Aluminum die casting turns out strong, dimensionally stable metal parts in seconds per shot, which is why it dominates high-volume housings, brackets and gearbox covers. What decides whether those parts come out cheap and clean or late and full of scrap is rarely the casting machine — it is the geometry you hand the foundry. Below are the four design levers that drive most die casting cost, lead time and defect rates: draft, wall thickness, porosity management and machining allowance.
Draft Angle: The Cheapest Insurance in the Process
Every wall perpendicular to the parting line needs draft — typically 1 to 3 degrees for aluminum alloys. Shallow, short features can survive on 0.5 degrees; deep cores and internal bosses usually want 2 degrees or more, because the casting shrinks onto the steel core as it solidifies and grips it. Zinc parts, cast at lower temperatures, often get away with 0.25 to 0.5 degrees.
If a visible face will be textured, add roughly 1 degree of draft per 0.025 mm (0.001 in) of texture depth. Designers who skip this end up with scored surfaces, galled cores and slower cycles — the ejector half pays for it on every single shot. Draft is free in CAD and expensive to add later, when the tool steel is already cut.
Wall Thickness: Uniform Beats Generous
The instinct to "make it stronger by making it thicker" is backwards in die casting. Aluminum alloys such as A380 and ADC12 fill best and solidify most evenly between roughly 1.5 and 4 mm. Sections above about 6 mm cool slowly, feed badly and pull shrinkage porosity into exactly the places you cannot inspect. Thick walls also stretch cycle time — the metal has to freeze before the die can open.
Where stiffness is the goal, rib it instead. A rib at 50–70 percent of the adjoining wall thickness adds more rigidity per gram than any slab of extra metal, without creating a hot spot. When a thickness step is unavoidable, transition gradually — a good rule of thumb is a ramp length at least three times the step height. Cored-out bosses around fastener holes, rather than solid ones, apply the same logic where screws load the part.
Porosity: Why It Happens and What Actually Fixes It
High-pressure die casting injects metal fast, and it traps things on the way in: air from the cavity, occasionally vapour from the lubricant. Add shrinkage in heavy sections and you get porosity — small voids that are a normal feature of the process, not automatically a defect. What actually helps:
- Uniform walls with ribs instead of thick sections — most shrinkage porosity is invited by the geometry, not by the foundry.
- Overflow wells and vents at the last places the metal fills, so oxides and trapped air land in sacrificial metal instead of your part.
- Vacuum-assist systems on the die for critical, thin-walled or cosmetic castings.
- Vacuum impregnation after casting when the part must hold air or fluid — standard practice for housings that see pressure testing.
- X-ray or CT spot checks on structurally loaded parts, specified only where the load case justifies the cost.
One trap worth flagging: machining into a thick section can open subsurface porosity that was invisible as-cast. If a face has to be both machined and pressure-tight, say so on the drawing. The foundry can shift metal feeding, add local die cooling or plan an impregnation step — far cheaper than discovering the leak at your final test.
Machining After Casting: Leave Stock, but Not Too Much
As-cast tolerances are decent — as a rough guide, think ±0.1 to ±0.25 mm on small features, opening up as the casting grows — but bearing bores, sealing faces and dowel holes almost always need a finishing pass. The knife edge here is machining stock. Leave too little and the cutter only skims the hard cast skin; leave too much and it digs through the dense surface layer into the porous zone beneath.
Around 0.3 to 0.8 mm of stock on critical faces is the usual working window, with the lower end preferred on flat sealing faces. Datum strategy matters just as much: fixture on as-cast surfaces where possible and reference machined features to one another, so the tolerance stack does not fight the casting's own variation. Small internal threads are another common miss — below roughly M4, it is usually better to tap after casting or use a cast-in insert than to expect clean threads straight from the die.
When those finishing passes have to hold tighter than ±0.02 mm, the standard route is pairing the cast blank with CNC machining on the critical features and letting the die carry everything else.
Alloys: The Choice That Quietly Reshapes the Design
A380 — often sold in Asia as ADC12 — is the workhorse: an Al-Si-Cu alloy with excellent fill, good as-cast strength and reasonable machinability. It is the default for housings, brackets and motor end bells. A360/AlSi10Mg trades a little machinability for better ductility and corrosion resistance, which suits thin, complex or outdoor-exposed parts.
Zinc (Zamak 3 and 5) casts at lower temperature, holds sharper detail, supports thinner walls — often down toward 1 mm — and plates beautifully, at the cost of weight and a lower service temperature. Magnesium AZ91D wins on mass when every gram counts, but demands more respect around wall thinness and handling.
A caution that surprises many teams: high-pressure castings are generally not solution heat treated the way sand or permanent-mold castings are, because trapped gas can blister the surface at solution temperatures. If your application assumes T6-type properties, raise it early in the design conversation — the alloy or the process may need to change.
A Pre-Quote Checklist
- Draft on every wall normal to the parting line: 1–3° for aluminum, more on deep cores, plus texture allowance.
- A wall-thickness map: ribs replacing thick sections, gradual transitions, cored bosses.
- Sealing and machined faces called out explicitly, with stock allowance and leak-test requirements.
- Datums that fixture on as-cast surfaces, not on features the die cannot hold.
- Tolerances split honestly between as-cast and machined features.
- Alloy named by designation — A380, ADC12, Zamak 5 — not just "aluminum".
None of this is exotic; it is the same handful of decisions on every cast part, made before tooling is cut. Getting them right is what separates a quote that lands on time at a sane price from one that grows a change-order chain. If you want a second pair of eyes on a casting design, our die casting team reviews draft, walls and fill behaviour as part of every quotation.
