CNC machining guide

Why machining underpins everything else

CNC machining deserves more attention than any other process, and not only because it makes finished parts. It also makes the tools that every other process depends on: injection molds, stamping dies, forging dies, casting patterns, and extrusion dies are all machined. Understanding machining is therefore a prerequisite for understanding the cost of almost anything else you might have manufactured.

The central fact is simple. A rotating cutter of finite diameter removes material from solid stock, and it must physically reach every surface it cuts. Nearly every design rule below is a consequence of that sentence. Rather than memorising thresholds, it is far more useful to understand which physical constraint each rule expresses, because then you can reason about the cases the rules do not cover.

The machines

3-axis vertical mills

The workhorse of every job shop. The table moves in X and Y while a spindle moves up and down in Z. Table travel is typically around twice as long in X as in Y. A 3-axis machine can only cut what it can reach from directly above, so a part with features on several faces must be unclamped and re-fixtured for each new direction. Each of those re-fixturings is a setup, and setups are where cost and tolerance error accumulate.

5-axis mills

Two rotary axes are added on top of X, Y and Z, letting the cutter approach from almost any angle. Some machines are built for indexing, holding a rotation while cutting in three axes, which is usually described as 3+2 machining. Others support fully simultaneous 5-axis motion, needed for genuinely sculpted geometry such as impellers and blades. The practical benefit for most parts is not exotic surfacing but setup reduction: five faces of a part can be cut without ever unclamping it.

What a modern machine has

• Tool carousels holding roughly 20 to 50 tools with automatic changing, so a part needing many different cutters is not inherently a problem.
• Spindle speeds typically in the range of 8,000 to 15,000 rpm, with flood coolant and air blast to control heat and clear chips.
• Automatic tool setting, measuring each tool’s real length and diameter and compensating for the difference from nominal.
• Touch probes for locating the part and the fixture in machine coordinates, and for in-process measurement.
• Positional accuracy on the order of ten microns within a single setup, which is why features cut in one setup can hold tolerances that features split across setups cannot.

How a job actually runs

Cost follows the sequence of work, so it is worth knowing what that sequence is.

• Planning and CAM programming. Toolpaths, tool selection, and machining strategy. This is one-time engineering effort per job.
• Stock selection and cutting to size.
• Machine setup: loading and setting tools, installing the vice or fixture, probing and setting work offsets for each operation.
• Cutting any custom workholding, most commonly softjaws machined to match the part profile.
• Running each operation, with the part re-fixtured between them.
• Inspection, then deburr, finishing, and packing.

Two things in that list are paid once per job regardless of quantity, and everything else is paid per part. That split is the key to reasoning about cost.

Workholding, and why it shapes your design

How a part is held is not a detail left to the shop. It determines how many setups are needed, how hard the part can be clamped, and therefore how fast it can be cut. Designing without considering workholding is the most common reason a part is more expensive than it needs to be.

Vice and work stop

The default setup everywhere. A machine vice grips two parallel faces, a work stop fixes position along the jaw, and parallels set the height. It is fast, repeatable, and free. If your part has two opposed parallel faces to clamp, you get this setup for nothing.

Softjaws

Custom vice jaws machined to match the profile of the part. The common arrangement is a double-vice setup: the first operation is cut with the raw stock in a standard vice, then the part is flipped into softjaws that cradle the now-machined profile for the second operation. The design implication is worth stating plainly: if every feature of your part is reachable from two opposing faces, the whole part can be made in two operations. That is the single most valuable DFM property a machined part can have.

Fixture plates

For larger quantities, several parts are held on one plate so the machine runs longer between operator interventions. This favors parts that can be located and clamped simply and identically, and it rewards designing a flat reference face into the part.

Dovetail fixtures for 5-axis

A dovetail form is cut into the stock so a matching vice can grip it from below, leaving five sides of the part exposed. It costs an extra preparation operation but makes efficient use of expensive 5-axis capacity.

The tools, standard and otherwise

Designing features that standard tooling can cut is most of DFM. Knowing what less common tooling exists is the rest, because it often turns a 5-axis part into a 3-axis part.

Custom-ground tooling is available and occasionally worth it, but only when volume justifies it or when a single custom tool collapses a multi-setup part into a simple one.

What actually drives cost

Paid once, spread over the quantity

• Programming and process planning. Feature complexity translates directly into programming time, so the simplest strategy that meets the function is always the cheapest. On a prototype run of a complex part this can dominate the total.
• Machine setup. A part that runs in a standard double-vice and softjaw arrangement costs materially less to set up than one needing a bespoke fixture.

Paid on every part

• Material. Worth optimizing only at high volume; swarf is recycled and stock is rarely the dominant cost at prototype quantities.
• Part setup labor. Loading and unloading is manual on most machines. Simple, unambiguous fixturing is loaded faster and more reliably. Tight tolerances slow this further, because chips and debris on locating faces must be cleared each time.
• Tool wear. Every cubic millimetre removed wears tooling. Minimising material removal matters at volume, sometimes to the point of designing around a standard extruded profile.
• Machining time, which is a direct function of your geometry.
• Tolerance, which affects machining time non-linearly.
• Inspection, which follows from tolerance and from how the drawing is dimensioned.

What makes machining time go up

Material removal rate is set by the largest, stiffest tool that can be used, and tool size is set by your smallest internal radius. Halving a corner radius can force a much smaller cutter across the entire feature, and the effect on time is far worse than proportional.

• Design every feature to be cut by the largest tool that will fit.
• Arrange the bulk of material removal in the first operation, while the stock is stiffest and most securely held.
• Stiffer parts, more secure clamping, softer materials, and looser tolerances all cut faster.
• A better ratio of finished part volume to stock volume means less metal to remove.
• Surface finish requirements slow cutting speeds, again non-linearly.
• Non-standard chamfer angles, rolling external fillets, and free-form surfaces are trivial to draw and slow to cut, because they are produced by a ball cutter stepping across the surface in many small passes.

Why tolerance is the sharpest lever

Tolerance cost is not linear. Loosening a dimension from a few hundredths of a millimetre to a tenth may cost nothing at all; tightening from a few hundredths to a few thousandths can multiply the price of the part. At the tight end, the machine’s own repeatability, tool deflection, fixture deflection, and the temperature of the workpiece and coolant all become variables that have to be controlled. Some shops are simply not equipped for that, and the honest answer is that a tolerance which cannot be measured reliably will become an argument after delivery rather than a specification before it.

Inspection follows tolerance

Inspection effort scales with how much you ask to be verified and how hard it is to verify. A go/no-go gauge on a hole is trivial; a bore gauge reading to a couple of microns is not. A caliper check costs a fraction of a CMM report. Restricting tight tolerances and formal inspection to genuine functional interfaces is one of the largest available cost reductions, and poorly constructed GD&T inflates this by forcing datum simulators to be built that the function never required.

Feature by feature

Outer profiles

The depth of a profile is limited by the flute length of the largest tool that can cut it, and that tool size is limited by the smallest internal radius anywhere on the profile. One tight corner therefore constrains the whole feature. Very deep profiles can be cut in two operations from opposite ends, but the blend where the two meet is only as good as the fixturing accuracy between them, and a visible step is the failure mode.

Pockets and flat-bottomed holes

The same logic applies. Choose a corner radius slightly larger than the tool that will cut it, rather than exactly equal, so the cutter engages evenly around the corner instead of wrapping fully into it. Even engagement gives a better finish and longer tool life. As a working threshold, pocket depths up to roughly six tool diameters are routine. Beyond that, special tooling is usually needed, which is possible but affects lead time and price. Approaching ten diameters is difficult regardless of tooling.

Fillets and chamfers

A fillet whose axis is parallel to the spindle is cut directly by the corner of an endmill and is cheap. A fillet whose axis is not parallel to the spindle has to be surfaced by a ball cutter in many passes, which takes far longer and leaves a visibly different, faintly scalloped finish.

Chamfer tools come in standard included angles, commonly 60, 82 and 90 degrees. A chamfer at one of those angles on a flat face is a fast 2D operation. An unusual angle must be surfaced. A chamfer that runs continuously across several planes, or wraps an undercut, needs either surfacing in multiple setups or continuous 5-axis motion, which restricts which machines can make the part at all. Chamfers are one click in CAD and can be one of the most expensive features on the part, so it is worth knowing which of yours are cosmetic.

Do not tolerance across setups

Within a single setup, machines position features relative to one another to roughly ten microns, so tight relative tolerances are almost free. The moment two features are cut in different setups, the tolerance between them includes all the uncertainty of re-fixturing. If two features must be precisely located relative to each other, design them so they are reachable from the same direction. This is often the difference between a part that is straightforward and one that needs a custom fixture and a CMM report.

Thin features and vibration

Cutting forces are a series of impacts containing a wide band of frequencies, and they will excite whatever vibration modes your part has. Chatter spoils surface finish and tolerance, and can damage the part outright. Blanket minimum-thickness rules miss the point, because what matters is local stiffness rather than thickness alone.

• Thin pocket floors behave like drumheads. The risk is governed by unsupported span relative to thickness, not thickness on its own.
• Thin stiffening webs lose stiffness non-linearly as their section shrinks. Beam intuition is the right instinct here.
• Cantilevered features such as tabs and snap fits are far less stiff than supported ones. Balance height against base width and thickness.

Undercuts

The only question worth asking is whether the undercut forces an extra setup or a 5-axis machine. Many undercuts do not, because keyseat cutters, slitting saws, lollipop cutters and dovetail cutters reach around corners in a 3-axis setup. Knowing which undercuts are cheap is far more useful than avoiding them on principle.

Warping and internal stress

Stock arrives with a non-uniform internal stress state. Extruded aluminum bar, for example, typically holds tension near the surface and compression in the core. Machining removes some of that stressed material and the remaining part moves to find equilibrium. Parts with strongly asymmetric geometry, or where most of the stock is hogged out, are the ones that warp when released from the fixture. A machinist can mitigate this by balancing the part within the stock or by rough-cutting, stress-relieving, then finishing, but it cannot always be designed around. If your part is large, thin and asymmetric, expect to discuss it.

Compliance and clamping

Parts are clamped with hundreds of pounds of force, and in the final operation they are clamped in their partly finished, least stiff state. Two things have to be true: the part must be grippable hard enough to resist cutting forces, and it must not deflect meaningfully under that grip. A part that is compliant when clamped can be machined, but only by slowing everything down, and no amount of slowing fixes the tolerance error caused by a part springing back after release. If you want a part cut cheaply and accurately, give it something stiff to be held by.

Three changes that usually pay for themselves

• Add flat, parallel reference faces. Somewhere for the part to sit on parallels and be gripped in a standard vice removes the need for a custom fixture and makes location repeatable.
• Align through-features so they share a direction. Fastener holes and lightening holes drawn normal to whichever face they sit on will each demand their own setup. The same holes made coaxial can be cut in one.
• Open up small internal radii and close small gaps between features. Increasing a corner radius so a larger cutter fits, and removing narrow slots between standoffs, often cuts machining time substantially for a negligible weight penalty.

A fourth, less obvious one: add stiffening where the part will be clamped. A structurally efficient open section can be a poor machining candidate purely because it flexes in the vice, and a rib that adds a few grams can move a part from needing a custom fixture to running in a standard double-vice setup.

Metals

Aluminum alloys dominate machined prototypes because they cut quickly and cost less per part in machine time. Steels and stainless are chosen for strength, wear, or corrosion resistance, and cost more in cycle time. Titanium and the superalloys are specified when strength to weight or temperature resistance justifies the machining difficulty.

Plastics

Machined plastics are chosen when a part needs chemical resistance, electrical insulation, or low friction, or where volumes do not justify a mold. Machined plastic parts behave differently from molded ones: there is no draft, no knit line, and internal stress from the stock can cause movement after cutting.

Choosing between them

• Specify the alloy and temper, not just the metal. "Aluminum" is not a specification, 6061-T6 is.
• No material family is biocompatible. Only a named grade with a certificate, and the certificate belongs to the grade and the lot rather than to the polymer or the alloy.
• For tight tolerance plastic parts, ask for stress relieved or annealed stock, and expect a rough cut, a stress relief, then a finish cut rather than one operation.
• If the part is cosmetic, decide the finish before the material, because anodising and plating constrain the alloy.
• For plastics, check chemical compatibility against what the part will actually touch in service.
• Ask whether a material certificate is required. It changes sourcing, and it is easier to arrange before the order than after.

What we run

Held in regular stock and machined in house: aluminum 6061-T6, 7075-T6 and 5052; mild steel 1018; alloy steel 4140; stainless 304 and 316L; brass C360; and POM, PC, PMMA and PTFE in plate.

Sourced to order, normally within a week: 17-4PH stainless, tool steels D2 and A2, Ti-6Al-4V, PEEK and Ultem. Where a material certificate is required, say so at inquiry stage, because it changes which mill lot is bought.

How tolerance is specified

A tolerance is the permitted deviation from a nominal dimension. If a drawing does not call out a tolerance for a feature, a general tolerance applies, usually taken from ISO 2768 or an equivalent block on the drawing. ISO 2768 defines classes, from fine through to very coarse, with the permitted deviation widening as the nominal dimension grows.

Where tolerance costs money

• Every tightened dimension adds inspection time, not just cutting time.
• Tolerances tighter than the general class should be called out individually, not applied to the whole drawing.
• Geometric tolerances (flatness, position, concentricity) often matter more than linear ones, and are cheaper than over-tightening every linear dimension.
• A tolerance tighter than the measuring equipment can resolve cannot be verified, and will be argued about after delivery.
• Plastics move with temperature and humidity. A tolerance that is routine in aluminum may be unachievable in nylon.

How to specify well

• Put a general tolerance block on the drawing so undimensioned features are unambiguous.
• Tighten only the features that carry a fit or a function.
• State the datum scheme. Position tolerance without datums is not measurable.
• Say whether inspection is required on every part or on a first article only.

What we hold

Tolerances that tight are verified on a CMM and reported. Plastics are quoted looser than metals because they move with temperature and with moisture, not because the machine cannot cut them.

Sending files

• Send a STEP file for geometry, and a PDF drawing for anything the geometry cannot carry: tolerances, finishes, threads, material, and inspection requirements.
• Do not rely on the model alone for critical tolerances. A model has no tolerance.
• Include the quantity you actually want, and the quantity you expect to want later. Process choice changes with volume.
• Say which features are critical. It is the fastest route to a useful quote.

Reducing cost without redesigning

• Loosen tolerances on anything that does not carry a fit.
• Increase internal corner radii so a larger, faster tool can be used.
• Accept a standard finish unless the part is cosmetic or has a functional surface requirement.
• Reduce the number of faces that need machining. Leaving stock faces as supplied is free.
• Combine parts where it saves a setup, or split them where a single part forces an expensive setup.

Avoiding rework

• Agree the datum scheme before production, not during inspection.
• Ask for a first article before a full run on anything with tight tolerances.
• Specify finish before anodising or plating, since coatings add thickness and can push a tight dimension out of tolerance.
• State whether deburring is required and how sharp edges should be treated.

How we work

The design review happens before the quote, not after the order. If a corner radius forces a smaller cutter than the pocket depth allows, or a tolerance would need an operation you may not want to pay for, it is in the quotation as a note with the cost of each option.

Parts ship as-machined and deburred unless a finish is specified. A first article dimensional report is standard on a new part, and material certificates, full-batch reports, and capability studies are supplied where the order calls for them.