Design for Manufacturability:
8 Rules for Aluminium Die Casting

Non-uniform wall thickness is the single most common cause of porosity and distortion in die castings. When thick sections adjoin thin sections, the thin section solidifies first, restricting feed to the thick section as it contracts — creating shrinkage cavities.

Target wall thickness of 2.0–3.5 mm for HPDC aluminium. Where thick sections are functionally necessary, use coring (internal voids) to reduce the section mass. Ribs are an effective way to add stiffness without increasing wall thickness — a ribbed thin wall is stiffer than a uniform thick wall of equivalent mass.

SAPL's DFM review flags every section transition greater than 3:1 ratio as a potential porosity risk.

Draft is the taper applied to vertical surfaces to allow the casting to be pulled clear of the die without scoring or sticking. Without adequate draft, ejection forces damage the casting surface and accelerate die wear.

Minimum draft for external surfaces (die cavity): 1.0–1.5°. Minimum draft for internal surfaces and cores: 2.0–3.0°. Textured or polished surfaces require additional draft — typically 1° per 25 µm of surface depth.

Zero-draft surfaces — flat sidewalls perpendicular to the parting direction — require slides in the die. Slides are mechanically complex, add cost, and reduce die life. Where zero draft is specified for functional reasons (seating faces, assembly datums), restrict it to the minimum necessary feature length.

The parting line is the plane at which the two halves of the die meet. Its position determines which surfaces will show a parting line witness mark and which features can be formed in each half of the die. The parting line also defines the ejection direction, which governs the draft angle requirements.

Ideal parting line placement: at the maximum perimeter of the component in the pull direction, avoiding critical sealing or mating surfaces, and keeping all critical dimensions within one half of the die (not crossing the parting line). SAPL's tool design team proposes a parting line during DFM review and discusses it with the customer before committing to die machining.

An undercut is any feature that prevents the casting from being pulled clear of the die in the primary ejection direction — a side hole, a groove, or a recessed lug. Each undercut requires a slide (also called a side action or cam) in the die to form and retract before ejection.

Slides increase tooling cost by 20–40% per action. They also introduce additional wear surfaces and potential for flash. Where possible, redesign undercut features as: - Machined features (drill the hole after casting) - Open slots rather than closed holes - Features accessible from the parting line direction SAPL's DFM review highlights every undercut and proposes alternatives where feasible.

Sharp internal corners create stress concentrations in the die steel — particularly problematic at areas of rapid temperature cycling. Thermal fatigue cracking (heat checking) starts at sharp corners and progresses into the die face, eventually transferring the crack pattern to the casting surface.

Minimum fillet radius at all internal corners: 0.5 mm. Preferred: 1.5 mm or greater for structural features. For corners in areas of high thermal loading (near gates, runners, and heavy sections), 3.0 mm or greater is recommended.

External corners on the casting (internal corners of the die) should be chamfered or radiused to prevent chipping of the die steel at thin die sections.

Features that straddle the parting line inherit an additional source of dimensional variation — parting line mismatch (flash or mismatch between the two die halves). Even with well-maintained tooling, parting line mismatch of 0.1–0.2 mm is typical.

For critical dimensions — bore diameter, bearing seat, sealing groove — locate the feature entirely within one half of the die. Where this is geometrically impossible, specify a machined finish on the critical surface so the machining operation absorbs the casting variation.

Ejector pins push the casting out of the die after each shot. They leave a witness mark (a circular impression or raised disc) on the casting surface. On functional surfaces — sealing faces, mating surfaces, visible A-surfaces — ejector pin marks are not acceptable.

Discuss ejector pin location with SAPL's tool design team early. Pins should be placed on non-functional surfaces, in overflow pockets, or on runner break-off tabs. If the component geometry forces pins onto a functional surface, the pin diameter and position should be agreed before tooling is started.

The most common cause of DFM iteration delay is receiving a 3D model without an annotated 2D drawing. The 3D model defines geometry; the 2D drawing defines: - Critical dimensions and tolerances - Surface finish requirements - Material specification and alloy designation - Treatment requirements (powder coat colour, masking areas) - Acceptance criteria (porosity standards, cosmetic grade)

SAPL conducts full DFM analysis on receipt of both STEP and annotated 2D drawing. DFM feedback is provided within 72 hours for standard components.