Guides / Design

Designing a Part for 5-Axis: Undercuts, Tool Access and Fixturing

October 1, 2026

A 5-axis machine reaches more of the part than a 3-axis mill, but it does not reach everything. The tool still needs a straight path in, the holder must clear the part and the machine must hold the part somewhere. Designing with those three limits in mind is the fastest way to get a prototype that is quoted quickly and cut right the first time.

Think in lines of sight

Every surface the machine cuts must be visible from some direction along the tool axis. With 5-axis the machine can tilt to find that direction. Ask yourself, for each feature:

• Is there an angle from which a straight tool can see this surface?
• At that angle, does the tool holder hit a wall, a boss or the table?
• Is the reach short enough for a stiff tool?

If the answer to the first question is no, no amount of axes will help. That feature needs a special cutter, EDM or a design change.

A quick CAD habit: set the view normal to the surface you care about and imagine a cylinder about twice the tool diameter wide running straight out of the part. If that cylinder hits another feature before it clears the part, the holder probably will too.

Undercuts

An undercut is material hidden under an overhang when viewed from the main machining directions. 5-axis helps with two kinds:

1. Angled undercuts. A pocket that goes in at 30 degrees under a flange is visible if the tool tilts 30 degrees. This is routine.
2. Shallow side undercuts. A small relief under a lip can be reached by leaning a ball end mill in.

It does not help with fully enclosed undercuts such as an internal groove in a blind bore. Those still need a slotting or lollipop cutter, and the groove shape must match a standard cutter profile.

Design tip: if an undercut is only there to save weight, remove it for the prototype.

Designing an undercut a standard cutter can reach

When an undercut has to stay, shape it around tools that already exist:

• Match standard profiles. Give internal grooves a width and bottom radius that fit a stock T-slot or lollipop cutter. A full radius at the groove bottom suits a lollipop cutter.
• Leave room for the neck. The cutter head goes in through the opening and the neck must pass with clearance. The radial depth a slotting cutter reaches is limited by the difference between its head and neck diameters, so a deep groove behind a narrow opening may have no standard tool.
• Use standard dovetail angles. Dovetail cutters are commonly 45 or 60 degrees. An angled undercut at one of those angles can be cut with one tool pass instead of a contoured toolpath.

Tool reach and length

A cutter deflects more the further it sticks out. As a rule of thumb, stiffness drops sharply once the tool extends more than about three to four times its diameter. Deep narrow pockets force small, long tools, and those cut slowly and chatter.

5-axis helps by tilting the tool away from a tall wall so a shorter tool reaches the floor. That only works if the geometry leaves room to tilt.

Design tips:

• Keep pocket depth under about four times the corner tool diameter where you can.
• Open a pocket on one side if the function allows it. The tool can then come in from the side.
• Avoid tall thin ribs next to deep floors in the same pocket.

Typical reach by tool diameter

The values below are typical for carbide end mills in aluminum. Steel, stainless and titanium pull them down.

Tool diameter	Comfortable reach (about 3x D)	Practical limit with long-neck tools (about 6x to 8x D, slow)
1 mm	3 mm	6 to 8 mm
2 mm	6 mm	12 to 16 mm
3 mm	9 mm	18 to 24 mm
6 mm	18 mm	36 to 48 mm
10 mm	30 mm	60 to 80 mm

If a corner radius forces a 2 mm tool and the pocket is 25 mm deep, the part sits past the comfortable range. Either the radius grows, the pocket opens up or the quote carries slow long-neck passes.

The holder is the other half of reach. It is much wider than the tool, so a deep feature placed right next to a tall boss can block the tilt that would otherwise let a short tool reach it. Leave space around deep features, not only inside them.

Internal corners and fillets

A rotating tool cannot cut a sharp internal corner. It leaves a radius equal to the tool radius. If the drawing asks for a smaller radius than a practical tool can give, the shop must use a tiny tool or a secondary process.

Design internal radii slightly larger than the radius of a standard cutter. For a 10 mm deep pocket, a corner radius of 3 mm lets the shop use a 5 mm end mill that sweeps the corner smoothly. A 0.5 mm radius in the same pocket needs a 1 mm tool and a lot of machine time.

On blended and contoured surfaces, consistent fillet sizes let the programmer use one ball end mill for large areas instead of changing tools.

Floor radii

The radius where a floor meets a wall is a separate choice. A sharp floor corner comes from a flat end mill. A floor radius that matches a standard bull-nose corner (for example 0.5 or 1 mm) comes from one tool in one pass. An odd floor radius such as 1.7 mm forces ball-nose finishing in small steps.

Walls and floors

Thin walls vibrate and move as material comes off. For aluminum prototypes, walls below about 1 mm need care. For titanium and stainless the practical minimum is higher. If you need a thin wall, say where it can have a slightly thicker base or a support that is removed at the end.

Floors that meet walls at a sharp angle are fine for 3+2 cutting. Floors that blend into walls with a changing radius need simultaneous 5-axis to cut cleanly.

Typical design values at a glance

These are typical starting points, not hard limits. The matched shop confirms what its tools and machines can hold on your part.

Feature	Typical design value	Why
Internal corner radius	At least one third of pocket depth, and larger than the tool radius	Lets a stiff tool sweep the corner
Pocket depth	Up to about 4x the corner tool diameter	Beyond that, long-neck tools and slow feeds
Wall thickness, aluminum	1 mm or more	Thinner walls chatter and move
Wall thickness, steel or titanium	1.5 mm or more	Higher cutting forces
Drilled hole depth	Up to about 6x diameter	Deeper needs peck drilling or special drills
Tapped thread depth	About 1.5x the thread diameter	More depth adds little strength
Smallest drilled hole	About 1 mm	Smaller needs micro tools
Engraved text	3 mm character height or more, on a flat face	Small text on curves needs simultaneous paths

For typical tolerances by material that pair with these rules, see the materials table on the home page.

Holding the part

Every part has to be clamped somewhere. On a production part the shop builds a fixture. On a prototype it usually uses one of these:

• Vise on a raised base. The part sits high so the spindle can tilt around it. Needs a flat, parallel area at the bottom.
• Tab or extra stock. The part is cut from a larger block and stays attached by a tab, which is cut off and cleaned at the end.
• Dovetail. A small dovetail is machined on the stock and held in a matching fixture. Common for 5-axis because it clears the spindle at steep angles.

Design tip: tell the shop where a witness mark is acceptable. That single note can remove a whole setup.

Designing for a fixturing tab

• Put the tab on a face with no tight tolerance and no cosmetic requirement.
• Say how the witness may be left: as cut, filed flush or blended within a stated amount.
• Expect extra stock under the part for dovetail or raised holding, typically a few millimeters up to about 10 mm. That matters for stock cost in titanium or Inconel.
• If the part has no flat area at all, add a small flat boss in the model and note whether it stays or is removed at the end.

Put datums where the machine can reach them

A key benefit of 5-axis is cutting the datum faces and the critical features in one clamping. When the locating face and a toleranced bore come from the same setup, their relationship depends on machine accuracy, not on re-clamping.

Help that happen. Place datums on real, machined faces near the critical features, not on the axis of a freeform surface. Check that a CMM probe can reach both the datums and the features they control, or inspection will be slow and indirect.

Holes and threads

Holes normal to a flat face are easy at any angle on a 5-axis machine. Holes that break out on a curved or sloped face are harder: the drill walks. A small spot face at the entry or exit keeps the drill straight.

Use standard drill and tap sizes. A thread specified as M6 is quoted in seconds. A custom thread needs a thread mill and more programming.

Use 3+2 where you can

Many angled parts need only 3+2: the machine tilts, locks and cuts as if it were a 3-axis mill. Grouping angled holes and faces onto a few planes keeps the part in 3+2 and widens the list of shops that can quote it. Save simultaneous motion for surfaces that actually twist or blend. The self-check on the home page helps you decide, and the simultaneous vs 3+2 comparison explains the trade-off in detail.

Features that quietly raise the price

Feature	Why it costs	Cheaper alternative
Very small internal radii in deep pockets	Tiny tools, slow feeds	Larger radius or open the pocket
Cosmetic chamfers on every edge	One more toolpath each	Break sharp edges only
Tight tolerance everywhere	Slow finishing and more inspection	General tolerance plus a few critical dims
Text engraved on curved faces	Simultaneous toolpath for a label	Flat area for text or a laser mark
Mirror finish on a contour	Many fine passes and polishing	Specify Ra only where it seals or slides

Drawing notes that save a round of questions

• A general tolerance, for example ISO 2768-m, for everything not called out.
• An edge break note, for example “break sharp edges 0.2 to 0.5 mm”.
• Thread callouts with type, size and depth, not modeled threads.
• Surfaces that must be finished with simultaneous 5-axis, marked on a view.
• Zones where a witness mark or tab remnant is acceptable.
• Ra values only on sealing, sliding or cosmetic faces.

Before you send the model

1. Check each feature for a line of sight from some tool angle.
2. Match internal radii to real cutters.
3. Mark where the shop may hold the part or leave a witness.
4. Tolerance only what matters and use a general tolerance for the rest.
5. Note whether any surface must be cut with simultaneous 5-axis for finish.
6. Check deep features against the reach table above.
7. Place datums on faces that can be cut in the same setup as the critical features.

For how these choices show up in money, read what a 5-axis prototype costs. When the model is ready, send it for matching and a shop that cuts similar geometry will tell you what it would change.

Frequently asked questions

Keep reading

• Aluminum Alloys for 5-Axis Prototypes: 6061, 7075 and 2024
• Fixturing a 5-Axis Prototype: Dovetails, Pull Studs and Soft Jaws