a second setup or 5-axis reach, and note where a blank-plus-machine or two-piece design would be cleaner.
Materials change the same rules
Aluminum forgives thin walls better than titanium or many plastics because it cuts cool and stiffens reasonably for its density. Stainless and titanium push you toward thicker sections and more open pockets. Soft plastics need gentle cuts and often temporary support. Apply the same checklist, then tighten or relax wall and depth choices for the alloy on the title block.
If you are migrating a cast or molded design to CNC, expect to thicken walls, add draft removal (machined parts do not need draft), enlarge radii and eliminate molding undercuts. A cast-looking model milled from billet is a common source of slow quotes.