What CNC Machining Can't Do: A Designer's Guide to the Real Constraints

CNC machining is one of the most capable and versatile manufacturing processes available. It produces accurate, strong, dimensionally stable parts from a wide range of metals and engineering plastics, and it can handle complex geometries that would be difficult or impossible to achieve through other methods. But it has constraints, and understanding them early saves time, cost, and the frustration of receiving a quote back with a list of questions about your design.

Most of the limitations come down to a simple physical reality: every cutting tool is round, rotates about an axis, and has to be able to reach the feature being cut. Once you understand that, most of the common constraints start to make intuitive sense.

Internal Corners Cannot Be Perfectly Square

This can be a point of confusion, particularly for designers who are used to working in CAD where a perfectly square internal corner is trivially easy to specify. In the real world, cutting tools are cylindrical. When a milling cutter machines a pocket or a slot, it leaves a radius at every internal corner equal to the radius of the tool.

A 6mm end mill, for example, will leave a 3mm internal radius in every corner it cuts. You can reduce that radius by using a smaller tool, but you cannot eliminate it. Very small tools introduce their own issues: they’re more fragile, they require slower cutting speeds, and they add cost and time to the program.

If your design has a mating part that needs to fit into a pocket with truly square corners, the practical solutions are to specify the largest acceptable corner radius and design the mating part accordingly, to add a small undercut or relief at the corners to clear the radius, or to address the corner with a secondary operation such as broaching. It’s worth having this conversation with your machinist before finalising the design, because the cleanest solution depends on what the feature is for.

Deep, Narrow Pockets and Slots Are Difficult

The deeper a pocket or slot, the longer the cutting tool needs to be. A long, thin tool flexes under cutting forces, which affects dimensional accuracy and surface finish. There’s also a limit to how far a tool can reach into a pocket before the tool shank begins to rub on the walls of the pocket rather than just the cutting tip doing the work.

As a general rule, the depth-to-width ratio of a pocket should be kept as modest as possible. A pocket that’s twice as deep as it is wide is manageable. One that’s five or six times deeper than it is wide starts to create real machining difficulties. The same logic applies to slots: very narrow, deep slots are challenging to machine cleanly and may require specialist tooling.

If your design requires a deep, narrow feature, it’s worth thinking about whether it genuinely needs to be produced as a single machined pocket, or whether the part geometry could be rethought to make the feature more accessible.

Undercuts Require Special Tooling

An undercut is any feature that sits beneath an overhang, where a standard cutting tool approaching from above cannot reach. Classic examples include T-slots, dovetail grooves, scalloped features on the underside of a flange, and internal grooves on a cylindrical bore.

Undercuts aren’t impossible to machine, but they require specialist tools such as T-slot cutters or undercut end mills, and the geometry has to allow the tool to be positioned correctly. On a three-axis machine, some undercuts simply can’t be reached. On a five-axis machine, the part can be approached from more angles, which opens up more of the geometry, but there are still features that can’t be cut in a single setup.

When reviewing a design, it’s worth asking whether any undercut features are truly necessary, or whether they could be repositioned or redesigned to be accessible from a standard approach angle. Where undercuts are essential, flagging them to the machinist at the quoting stage avoids surprises later.

Truly Blind Internal Features Are Not Accessible

CNC machining is a subtractive process. The tool starts from the outside of the billet and removes material from the accessible surfaces. Any internal feature, whether a cavity, a channel, or a bore, needs a path by which the tool can reach it.

This means fully enclosed internal cavities, the kind of feature that additive manufacturing can produce with relative ease, are not possible in a single CNC machined part. An internal channel that doesn’t break a surface, a hollow sealed within the body of a part, or a curved internal path cannot be machined in one piece.

The practical workarounds are to split the part into two pieces, machine the internal features in each half, and then join them, or to rethink the design so that internal features are accessible from an open face. This is a useful prompt to consider during the design stage: if you’re creating an internal channel for fluid flow or cable routing, how will it actually be machined?

Very Thin Walls and Features Can Flex or Break

Thin walls and fine features are difficult to machine because the cutting forces involved in material removal are transferred into the part itself. A thin wall will deflect under the cutter rather than hold its shape, which means the finished dimension won’t match the intended one. In extreme cases, the feature breaks entirely during machining.

Minimum wall thickness depends on the material and the geometry, but as a rough guide, walls thinner than 0.5mm in metal or 1mm in plastic become increasingly problematic. The taller a thin wall is, the worse the problem gets, because there’s more unsupported structure for the cutting forces to act on.

Where very thin features are essential, they’re often better produced by a different process. Thin sheet metal features, for example, might be better formed than machined. Thin plastic features might be better suited to vacuum casting or injection moulding.

Draft Angles Don’t Apply, But Deep Vertical Walls Do Create Issues

Unlike injection moulding, CNC machining doesn’t require draft angles to release the part from a tool. This is one of the genuine advantages of machining for prototype work: you can machine vertical walls without worrying about how the part will eject from a mould.

However, very deep vertical walls still present machining challenges. As the tool reaches deeper into the material, the unsupported length of the cutter increases, tool deflection becomes more of a factor, and cutting conditions become harder to control. The surface finish at the bottom of a deep vertical wall is often less good than at a shallower depth.

For a prototype that will ultimately be injection moulded, it’s worth noting that features machined without draft will need to be revisited when the production tool design is finalised. CNC is forgiving in this respect, but it shouldn’t lead to an assumption that the same geometry will translate directly to a mould tool.

Threads Have Pitch and Size Limits

Tapped threads are a standard feature in CNC-machined parts and are generally straightforward to produce. However, there are practical limits at both ends of the size range.

Very fine or very small threads, below M2 in most cases, are fragile to cut and prone to breakage during tapping. The smaller the tap, the higher the risk. Very coarse or large threads may require tooling that isn’t held as standard stock, which can affect lead time.

At Prototype Projects, standard threads from M2 to M12 are supported on all services. Non-standard threads, left-hand threads, or very fine pitches should be flagged at the quoting stage so that the right tooling can be confirmed.

Perfectly Flat Surfaces Have a Practical Limit

CNC milling produces flat surfaces by passing the cutter across the material in a series of parallel passes. The result is a surface that’s very flat by most practical standards, but which carries subtle tooling marks from the cutter path. The spacing and depth of these marks depends on the tool diameter, the step-over distance, and the feed rate.

For most prototype applications this is entirely acceptable and often goes unnoticed after degreasing and inspection. Where an optical-quality or mirror-flat surface is required, additional finishing operations such as lapping or grinding may be needed, which fall outside standard CNC machining operations.

The Part Has to Be Held Somewhere

Every CNC machining operation requires the workpiece to be clamped securely in the machine. This seems obvious, but it has a design implication: the surfaces used to hold the part need to be accessible and robust enough to allow clamping without damage.

Very small parts, very thin parts, and parts with no obvious flat reference surfaces can all be awkward to hold. Sometimes a fixture needs to be made specifically for the part, which adds time and cost. In some cases, the solution is to machine the part from a larger billet with a flange left in place for clamping, which is then removed as the final operation.

If your part is unusually small or has no obvious clamping surfaces, raising this at the design review stage is worthwhile. It’s a solvable problem in virtually all cases, but the solution is easier to build into the process from the start than to work around after the fact.

Ready to start your next project?

Knowing what CNC machining finds difficult is only half the picture. If your design has constraints that push against the limits described in this article, we can often suggest a practical workaround, whether that’s a design modification, an alternative process, or a combination of both.

Contact us to discuss your project, request a quote, or take a look at the full CNC machining service to see what’s possible.