A new die-cast aluminum housing for a gear motor showed up at the assembly line with cracks around the bearing bosses. The die was freshly cut, the part came out of the die clean, and the crack appeared after the trim press. The casting engineer blamed the trim die. The die maker blamed the part design. The part design was the problem — the wall thickness transitioned from 6 mm at the boss to 2 mm at the web with no blend. The trim press just found the weak spot.
The wall thickness rule that comes first
Die casting works because molten aluminum fills the die and solidifies under pressure. The cooling rate is what drives the design rules. A 6 mm wall takes about 4x longer to solidify than a 3 mm wall (cooling time scales with the square of thickness). When thick and thin sections sit next to each other, the thin section freezes first, the thick section freezes later and shrinks, and the interface pulls. If the transition is sharp, it cracks.
The rule of thumb for aluminum die casting: keep wall thickness between 1.5 mm and 4 mm. Below 1.5 mm the metal won’t fill the cavity completely (especially at distance from the gate). Above 4 mm the porosity risk goes up — the center of the thick section shrinks as it solidifies and pulls a void. For the housing in question, the 6 mm boss was fine as a boss, but the step to 2 mm web needed a fillet of at least 1.5 mm radius, ideally a tapered transition over 10 mm. The die was cut without either.
Draft angles: why parts stick
Every surface perpendicular to the die opening needs draft — a small angle that lets the part release from the die. Without draft, the part locks in the die and the ejector pins either bend it or the die scratches the part on ejection.
| Surface type | Minimum draft (aluminum) | Typical production value |
|---|---|---|
| External walls | 0.5° | 1.0-1.5° |
| Internal walls (core side) | 1.0° | 1.5-2.0° |
| Deep ribs and fins (depth > 5x width) | 1.5° | 2.0-3.0° |
| Bosses (outer) | 0.5° | 1.0° |
| Bosses (inner hole) | 1.0° | 1.5° |
| Textured surfaces | +1.0° over base | 2.0-3.0° total |
The housing in question had zero draft on the internal bearing pockets. The ejector pins pushed the part out anyway — aluminum is forgiving enough on a fresh die. But every cycle scuffed the pocket. After 5000 cycles the pockets were 0.1 mm oversize and the bearing fit was loose. The die had to be reworked with 1.5° draft added, which changed the bearing seat diameter and forced a re-certification of the housing.
Shrinkage and the die size
Aluminum shrinks about 0.5-0.7% (linear) from the molten state to room temperature. The die cavity is cut oversize by that amount. But shrinkage isn’t uniform — it’s affected by die temperature, section thickness, and how fast the part cools. A part with uneven sections shrinks unevenly. The die maker compensates with a single shrinkage factor, but the smart ones add a second, local factor for thick sections.
For the housing, the nominal shrink factor was 0.6%. The thick bosses shrank more like 0.7%, the thin webs more like 0.5%. The bearing bore, machined after casting anyway, was fine. But the bolt holes cast in place — positioned by cores — drifted by 0.1 mm between the bosses and the web. The fix was to cast the bolt holes undersized and drill them in a fixture, or move the holes to the thin web section where shrinkage was predictable. The housing was redesigned to drill all critical holes post-casting.
Ribs: the right way to stiffen
Instead of increasing wall thickness to stiffen a die casting (which adds porosity risk), use ribs. A rib doubles stiffness with a fraction of the material. The rule: rib height up to 3x the base wall, rib thickness 0.6-1.0x the base wall, and rib draft at least 1° per side. The rib base needs a fillet (0.5-1.0 mm) so it doesn’t crack at the transition.
The housing needed a stiffer base plate. The original design was 5 mm thick everywhere — heavy and porosity-prone. The redesign used a 3 mm base with three 8 mm tall ribs. It was 30% lighter and measurably stiffer. The fill time stayed the same, the porosity dropped, and the cracking at the bearing bosses disappeared.
Porosity: what causes it and what to do
Porosity is the die caster’s daily fight. It comes from three sources. Entrapped air — the cavity isn’t fully vented, and the metal traps air pockets. Shrinkage — the thick sections pull voids as they cool. Lubricant vapor — the die spray boils and the vapor gets trapped in the metal.
The design side can help: keep walls even, avoid isolated thick sections, place gates and vents in the right spots (that’s the die designer’s job, but the part geometry dictates where they can go). If a leak-tight part (hydraulic housing, valve body) can’t avoid a thick section, specify vacuum-assisted die casting — the die is evacuated before injection, cutting porosity to near zero. It adds cost per part but eliminates the scrap rate.
Ejector pins and where they mark
Ejector pins push the casting out of the die. They leave small round marks on the part surface. If the part has a cosmetic surface, the ejector pin marks need to be on the inside or in a hidden area. The housing had a logo surface on the outside — the original die put ejector pins on the logo side. Every part had a visible pin mark through the logo. The die was reworked to move pins to the inside of the casting. This is a design consideration: the part designer should mark “no ejector pins on this surface” on the drawing, because the die maker will put them wherever is easiest.
The design review checklist
- Wall thickness 1.5-4 mm, transitions filleted with radius > 1.5 mm
- Draft 1° external, 1.5-2° internal, more on deep features
- Ribs instead of thick walls, rib height < 3x base wall
- Shrinkage factor 0.6% nominal, verify with the caster
- Bosses: outer diameter 2x the hole diameter minimum
- No isolated thick sections (porosity magnets)
- Mark no-ejector surfaces and no-parting-line surfaces
- Critical holes drilled post-cast, not cast to tolerance
The cracked housing wasn’t a die problem. It was a 6-to-2 mm wall step with no fillet. Every rule above traces back to the same physics: aluminum cools at different rates in different sections, and the design either accommodates that or fights it. Accommodating it is cheap. Fighting it costs a die rework.
Die casting design is cooling management. Keep walls 1.5-4 mm, fillet every transition, draft every surface, rib instead of thicken, and drill critical holes after casting. The housing cracked because nobody blended the 6 mm boss into the 2 mm web. The die didn’t cause it, the trim press didn’t cause it — the design did.
