Deciding the tolerance on a die cast part is where design and purchasing most often go back and forth. Too loose and the part will not assemble; too tight and the quote doubles, scrap rises, and the supplier has to machine the feature back into specification. This guide sets out the tolerances the industry actually works to, what moves them, and how to specify them so you pay only for the precision you need.
Most disagreements start with mixing three things together:
As-cast tolerance — what the casting achieves straight out of the die, driven by alloy, size and geometry.
Machined tolerance — what CNC achieves after stock is left on the casting, typically an order of magnitude tighter.
Assembly tolerance — the accumulated stack-up across several parts, which is a different question again.
If a drawing puts ±0.02 mm on an as-cast surface, the supplier has two options: quote a price that includes secondary machining, or decline. Being clear about which of the three you actually need makes the rest of the conversation much shorter.
The most widely referenced basis for high pressure die casting is the NADCA product standard, which splits capability into two tiers:
| Grade | First 25.4 mm (1 in) | Each additional 25.4 mm | Typical use |
|---|---|---|---|
| Standard | ±0.25 mm | ±0.025 mm | General structure, cosmetic faces, non-mating features |
| Precision | ±0.05 mm | ±0.025 mm | Mating faces, sealing faces, bearing seats, locating faces |
Zinc holds tighter than aluminium because it shrinks less and flows better: on the same first inch, roughly ±0.038 mm standard and ±0.02 mm precision. That is why small precision parts and decorative components are usually specified in zinc.
A word on ISO 8062-3: it expresses similar ideas through DCTG grades, but the steps do not map one-to-one onto NADCA. Export projects often reference both, so agree up front which one will be used for acceptance, or first-article inspection becomes an argument.
Treating "die casting tolerance ±0.1 mm" as one number for the whole part is the most common mistake. On a single component the achievable bands differ considerably:
| Feature | Typical reference range | Note |
|---|---|---|
| Linear dimension, as-cast | ±0.10 to ±0.25 mm | Opens up with size, first segment plus increments |
| Parting line mismatch | 0.10 to 0.25 mm | Separate tolerance item, tied to parting line placement |
| Slide / core pull features | ±0.15 to ±0.30 mm | Slide clearance and wear accumulate |
| Flatness | about 0.10 to 0.30 mm over the area | Values are not comparable across different reference areas |
| Hole centre distance | ±0.10 to ±0.20 mm | Hole diameter tolerance is counted separately |
| Draft angle | 1–2° inside, 0.5–1° outside | About 2° per side for blind holes |
| Machined dimension | ±0.02 mm or tighter | Depends on machine, fixturing and process capability |
These are industry reference ranges for judging whether a requirement is reasonable. They are not a commitment by any specific supplier. Real capability must be assessed against the actual part geometry, wall thickness and tooling concept.
Tolerance bands widen with size by physics, not by cutting corners. A 20 mm feature and a 400 mm feature cannot share the same absolute tolerance.
Aluminium (A380, ADC12) and zinc (ZAMAK 3/5) behave differently: zinc shrinks less and holds dimensions better, which is why small precision parts are often specified in zinc. Actual shrinkage also depends on wall thickness and die temperature.
Abrupt wall changes are where sink marks and distortion appear, and where tolerances are lost first. Smooth transitions are the cheapest way to gain dimensional stability.
Parting line mismatch and slide clearances add position error on top of the base tolerance. Keep critical dimensions away from the parting line and the gate area.
Die wear, die temperature variation, intensification switch-over and ejection balance all show up in the measurements. Mid-production drift is usually a tooling and process maintenance issue rather than a design issue.
A practical rule: if a feature is tighter than ±0.05 mm, assume it will be CNC machined after casting. In practice that covers:
sealing faces, O-ring grooves and cover joint faces;
bearing seats, dowel holes and gear shaft bores;
threads and any interface that has to screw together;
locating faces that mate directly with another part.
Stock therefore has to be allowed on the casting, commonly 0.25 to 0.5 mm depending on size and operation. The cost is direct: precision tolerance typically adds 10% to 25% to the part price before machining time, while a DFM review early in the project commonly saves 15% to 20% of the total.
Call out only the critical features. Leave the rest to a general tolerance, stated on the drawing as NADCA Standard or a named ISO 8062-3 grade.
Set datums from the assembly. Datums should reflect how the part is fitted and measured, not where modelling was convenient.
State the draft. 1–2° inside, 0.5–1° outside. Unspecified does not mean unnecessary, it just gets added at trial.
Mark machined faces and stock allowance. Cheaper to write down than to argue about later.
Keep critical dimensions off the parting line and gate. This is free precision.
Agree porosity acceptance. Especially on faces that will be machined — porosity moves the dimension after cutting and can ruin a sealing face.
CNC tolerances on a casting drawing. Every supplier quotes a machined part, and the price rises for no functional gain.
Precision on every dimension. In practice a DFM review usually shows that more than half of the precision callouts can be relaxed.
No draft angle. Discovering drag marks or sticking at trial means changing the tool, which is a five-figure decision.
No machining stock. A casting made to nominal leaves nothing to cut later.
No agreed measurement basis or temperature. The same part measured from a different datum, or at a different temperature, can move a large part of the tolerance band. Measuring at 20°C against an agreed datum is the standard approach.
Which standard do you accept against — NADCA, ISO 8062-3, or the customer drawing alone?
What can you hold as-cast, and what after machining? Can you show measured data from comparable parts?
Do you run flow simulation and DFM review, and is it done before the tool is cut?
What inspection capability is in house — CMM, CT scanning, X-ray, roughness, salt spray?
How is first-article approval and series process capability (Cpk) reported, and how long are traceability records kept?
A supplier who can answer these clearly can usually also explain the price: how much comes from tolerance and how much from secondary operations.
Tolerance is not "as tight as possible". It is tight where the function needs it and relaxed where it does not. Getting that balance right makes quotes more competitive and production more stable — usually worth more than another round of price negotiation.
EDT Diecasting Technology (Suzhou) produces custom aluminium and zinc die castings for automotive, industrial, electronics and appliance customers. DFM review and flow simulation are available before tooling, with CMM, CT and X-ray inspection in production. The plant is certified to ISO 9001, IATF 16949 and ISO 14001. Contact us to assess tolerance feasibility on a specific drawing.
Hotline
0512-67371602
E-mail：sales@edt-china.cn
Add：West Building, 66 Songshan Road, Suzhou New District, P.R. China
Hotline
