Die Casting vs. CNC Machining: How the Manufacturing Method Rewrites the Design Rules

The Fundamental Divide: Subtractive vs. Formative Manufacturing

CNC machining is subtractive: you start with a solid block or bar of material and remove everything that isn't the part. This means the process is inherently flexible — you can machine almost any geometry that a tool can reach, with the primary constraint being tool access and the physical limits of the cutting process. There's no tooling cost beyond the standard cutters, fixtures, and programming time. Setup is relatively fast, making machining ideal for prototypes, low volumes, and parts that will likely change.

Die casting is formative: you inject molten metal under high pressure into a hardened steel mold, the metal solidifies almost instantly, and the part is ejected. The mold is the negative of the part, and every feature on the part must be shaped by a cavity in the mold. The mold is expensive — typically $10,000 to $100,000 or more — and changing it is slow and costly. But once the mold exists, parts can be produced at rates of hundreds per hour, with excellent repeatability and low per-part cost. Die casting is the domain of high-volume production.

The design implications flow directly from this divide. A machined part's cost is driven by material removal time, tool changes, and setup complexity. A die-cast part's cost is driven by mold complexity, cycle time, and secondary operations. Designing for one process when the other is intended is the most expensive mistake a product designer can make.

Draft Angles: The Casting's Best Friend, the Machined Part's Stranger

In die casting, draft is not optional. Every surface parallel to the mold's opening direction must have a slight taper — typically 0.5° to 3° — to allow the part to eject from the mold without dragging or scoring. A zero-draft wall in a die casting means the part will stick in the mold, requiring complex slides or lifters, or it will be literally torn out of the cavity, damaging both the part and the tool. Draft is one of the first things a die casting engineer checks, because insufficient draft makes a part uncastable.

In machining, draft is optional and often absent. A vertical wall in a milled pocket is the default — the tool is a cylinder, and the wall it leaves is straight. Adding draft to a machined pocket requires either a tapered tool, a 3D surfacing toolpath with a ball endmill, or a secondary operation. All of these add time and cost. A machined part with drafted walls is more expensive than one with straight walls, all else being equal.

Designers who transition from machined parts to die castings often overlook draft entirely, producing a model that looks perfect in CAD but cannot be ejected from a mold. The fix is to incorporate draft early, ideally by building it into the base sketches and extrusions, or by using the draft analysis tools in the CAD software to verify every face.

Old Li, who has reviewed both machined and cast parts, puts it bluntly: "A machined wall is a soldier standing at attention. A cast wall is a soldier leaning slightly backward, ready to retreat from the mold. Ask a machined wall to lean, and you'll pay for the privilege. Ask a cast wall to stand straight, and it will fight the mold and lose."

Wall Thickness: Uniform for Casting, Flexible for Machining

Die casting demands uniform wall thickness. When molten aluminum at 650°C fills a mold, it cools from the outside in. If the wall thickness varies significantly — say, a 2mm wall next to a 8mm boss — the thin section solidifies first, while the thick section is still liquid. As the thick section cools, it shrinks, pulling material from the already-solid thin section and creating internal voids, sink marks on the surface, or even cracks. Good die casting design maintains a consistent nominal wall thickness throughout the part, with gradual transitions between sections and generous radii at junctions.

Machining has no such constraint. You can carve a part with a 1mm wall transitioning abruptly to a 20mm solid boss, and the machine won't care (though the part may distort). The only limits are tool access and the mechanical properties of the material. This gives the machined part designer enormous freedom, but it also means that a design optimized for machining often has exactly the kind of non-uniform walls that will cause casting defects.

When a customer brings us a machined part and asks us to quote it as a die casting, we immediately check the wall thickness uniformity. If the walls vary by more than a factor of about 2:1, we recommend a redesign to even them out. Old Li's wall thickness rule for castings: "Think of the metal like honey pouring into the mold. It flows smoothly where the channels are even, and it pools and sinks where the channels widen suddenly. A good casting is a gentle river, not a series of rapids and pools."

Corner Radii: Sharp Is Cheap in Casting, Expensive in Machining

Here's one of the most dramatic reversals between the two processes. In machining, as we've written before, a sharp internal corner is the single most expensive geometric feature — it requires either a vanishingly small tool, a secondary broaching operation, or EDM. In die casting, a sharp external corner is also problematic (it creates a stress concentration in the mold and can cause hot tearing in the part), but a sharp internal corner is relatively easy to produce because the mold cavity is formed by a shaped electrode that can have a very small radius. A die-cast part can have internal corners with radii as small as 0.3mm to 0.5mm without significant cost penalty.

However, die castings benefit enormously from generous fillets and radii for a different reason: they promote metal flow and reduce stress concentrations during solidification. A sharp corner in a casting mold is also a sharp corner on the mold itself, which is prone to wear, cracking, and erosion from the high-velocity molten metal. Good casting design rounds every internal and external corner to at least 0.5mm, and larger where possible.

For machined parts, the rule flips: internal corners are costly to sharpen, but external edges can be broken with a simple chamfer tool and are essentially free. This means a designer moving from casting to machining, or vice versa, must completely rethink their corner strategy.

Old Li's corner comparison: "In machining, the tool is round, so the corner is round. In casting, the mold is the reverse of the part, so a sharp internal corner on the part is a sharp external corner on the mold. Sharp steel in a mold wears out fast. So you still want fillets, but for different reasons."

Undercuts and Side Actions: The Casting's Hidden Cost

An undercut in a machined part requires either a special tool (T-slot cutter, dovetail cutter, lollipop cutter) that can reach the feature, or a secondary setup that reorients the part. It adds cost, but it's usually manageable in small quantities.

An undercut in a die casting requires a side action — a moving section of the mold that slides in from the side, forms the undercut, and then retracts before ejection. Side actions are expensive. They add thousands of dollars to the mold cost, they increase cycle time because the slides must move before ejection, and they create witness lines on the part where the slide meets the main cavity. A simple two-plate mold with no side actions is the ideal; every undercut adds complexity, cost, and a potential maintenance headache.

A part designed for machining that has multiple undercuts and re-entrant features is a die casting engineer's nightmare. The redesign usually involves either eliminating the undercuts, reorienting the part in the mold so the undercuts are in the line of draw (parallel to the mold opening direction), or converting the undercuts to features that can be formed by the core (the moving half of the mold) rather than a separate slide.

Old Li's undercut rule for castings: "Every undercut is a moving part in a tool that costs more than your car. If you can design it out, design it out. If you can't, know that you're paying for a little mechanical robot inside the mold that has to work perfectly for 100,000 cycles."

Tolerances: What's Achievable Without Secondary Machining

A CNC machine can hold ±0.01mm on a bore relatively easily, and ±0.05mm on general dimensions is standard for a well-set-up shop. Die casting, as a raw process, is looser. Typical linear tolerances for aluminum die castings are around ±0.1mm to ±0.3mm for dimensions up to 25mm, and larger for longer dimensions. Flatness, perpendicularity, and concentricity are not as tightly controlled as in machining because the part shrinks during solidification, and the shrinkage is never perfectly uniform.

If a die-cast part requires a bearing bore, a dowel pin hole, or a sealing face with tight tolerances, those features are typically machined in a secondary operation — drilling, reaming, boring, or milling the critical surfaces after casting. This hybrid approach (cast to near-net shape, then machine the precision features) is extremely common and combines the low cost of casting with the precision of machining. The design should clearly identify which features are critical and provide stock allowance for the machining operation. Casting designers who specify machined tolerances on as-cast surfaces are setting themselves up for disappointment and high costs.

Old Li's tolerance rule for castings: "The casting gives you the rough shape cheaply. The machining adds the precision expensively. Don't ask the casting to do what the machine does, and don't ask the machine to remove what the casting could have shaped."

Surface Finish and Cosmetic Requirements

Machined surfaces have a characteristic appearance — a pattern of tool marks, a consistent lay direction, and a predictable roughness depending on the tool and parameters. A fine machined finish can be achieved directly off the machine, or with light polishing.

Die-cast surfaces have a different character. They typically show a fine "pebbled" or matte texture from the mold surface, witness lines from ejector pins and parting lines, and possibly flow marks where the molten metal entered the cavity. A high-gloss cosmetic surface on a die casting requires polishing the mold cavity to a mirror finish, which is expensive and must be maintained. Many die-cast parts are painted, powder-coated, or textured to hide the natural as-cast appearance.

Designers who want a "machined look" on a consumer product should understand that machining the entire external surface of a die-cast part defeats the purpose of casting. The better approach is to decide early whether the cosmetic requirement points toward machining (for a premium, small-batch product) or casting (for a cost-sensitive, high-volume product), and then design the part's aesthetic accordingly.

When to Choose Which: A Practical Framework

We use a simple decision tree when a customer brings us a part design and isn't sure whether it should be machined or die cast:

• Volume: Under roughly 500-1,000 units per year, machining is usually cheaper because the mold cost for die casting dominates. Above 5,000-10,000 units, die casting's low per-part cost overcomes the mold investment. Between those ranges, the decision depends on complexity.

• Complexity: A simple part with a few features can be machined cost-effectively at higher volumes. A complex part with organic shapes, thin walls, and internal features may benefit from casting even at lower volumes, especially if the machining alternative requires extensive 5-axis work or multiple setups.

• Material: Some materials are only castable, some are only machinable. High-strength aluminum alloys like 7075 are typically machined, not cast. Zinc, magnesium, and some aluminum-silicon alloys (like A380) are commonly die cast. The material requirement often drives the process.

• Tolerances: If the part has multiple tight-tolerance bores and surfaces that must be accurate, machining is likely the primary process, or casting with significant secondary machining.

• Lead time: Machining has no mold lead time; you can start cutting as soon as the material arrives. Die casting requires mold design, mold building, sampling, and approval — typically 8 to 16 weeks. For fast-turnaround projects, machining is often the only option.

The Horror Shelf Gets a Casting and a Machined Twin

We've mounted two nearly identical aluminum housings on our horror shelf. One was designed for machining and then, without redesign, sent to a die caster for a quote. The die caster's feedback was brutal: zero draft on vertical walls, walls varying from 1mm to 12mm, sharp internal corners, six undercuts requiring side actions. The quoted mold cost was astronomical. The part is labeled: "Designed for machining, quoted for casting. Didn't fit."

Next to it is the redesigned version: draft added, walls uniformed, undercuts eliminated, generous radii. Its label: "Designed for casting. Mold cost reasonable. Production cost $6.80." Between them, a sign: "The process chooses the design. Not the other way around."

Old Li added a third item: a simple machined prototype of the same housing, which cost $400 as a one-off. Its label: "Machining: the flexible friend. One part, no mold. Expensive at scale, invaluable for proof." He calls this triptych "the sermon on the mount" and shows it to every customer who asks about transitioning from prototype to production.

A Short Checklist for Process-Sensitive Design

If you're designing a part and you're not sure whether it will be machined or die cast, ask yourself these questions:

1. What is the annual volume? This is the single most important question. It often determines the process.

2. Are all walls drafted for mold release? If not, and the part is headed for die casting, add draft now.

3. Is the wall thickness reasonably uniform? If not, a casting will likely have sink marks, voids, or cracks.

4. How many undercuts? Each one adds a side action to a die casting mold.

5. What are the critical tolerances? Identify which features need secondary machining and which can be as-cast.

6. What is the cosmetic requirement? A machined look and a cast look are different. Decide which one you want, and design for that process.

7. What is the lead time? If you need parts in 4 weeks, die casting is probably out of the running.

The partnership between design and manufacturing is never more important than when choosing between these two processes. A good machine shop can advise on machinability; a good die caster can advise on castability. Involve both early, and you'll end up with a part that works in production, not just in CAD.

Old Li, who has now seen hundreds of parts transition between processes, says: "The designer imagines the part. The process imagines the cost. The two imaginations have to meet somewhere in the middle. The best designs are the ones where the part and the process were introduced before the ink was dry." Then he goes back to inspecting a freshly machined casting, checking that the secondary bores are concentric to the as-cast features. The hybrid part is where many products land, and it works beautifully — when both processes are respected from the start.

Have you ever redesigned a machined part for die casting and watched the per-piece cost plummet? Or fought a casting design that kept warping because the walls weren't uniform? I'd love to hear your process-transition war stories in the comments — we're all learning the delicate dance between subtractive and formative.