Designing Aluminum Castings: Design Rules That Reduce Cost and Scrap

An aluminum casting is inexpensive and repeatable when it has walls that are as uniform as possible, gentle transitions, draft angles matching the mold ejection direction, and as few cores as possible. These features are determined by the designer: according to the academic textbook "Odlewnictwo" (WNT), design accounts for about 7% of the product cost, yet as much as 65% of the influence on that cost. We have gathered the rules worth checking before the model goes to the foundry.

In brief

• Minimum wall thickness depends on the process: 3–6 mm in a sand mold, 2.5–5 mm in a permanent mold, and 0.7–1.5 mm in die casting.
• Design internal walls about 20% thinner than external ones, and keep the thickness ratio of adjacent walls within 2:1; ease larger differences with a taper of no more than 1:4.
• Approximate draft angles: sand mold about 2° (minimum about 1°), die casting about 2° on internal walls and about 1° on external ones; shallow features and permanent molds require larger angles.
• Wall intersections, T-joints without relief and massive thick sections create hot spots, a frequent source of shrinkage cavities and leaks.
• Every additional core, undercut and second parting plane raises tooling cost. In metal molds, cores should share a common pull direction.

Why does design determine the cost of a casting?

A full breakdown from the same source shows where cost is incurred and where it is decided:

Stage	Share of product cost	Influence on product cost
Design	7%	65%
Production	33%	19%
Materials	40%	15%
Administration	20%	1%

Decisions on material and process are made at the design stage, and the process engineer's later choices have relatively little effect on cost. It is therefore worth checking design-for-manufacturability rules before ordering molds and patterns. We describe the cost, service life and ownership terms of these tools in the article on patterns, permanent molds and die casting dies.

Manufacturability rules are grouped by purpose: making the tooling and molds, filling the mold with metal, feeding the casting, limiting stresses, and cleaning.

Wall thickness: minimum for each process and uniform distribution

Minimum wall thickness is the limit below which the metal may not fill the mold. The textbook gives the following for aluminum alloys:

Casting method	Minimum wall thickness	Notes
Sand mold (bentonite-bonded sand)	3–6 mm	value given for non-ferrous metals
Permanent mold	2,5–5 mm	2.5 mm for small surfaces, 5 mm for larger ones
Die casting	0,7–1,5 mm	0.7 mm for small parts, 1.5 mm for medium-sized parts

The minimum is not a recommendation. A wall that is too thin risks misruns, and a large flat wall also risks cold shuts. Thickening the wall helps, and for a large flat wall, so does inclining it.

The other extreme is walls that are too thick. Thicker sections cool more slowly, have a coarser structure and lower properties, and massive areas are prone to shrinkage porosity. How wall thickness translates into strength is explained in the article on the mechanical properties of aluminum castings.

Three proportion rules:

• Internal walls about 20% thinner than external ones (Y = 0.8X). The interior of a casting loses heat more slowly, so a thinner wall evens out cooling.
• A rib at its base no thicker than about 80% of the wallit grows from. A thicker rib creates a hot spot at the junction.
• Thickness ratio of adjacent walls up to 2:1. When a larger difference is unavoidable, join the sections with a taper of no more than 1:4. The taper should be at least four times longer than the thickness difference. An alternative is to split the part into two castings.

Build stiffness with ribs rather than mass. Ribs and ties also stiffen sections prone to cracking and distortion.

Transitions, fillets and hot spots

A hot spot is a location where more metal collects than in the surrounding area. It solidifies last, so there is no liquid metal left to compensate for shrinkage, and a shrinkage cavity or porosity forms.

Risky design	Better design	Why is
Wall intersection (X junction)	offset junction (Z type), hexagonal grid or a ring at the junction	less metal concentrated in one place
T junction with a sharp corner or a fillet radius alone	a coring-out (recess) at the junction	without a recess at the junction, a shrinkage cavity forms; a core at the junction works but is uneconomical
Abrupt transition from a thick to a thin wall	gradual, rounded transition	lower risk of cracking and warping
Straight arms and large flat walls	curved arms, curved or sloped walls	lower casting stresses
Massive thick section far from the riser	junction moved toward the riser, or a feeding rib	directional solidification, easier feeding

Fillets at wall junctions are practically mandatory in castings. The radius is chosen in proportion to wall thickness: too small promotes cracking, while too large creates a local hot spot of its own. It is best to agree specific radii with a process engineer for the given method and alloy.

Hot spots are easy to find with the inscribed circle method: circles are drawn in the walls and junctions of the model's cross-section. The larger the circle that fits in a junction compared with the adjacent wall, the higher the risk of a shrinkage cavity. Porosity at junctions is also a common cause of leaks – we write about this in our article on leak tightness of aluminum castings.

Draft angles and shrinkage

Draft is the taper of walls parallel to the direction in which the pattern is withdrawn from the mold or the casting is ejected from a metal mold. Without it, the pattern damages the sand mold on withdrawal, and the casting jams in the permanent mold or die.

Method	Approximate draft	Notes
Sand mold	approx. 2°, minimum approx. 1°	external and internal walls
Permanent mold	approx. 3° at a depth of 25–127 mm	shallower features 5–10°, deeper than 127 mm approx. 2°; holes formed by steel cores 3–10°
Die casting	approx. 2° internal, approx. 1° external	at depths from approx. 25 mm; in precision work approx. 1° and 0.5°; at a depth of 10 mm approx. 3° internal

The values for die casting come from NADCA recommendations, for permanent molds from a permanent mold casting manufacturer's guide and AFS, and for sand molds from typical design recommendations. They are starting points, not standard requirements.

Internal walls need more draft than external ones, because the cooling casting shrinks and grips the cores and protrusions of the mold. The 2023 edition of ISO 8062-3 introduced draft angle tables for individual methods (tables 2–6). How draft angles and machining allowances relate to dimensional tolerances is described in our article on casting tolerances according to ISO 8062-3. Draft angles, the parting plane and the direction of withdrawal are indicated on the drawing according to ISO 10135.

After cooling, the casting is smaller than the mold cavity, so tooling is made oversize by the shrinkage allowance. For aluminum alloys, a typical value is about 1.2% (range 0.8–1.5%), and less for die casting – for example, about 0.6% is given for the American alloy A380. In a metal mold, and where the cores restrain shrinkage, shrinkage is lower than in a sand mold. On the part drawing you specify nominal dimensions, and the foundry accounts for shrinkage when designing the tooling.

Parting plane, cores and undercuts

The least expensive casting has a single, flat parting surface and dimensions that can be produced from one mold half. This means shorter molding time, a cheaper pattern set and better accuracy, because mold half shift does not affect the dimensions.

Cores are separate tooling and a separate operation. This is easy to see in the example of one part in three versions: with three cores (most expensive), with one, and with no cores (least expensive). Simple outlines and open designs make molding easier and reduce the number of cores.

Permanent molds and die casting dies are subject to additional rules:

• metal cores should share a common pull direction,
• avoid undercuts in outer walls that are parallel to the parting plane, because they require side cores,
• extend ribs and thickened sections all the way to the parting plane or move them to the outer walls,
• keep in mind that an undercut that a core can solve in a sand mold may be difficult or impossible to produce in a metal mold.

In a sand mold, a core must be supported on two sides, and deep pockets in bentonite-bonded sand are hard to compact evenly. For bentonite-bonded sands, a rough rule is that pocket depth should not exceed half its width when the pocket is closed on four sides, one width with three walls, and three widths with two (h/a = 0.5 / 1.0 / 3.0). A deeper pocket usually means a core. For more on compaction, see the article on molding sands, and for core technologies, see the text on foundry cores.

Cast holes: when to use a core and when to drill

A cast hole saves machining, but its depth is limited by its diameter. Approximate limits according to NADCA recommendations for aluminum die casting:

Hole diameter	Maximum depth	Depth / diameter
3,2 mm	approx. 8 mm	approx. 2.5
6,35 mm	approx. 25 mm	4
12,7 mm	approx. 51 mm	4
19 mm	approx. 114 mm	6
25,4 mm	approx. 152 mm	6

These are recommended maximum values, not the limits of any particular foundry. In a permanent mold, holes with a diameter below approx. 6 mm are usually impractical to cast, and holes of approx. 3 mm and smaller are made only in special cases, on fixed pins. When a hole is too deep relative to its diameter, the core is inserted from both sides. Closely spaced holes are usually not cast.

In sand molds, the limits depend on the type of core, so agree on them with the foundry, and plan small holes for drilling from the start.

Flash, risers and cleaning

Part of a casting's cost is cleaning: removing flash, the gating system, risers and core sand. Design can reduce it:

• orient the casting so that flash falls on machined surfaces – it will disappear together with the machining allowance,
• design flat riser locations, because the remnant of a flat riser is removed without contour machining,
• route flash along flat external surfaces, because it is removed much faster there than in cavities,
• position holes so that burnt-on sand can be easily removed from cavities.

Provide a machining allowance on machined surfaces, and choose measuring datums away from the parting line.

Checklist before sending a model to the foundry

1. Walls no thinner than the minimum for the chosen method and as uniform as possible; internal walls approx. 20% thinner than external ones.
2. Thickness differences up to 2:1, tapered transitions no steeper than 1:4, rounded corners.
3. No X-junctions or massive thickened sections; T-junctions with a cutout.
4. Draft on all walls parallel to the ejection direction, greater on internal walls.
5. One flat parting surface and critical dimensions in a single mold half.
6. As few cores as possible; in metal molds, a common pull direction and no undercuts parallel to the parting plane.
7. Deciding which holes to cast and which to drill.
8. Marked machined surfaces and datums; gates and risers on machined or flat surfaces.
9. 3D model (e.g., STEP) and a drawing with tolerances, alloy grade and planned quantity.

The 3D model is useful for more than quoting: it is the basis for producing tooling on CNC machines and for casting process simulation.

Frequently asked questions

We will review your model before tooling is made

Send us a 3D model and a drawing. A process engineer will assess walls, draft angles, cores and the parting plane, and we will prepare the casting pattern as part of modeling and prototyping – also based on a 3D scan of an existing part. We will produce castings, among others, in permanent molds or by high-pressure die casting. Send the model for analysis.

Sources and standards

• M. Perzyk (ed.), Casting, WNT, Warsaw – ch. 3.2 (Fig. 3.28, Tables 3.11–3.16, pp. 163–179), 3.3 (Table 3.20, pp. 185–186), 3.4 (process selection, pp. 190–194), 5.2.2 (gaps in bentonite-bonded sand, p. 276).
• ISO 8062-3:2023 – general dimensional and geometrical tolerances and machining allowances for castings; casting draft angle tables 2–6.
• ISO 10135:2007 (EN ISO 10135:2009) – indication of molded parts in technical documentation (draft angles, parting plane).
• NADCA (North American Die Casting Association) – design recommendations for die castings: draft angles and cast holes.
• AFS (American Foundry Society) – "Designing Aluminum Permanent Mold Castings", Casting Source 2019 (based on "Aluminum Casting Technology", 3rd ed.).
• Batesville Products – Design Guide for Permanent Mold Aluminum Casting (2024) – draft angles in permanent molds as a function of depth.
• M. Finke, Formelsammlung Gießereitechnik, 2nd ed., Verlag Europa-Lehrmittel, 2023 – casting shrinkage of aluminum alloys.
• Eazall, A380 alloy data sheet – die casting shrinkage 0.006 in/in (0.6%).