Why Tolerances Matter in Die Casting
Die casting can hold tight dimensions, but the tolerance you specify directly drives tooling cost, cycle time, and scrap rate. A part that needs ±0.05 mm across a 200 mm span will cost noticeably more than one that can live with ±0.15 mm. The trick is knowing where the process is naturally strong and where you are asking it to fight physics.
Aluminum die casting (A380, ADC12) typically delivers ±0.1 mm on small features up to about 75 mm. Beyond that, thermal shrinkage and mold wear push you toward ±0.15–0.2 mm. Zinc alloys (Zamak 3) shrink less and hold closer—often ±0.05 mm on similar dimensions—so if precision is the priority, material choice is your first lever.
Magnesium alloys (AZ91D) sit in between: roughly ±0.08 mm on small features, with the advantage of lower density for weight-sensitive parts. The downside is faster tool erosion and more aggressive oxidation, so shops often add protective coatings to the mold cavity after 20,000–30,000 shots.
Linear Tolerance Bands by Feature Size
Most shops quote to NADCA (North American Die Casting Association) standards. Here is the practical breakdown for aluminum:
- 0–25 mm: ±0.05 mm (critical fits only)
- 25–75 mm: ±0.10 mm (standard commercial)
- 75–150 mm: ±0.15 mm
- 150–300 mm: ±0.20 mm
- Over 300 mm: ±0.25 mm or negotiate
These numbers assume a single-cavity die with normal gating. Multi-cavity tools add cavity-to-cavity variation of 0.03–0.08 mm, which you must either design around or pay for tighter process control. If you are running a four-cavity tool and need all four parts to interchange, specify ±0.05 mm on mating dimensions and let the shop add process monitoring rather than hoping.
Hole and Thread Tolerances
As-cast holes in aluminum are rarely precise enough for press fits. A cored hole will typically be ±0.08 mm and may taper slightly because the core heats unevenly. If you need H7 tolerance, plan on CNC machining the hole afterward. That is standard practice, not a failure of the casting process.
Threads are almost always machined in a secondary operation. As-cast threads are possible with special collapsible cores, but the pitch accuracy is poor and the surface finish is rough. For production volumes, machining adds pennies per part and saves hours of assembly headache. A 6 mm coarse thread machined after casting costs about $0.02–0.05 per hole in volumes above 5,000 pieces.
Blind holes need extra attention. The trapped air at the bottom of a blind cored hole can create porosity that weakens the thread. Machining 1.5× the thread depth beyond the nominal bottom clears the porous zone and gives a reliable engagement length.
Flatness, Straightness, and Warpage
Thin walls cool faster than thick sections, so flatness is where die casting hurts most. A 200 × 100 mm cover with 1.5 mm walls may bow 0.3–0.5 mm unless the die has excellent cooling balance. NADCA recommends 0.15 mm per 25 mm of length for standard parts, and 0.08 mm per 25 mm for precision-grade work.
Straightness on long ribs or bosses follows similar rules. If you need a 150 mm rib straight within 0.1 mm, consider adding machining stock or switching to CNC machining for that feature. Another option is to add stiffening ribs on the non-critical side: a 2 mm rib every 30 mm can cut bow by 40 % without touching the tolerance spec.
Warpage is also sensitive to ejection temperature. If the part is still 250 °C when the ejector pins push it out, it will sag under its own weight. Most shops target 180–200 °C for aluminum ejection, which means cooling time is 8–15 seconds for 2 mm walls and 20–30 seconds for 5 mm walls.
DFM Rules That Buy You Tolerance
You cannot tighten process variation without paying for it, but you can design so the variation matters less:
- Uniform wall thickness: Keep walls within a 2:1 ratio. Thick sections sink and thin sections warp. A 4 mm boss on a 1.5 mm wall will create a visible sink mark 80 % of the time.
- Draft angles: 1° per side on vertical walls, 2° on deep cores. Less draft means more ejection force and more distortion. For textured surfaces, add 1° extra draft per 0.025 mm of texture depth.
- Radii: Internal corners need at least 0.5 mm radius. Sharp corners concentrate stress and crack during solidification. A 0.2 mm internal corner is a reject waiting to happen.
- Machine stock: Leave 0.3–0.8 mm on mating surfaces that need tight fits. It is cheaper to machine a flat face than to hold ±0.05 mm across a whole casting. For bearing bores, 0.5 mm stock is typical; for sealing faces, 0.3 mm is enough.
When to Move Tolerances to Secondary Machining
Die casting excels at complex 3D shapes and thin walls. It does not excel at mirror-flat surfaces or bearing bores. A good rule of thumb: if a dimension appears on a mating drawing with a GD&T tolerance tighter than ±0.05 mm, plan on machining it. The combined process—cast near-net, then machine critical features—usually beats trying to hold everything in the mold.
At Protom, we review tolerance stacks before cutting steel. Moving one bore from as-cast to machined can save weeks of tool rework and cut scrap from 8 % to under 2 %. If you are unsure which faces need machining, send us the drawing and we will flag the high-risk dimensions.
One last point: always specify which datum features are as-cast and which are machined. A machinist who assumes the mounting face is flat when it is actually bowed 0.2 mm will compensate in the wrong direction and scrap the part. Clear datums on the drawing prevent that conversation.
