Key takeaways
- Die casting fills a steel die in milliseconds, so wall thickness is a flow variable before it is a strength variable.
- Draft is not a tolerance; it is the angle that lets the casting leave the die without dragging.
- Thin walls, sharp corners and uneven sections create cold shuts, porosity and warpage in that order.
- Design the machining allowance and the ejector and gate marks into the drawing, because they cannot be removed later without cost.
What the process does
Aluminium die casting injects liquid metal into a hardened steel die under high pressure. The die is a two-part tool with a cavity, a runner, a gate and overflow wells, and it opens on a parting line. The metal fills the cavity in milliseconds, solidifies against the die wall, and is ejected as a near-net shape with gates, runners and flash attached.
The process is fast and repeatable, and the tool is expensive. That combination sets the volume band. A die casting is economical when the tool can be amortised over tens of thousands of parts or more, and it is a poor fit for a prototype unless the geometry is already stable and the programme is funded.
Compared with sand casting, die casting holds a thinner wall, a better surface and a tighter as-cast tolerance. Compared with machining from solid, it produces a shape closer to the finished part with far less metal removal. The design rules below are the price of those advantages.
From melt to trimmed casting
The sequence is short, but every step leaves a mark on the part or on the drawing.
- 01
Melt and degas
The alloy is melted and treated to remove dissolved gas. Hydrogen left in the melt becomes porosity in the casting, so the melt quality is the first control point.
- 02
Slow shot
The plunger pushes metal through the shot sleeve at low speed to avoid trapping air ahead of the wave.
- 03
Fast shot and fill
The cavity fills in milliseconds through the gate. Gate position and thickness decide where the metal arrives last and where the flow marks sit.
- 04
Intensify and solidify
Pressure is held while the casting skin forms and the section solidifies. Thick sections cool last and shrink away from the die.
- 05
Open, eject and trim
The die opens, ejector pins push the part out, and a trim press removes the runner, the overflow and the flash.
- 06
Machine and finish
Critical faces, holes and threads are machined after casting. The casting must leave enough stock for that operation.
Alloy choice sets the baseline
A380, known in the Japanese designation as ADC12, is the workhorse die casting alloy. It fills well, casts thin sections and is inexpensive, at the cost of some ductility and corrosion resistance. A360 and its relatives give better ductility and corrosion resistance with slightly lower fluidity. AlSi9Cu3(Fe), the EN AC-46000 family, covers a similar ground in European practice.
| Alloy | Character | Typical parts |
|---|---|---|
| A380 / ADC12 | Fills well, casts thin walls, economical | Housings, covers, general parts |
| A360 | Better ductility and corrosion resistance | Parts exposed to moisture or bending |
| AlSi9Cu3(Fe) | European family, good castability | Machine covers and structural parts |
Descriptions are typical, not a substitute for the mill certificate and the mechanical requirement.
Wall thickness is a flow rule
A die casting wall has to fill before it freezes. A thin wall cools quickly and may never fill at the far end of the cavity, which shows as a cold shut or a missing corner. A thick wall fills easily and then cools slowly, which produces a shrink cavity in the centre and a sink mark on the surface.
The usual band for aluminium die casting is 1.5 to 3 mm, with 1 mm achievable on a small part in a well-controlled die and 4 mm or more reserved for structural sections that are designed for it. These are illustrative bands, not limits. The real limit depends on the alloy, the flow length, the gate and the die temperature.
The more important rule is uniformity. A part with a 2 mm wall next to a 6 mm boss will have a hot spot at the boss and a sink on the opposite face. The fix is a gradual transition, often at 3:1 or 4:1, and a rib or a core that removes metal rather than adding it.
Draft and fillets
Draft is the taper on every surface that moves against the die. Without it, the casting drags, scuffs or cracks as it is ejected. The usual call is 1 to 3 degrees on a machined or as-cast wall, with 0.5 degrees possible on a simple, shallow core and more needed on a deep cavity or a textured surface.
Inside surfaces need more draft than outside surfaces, because the casting shrinks onto the core as it cools. A deep core with too little draft will grip and tear. Textured surfaces need extra draft because the texture itself creates undercuts at a microscopic scale, and a sandblast or a coarse texture can add a degree or more to the requirement.
Fillets do the same job for stress and flow. A sharp internal corner is a stress riser, a hot spot and a place where the metal hesitates. A fillet radius of about half the wall thickness is a common starting point, and a larger fillet at a boss or a rib root reduces both the stress and the sink.
Draft is not a tolerance
A dimension can be met without draft, but the casting cannot leave the die. Check the draft on every vertical face, including the small ones.
Ribs, bosses and the marks the die leaves
A rib adds stiffness without adding a thick section. The rule is to keep the rib thinner than the wall it meets, typically at 50 to 70 per cent of the nominal wall, and to add a fillet at the root. A rib as thick as the wall creates a hot spot at the intersection and a sink on the opposite face, which is the problem the rib was meant to solve.
A boss is a local thick section, so it carries the same risk. A boss wall of about half the nominal wall, with a cored hole and a fillet at the base, cools more evenly than a solid boss. A boss that stands free should be tied to a rib or a wall, because an isolated boss is a shrinkage defect waiting for a machining cut to expose it.
The die also leaves marks. Ejector pin marks sit on the face the pins push against, gate and runner marks sit where the metal entered, and the parting line sits where the two die halves meet. These are not defects, but they are features. Put them on a non-cosmetic, non-sealing face in the drawing, or expect to pay for a second operation to remove them.
Porosity, gating and the machining allowance
Porosity in a die casting comes from gas trapped during fill, from shrinkage as a thick section cools, or from a cold shut where two flow fronts meet without welding. The first is controlled by the shot profile and the venting, the second by wall uniformity and intensification pressure, and the third by gate position and die temperature.
The design response is to keep the machined surfaces out of the last-to-fill and last-to-solidify regions where possible. If a sealing face or a threaded hole must sit in a thick section, expect a higher reject rate and specify a pressure test or a radiographic check. The article on porosity in this section covers the defect types and the acceptance methods in more detail.
The casting also needs machining stock. A machined face usually needs 0.5 to 1 mm of stock, and a machined bore needs enough to clean up the draft and the distortion. Too little stock leaves a black skin or a hard spot that damages the tool. Too much stock adds cycle time and exposes more porosity.
What the drawing should show
Show the parting line, the gate position if it is fixed, the ejector mark areas and the surfaces that must not carry a mark. Show the machining allowance on every machined face and the as-cast tolerance separately from the machined tolerance. State the alloy, the heat treatment if any, the porosity acceptance and the pressure test.
Add the draft on the drawing, or state a default and mark the exceptions. A supplier will add draft whether or not it is shown, and a part designed without it will be quoted with a correction that changes the geometry.
Frequently asked questions
What is the minimum wall thickness for aluminium die casting?
Typically 1.5 to 3 mm, with around 1 mm possible on a small, simple part in a well-controlled die. The limit depends on the alloy, the flow length and the gate, so confirm it with the caster for the specific geometry.
How much draft does a die casting need?
About 1 to 3 degrees on most surfaces, 0.5 degrees on a simple shallow core, and more on deep cores and textured faces. Inside surfaces need more than outside surfaces because the casting shrinks onto the core.
Why does a die casting have sink marks opposite a boss?
A boss is a thick section that cools last. As it shrinks it pulls the opposite wall inward, leaving a depression. A thinner boss wall, a cored hole and a fillet at the base reduce the effect.
Can die casting be used for a prototype?
It can, but the tool cost usually makes it a poor choice for a one-off. Prototype quantities are better served by sand casting, gravity casting or machining from solid until the geometry is stable.
Sources and further reading
- ISO 8062-3, Geometrical product specifications for moulded parts, casting tolerances
- EN 1706, Aluminium and aluminium alloys, castings, chemical composition and mechanical properties
- Qumek engineering desk notes on aluminium die cast and machined parts
Qumek Engineering Desk
Engineering team
The engineering team behind Qumek drawings, DFM notes, tolerances and inspection standards. Every guide is reviewed against the drawings and processes used on live programmes.
Have a die casting drawing before tooling?
Send the model and the volume. The engineering desk will reply with the wall, draft and stock changes that lower the risk before the die is cut.
Send a drawing