Guide
Undercut machining on milled parts: which T-slot, dovetail and lollipop undercuts can a cutter reach, and how should you dimension them?
Undercut machining is the cutting of a feature that sits behind an overhang when seen from the spindle direction, so a plain end mill coming straight down cannot reach it: the inside of a T-slot, the angled flanks of a dovetail, a groove around the inside of a bore or a pocket wall that leans back under its own lip. A standard three-axis mill cuts these only with form cutters that have a narrow neck and a wider cutting head, and the shape of that head is what decides whether your undercut is a routine feature or a redesign.
By Saola Manufacturing engineering team · Published · Updated
This guide is written for the person drawing the part. It does not repeat general design-for-machining advice; it covers the one question that decides cost on an undercut: can the cutter physically get in, sweep the shape and get back out, and how do you put that shape on the drawing so that it can be made and inspected without argument. For edge breaks and shoulder relief grooves on turned parts, see fillet vs chamfer on machined parts; for back-side spotfaces, see counterbore vs countersink vs spotface.
On this page
Which undercut shapes can standard cutters reach on a three-axis mill?
Four families of undercut are routine because a catalog cutter exists for each: T-slots, dovetails, keyseat or slot-cutter grooves, and lollipop (undercut ball) profiles. Anything that does not match the head shape of one of those cutters, or that a neck cannot reach, is where cost and redesign start.
The cutter families are old and standardized. The ASME standard for high speed steel milling cutters and end mills (ASME B94.19) covers T-slot cutters, Woodruff keyseat cutters and dovetail cutters alongside ordinary end mills; the standard itself is limited to one-piece high speed steel tools, but carbide cutters of the same types are sold too. Each has the same anatomy: a shank held in the spindle, a reduced neck, and a head wider than the neck. The head cuts the hidden part of the feature; the neck has to pass through the visible opening without rubbing.
Three facts follow from that anatomy, and they apply to every undercut on a three-axis part. First, there must be an open path for the head to enter, usually from the end of a slot, from a pocket that was cleared first with an end mill, or by plunging down a bore and then moving sideways. Second, the radial depth of the undercut can never exceed the difference between head and neck radius, minus a clearance so the neck does not drag. Third, the cutter leaves its own profile behind: its corner radius at the root, its angle on a dovetail, its ball radius on a lollipop. You design to the cutter, not the other way around.
What does each undercut type need on the drawing?
Dimension the functional surfaces you can inspect, leave the theoretical sharp corners as reference, and say what corner condition the cutter may leave. The table sets out the usual approach for each type.
The pattern is the same in every row: give the size that the mating part actually touches a real tolerance, and make the rest either a basic dimension controlled by a profile tolerance or a reference value. Dimensioning and tolerancing conventions here follow ASME Y14.5; if your drawings are on ISO GPS, the logic is the same with different symbols.
| Undercut type | Cutter that makes it | Dimension with a tolerance | Give as reference or let the cutter set |
|---|---|---|---|
| T-slot | End mill for the throat, then T-slot cutter for the head | Throat width, head width, depth from the top face to the underside of the lips (the face the bolt head bears on) | Head height and total slot depth if the floor carries no load; corner radii in the head |
| Dovetail (female or male) | Dovetail cutter at a catalog angle, usually 45° or 60° | Angle, depth, and width measured over or between gauge pins | Theoretical sharp-corner width; root relief |
| Internal groove in a bore | Keyseat or slot cutter, moved on a circular path | Groove diameter, groove width, position from a datum face | Groove corner radii |
| Lollipop undercut wall or pocket | Undercut ball (lollipop) cutter | Profile of a surface to a datum reference frame | Ball radius and allowed scallop |
| Back-side chamfer or spotface | Back-chamfer or back-spotface tool through the hole | Spotface diameter and depth from the far face | Edge break size |
How do you dimension a T-slot so it can be made and checked?
Treat the throat width as the controlled size, because that is what guides the bolt or the mating tongue, and dimension the depth from the top face down to the underside of the lips, because that is the face the bolt head pulls against. If the slot takes standard bolts, call out the standard slot size rather than inventing one.
Machine-table slots are standardized: per ISO 299 (ISO 299:1987) the throat widths form a preferred series, from 5 mm through 54 mm, with matching head dimensions and bolts, and T-slot cutters are made to suit those sizes. A fixture plate or slide that takes off-the-shelf T-bolts should simply reference the standard size; it then fits the cutters in every shop and the bolts in every catalog.
Custom T-slots are fine, but three details decide whether they are cheap. Keep the head width and height to sizes a catalog cutter cuts in one pass; a head taller than the cutter needs passes at two heights, which doubles the cutter path and can leave a witness line. Let the cutter corner radius stand in the corners of the head unless a square corner is truly needed for a mating part. And give the slot an open end: a T-slot closed at both ends needs a drilled or milled entry pocket large enough to drop the cutter head in, which must appear on the drawing.
For inspection, the throat width is checked directly with a flat plug gauge or gauge blocks; the head width and height are hard to reach and are usually checked on a sectioned first article or with a probe that can reach under the lips. Make the depth to the underside of the lips the toleranced dimension, since that face is what clamps.
How should a dovetail be dimensioned when its edges are sharp only in theory?
Dimension a dovetail by its angle, its depth and a width measured over (male) or between (female) two precision gauge pins, and show the pin diameter. The sharp-corner width a CAD model reports cannot be measured, so it belongs on the drawing as a reference only.
Dovetail cutters come in fixed angles, and the most common in tool catalogs are the 45 and 60 degree families, which is the typical reason dovetail slides are drawn at one of those two angles. Pick one of them unless a mating part forces otherwise; a nonstandard angle means a special-ground cutter.
The pin measurement is pure geometry and needs no lookup. For a female dovetail with flank-to-floor angle A and theoretical floor width W, two pins of diameter D lying in the corners give a width between pins of M = W − D × (1 + cot(A/2)). For a male dovetail the measurement over pins is M = W + D × (1 + cot(A/2)), where W is the theoretical width at the root, where the flanks meet the base surface the pins rest on. Put M, D and the angle on the drawing with M carrying the tolerance, and the shop and your incoming inspection will measure the same thing.
The root of a dovetail always has a small radius or flat from the cutter tip. If the mating part has a sharp corner there, add a relief groove or a chamfer on the mating part, and say so; otherwise the two parts bear on the root instead of the flanks.
When does undercut machining force a redesign or an extra setup?
Undercut machining stops being routine when the head cannot reach the feature, when the neck would have to be too thin for the depth and length involved, or when the shape matches no catalog cutter. In those cases splitting the part, opening an access side or changing the shape is usually cheaper than special tooling.
The warning signs show up early in a model review:
- Closed undercuts. An undercut with no open end and no pocket above it cannot be reached by any cutter. Open one end, or add an access pocket and show it on the drawing.
- Deep undercuts behind thin necks. The deeper the undercut relative to the opening, the thinner the neck has to be, and a long thin neck deflects and chatters. Keep the reach short and the radial undercut shallow; a tight tolerance at the bottom of a deep, narrow undercut is the most expensive feature you can draw.
- Undercuts on several faces. Each face that carries an undercut is typically its own setup on a three-axis machine, with its own fixture and its own datum transfer. Group undercuts on one face where you can.
- Freeform undercut surfaces. A lollipop cutter can sweep a curved undercut wall, but the surface is built from many passes with scallops between them, and some undercut geometry needs a tilted tool. Saola does not offer simultaneous five-axis machining, so a part that only works that way should be redesigned or sent to a shop that runs it.
- Undercuts that could be a second part. A dovetail way or a T-slot is often easier as a bolted-on gib, strip or clamp plate than as a cut into a large block.
On a cast part, an undercut that would need a side action in the die is often cheaper to cast straight and add afterward by CNC milling, which at Saola is set up as secondary machining on the plant’s own ADC12 aluminum and Zamak 3 zinc die castings and on sand-cast brass and bronze, rather than as a general billet-machining shop. The milling page also lists the bore and concentricity limits the plant holds; check those against any tolerance you put on an undercut before you send the RFQ. Why slides and cores raise die cost is covered in die casting mold cost, and how many setups add to a quote in what drives CNC machining cost.
How should a lollipop undercut or internal groove be toleranced?
Use a profile tolerance on the undercut surface against your datums, and state the largest ball radius and the scallop height you accept. Plus-and-minus coordinates on a curved undercut wall cannot be inspected consistently.
A lollipop cutter is a ball on a reduced neck. Because the ball can cut above its own equator, it reaches back under an overhang, but the surface it leaves is a set of cusps whose height depends on the ball radius and the step between passes. The drawing should let the shop choose a ball no smaller than a stated radius and set a maximum scallop or a surface texture limit, then control the shape with a profile tolerance referenced to the datum reference frame, as described in profile tolerance and the GD&T symbols chart.
Internal grooves in bores, such as retaining ring or seal grooves, are cut with a slot cutter moved on a circular path, the same circular interpolation a thread mill uses but without the axial feed (see thread milling vs tapping). Dimension the groove diameter and width with tolerances, locate the groove from a datum face rather than from the bore entrance, and note whether the groove corners may carry the cutter radius. If the groove is in a blind bore, make sure the bore is deep enough below the groove for the cutter head to clear.
What should the RFQ say about undercuts?
Send the 3D model and a drawing that marks every undercut, says which dimensions are functional, and states whether cutter radii and catalog angles are acceptable. That lets the supplier quote the real cutter and setup plan instead of guessing.
A short checklist that removes most back-and-forth:
- A note such as “INSIDE CORNERS OF UNDERCUTS MAY CARRY CUTTER RADIUS UNLESS OTHERWISE SPECIFIED”, and a maximum radius where a mating part needs clearance.
- For each dovetail: the angle, the gauge pin diameter and the toleranced measurement over or between pins.
- For each T-slot: the standard size it follows, or throat width, head width and depth to the head underside.
- For freeform undercuts: a profile tolerance, the datum reference frame, and the accepted ball radius or scallop.
- Whether access pockets or entry holes may be added, and where they must not go.
- Which undercut dimensions you want reported on the first-article inspection, since a buried feature may need sectioning or special gauging.
The general RFQ package is covered in how to prepare a machining RFQ. When the drawing is ready, send it for a quote; Saola’s drawing review returns a marked-up copy and a short DFM list, per the quality page, and that is where an undercut that cannot be reached gets flagged.
Frequently asked
Can a T-slot cutter make a slot that is closed at both ends?
Only if there is somewhere to drop the head in. A closed slot needs an entry pocket or hole at least as large as the cutter head, usually at one end of the slot, and that pocket has to be acceptable on the finished part and shown on the drawing.
Why not just dimension a dovetail at its sharp corners?
Because the sharp corner never exists on the part: the cutter tip leaves a radius or flat, and the top edge is usually broken. Nobody can put a caliper on a theoretical corner, so supplier and buyer end up measuring different things. A width over or between gauge pins is repeatable and maps directly to the model.
Is a lollipop cutter the same as a ball end mill?
No. A ball end mill has a neck as wide as the ball, so it cannot cut above the ball’s equator. A lollipop cutter has a reduced neck behind a near-spherical head, which lets it reach back under an overhang. It is less rigid, so feeds are lighter and the surface needs more passes.
Can undercuts be die cast instead of machined?
Sometimes, with side actions or slides in the die, but each one adds tool cost and maintenance. For a single slot or groove, casting the part without the undercut and milling it afterward is often the simpler route; the decision depends on volume and is worth asking about at the RFQ stage.
Sources
- ASME B94.19, Milling Cutters and End Mills, ASME, 1997 edition (stabilized), accessed October 2026
- ISO 299:1987, Machine tool tables — T-slots and corresponding bolts, ISO, 1987
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018