Guide
How do you set datums on castings for machining?
Datums on castings are the reference features, usually datum targets on raw cast surfaces, that fix a casting in space before any metal is cut, so that the first machining operation can locate the part the same way every time and produce the machined surfaces that later become the finished part’s own datums.
By Saola Manufacturing engineering team · Published · Updated
Most writing on this topic stops at geometric dimensioning and tolerancing theory. This guide follows the part instead: from datum targets on the raw casting, to the fixture of the first machining operation, to the machined datum reference frame that the finished drawing is inspected against, and finally to what a first article report should show at each stage. It is written for mechanical engineers and sourcing managers who send die-cast or other cast parts to a supplier for casting and machining, often in another country. The datum rules described here come from ASME Y14.5 and ASME Y14.8; the tolerance values in the table come from published die casting industry guidance and describe the process in general, not any one shop.
On this page
What is a datum target, and why do castings need one?
A datum target is a designated point, line or small area on a part that contacts the inspection or machining fixture, and together the targets establish a datum when a whole surface is too rough, drafted or uneven to serve as one. Raw castings are the classic case, because their surfaces carry draft, parting-line flash, gate remnants and local sink that make full-surface contact unrepeatable.
Datum targets are defined in ASME Y14.5-2018, the US standard for dimensioning and tolerancing, whose revision put more emphasis on datum references and the degrees of freedom each datum constrains. On a drawing, each target is identified by a divided circle: the lower half carries the datum letter and target number (A1, A2, A3), and the upper half carries the size of the contact area when the target is an area rather than a point.
The logic is simple. A primary datum plane on a casting is typically set by three point or small area targets, which settle the part against three locators. A secondary datum is typically set by two targets and a tertiary by one. That familiar three-two-one scheme removes all six degrees of freedom with the fewest possible contacts, which is exactly what you want on a surface that is not flat enough to sit on as a whole.
ASME Y14.8-2022 is the companion standard for castings, forgings and molded parts. It builds on Y14.5 for the drawing conventions those parts need, such as parting lines, draft and machining allowance. If your drawing is to ISO rather than ASME, the equivalent datum rules live in ISO 5459, and the concepts carry over even though the symbols differ in detail.
Which cast features make good datum targets?
Good cast datum targets sit on stable, well-supported surfaces formed by one die half, away from the parting line, gates, overflows, ejector pin marks and any face that will later be machined away. They should also be spread as far apart as the part allows, because widely spaced targets resist rocking and reduce the angular error that a small surface bump can cause.
- Stay inside one die half. NADCA notes that flash increases thickness at the parting line and alters dimensions measured across it, and advises keeping critical dimensions within one die half (NADCA, parting line). Put the primary targets on the same side as the features they control.
- Mind the draft. Walls parallel to the die opening direction carry draft (NADCA, draft), so a target on a drafted side wall locates at a different height depending on where the locator touches. Put secondary and tertiary targets at a stated height, or on small pads cast square to the parting plane.
- Avoid trim and ejector witness marks. Gate stubs, trimmed flash and ejector pin marks are the least repeatable spots on a die casting. Ask the die caster where they will fall before fixing target locations.
- Avoid faces that will be machined. A target on a surface that the first operation cuts away is fine for that operation, but the second operation can no longer find it. Keep at least one as-cast reference that survives machining, or plan the handoff described below.
- Use cast pads or bosses when the part has no flat. A part with few flat surfaces is the usual trouble case. Small raised locating pads, added to the casting for no other reason, give the fixture a defined contact and cost little in the die.
How do you hand off from cast datums to a machined datum reference frame?
Locate the raw casting on its datum targets for the first operation, machine the surfaces and holes that will become the functional datums, and then locate every later operation, and the final inspection, on those machined features. The drawing should show both frames and the tolerances that link them, so nobody has to guess which one governs a given feature.
A workable sequence for a die-cast housing:
- Operation 10, cast datums. The casting sits on targets A1 to A3, pushes against B1 and B2, and stops against C1. The first operation mills the mounting face and bores the main locating hole and a second hole or slot.
- Operation 20, machined datums. The part now locates on the milled face, the bored hole and the slot. Every remaining feature, including the far-side faces, threads and sealing grooves, is cut from this frame.
- Inspection. Machined features are measured to the machined frame. The relationship between the machined frame and the as-cast surfaces that remain, such as wall thickness to an internal core or clearance to an as-cast outline, is checked back to the cast datums.
The failure to avoid is a drawing where the machined features reference datum letters that only exist on the raw casting. Once the part has been machined, those targets may be gone or disturbed, and every position tolerance becomes unmeasurable. The opposite failure is a drawing that defines only the machined frame, which leaves the first operation free to locate the casting however the shop chooses, so the machining stock can end up uneven or missing on one side.
Machining stock is part of the handoff. As a basis for planning, the International Zinc Association suggests an allowance of 0.25 mm on zinc die-cast surfaces that must be machined, and warns that removing too much material tends to expose porosity (IZA, design rules). Heavier stock on aluminum castings raises the same porosity concern, which is one more reason to locate the first cut from the casting’s own datums rather than from an arbitrary face.
How much does the die layout add to datum-related tolerances?
It adds a measurable amount: published die casting guidance gives a wider alignment tolerance when a surface is formed in the opposite die half from its datum, and wider still when it is formed by a moving die element such as a slide. The table shows those published values for zinc die castings.
| Longest diagonal of surface (mm) | Same die half as datum | Opposite die half, or moving die member in datum half | Moving die element in opposite half |
|---|---|---|---|
| 0 to 80 | 0.13 | 0.20 | 0.28 |
| 101 to 125 | 0.18 | 0.27 | 0.40 |
| 161 to 200 | 0.25 | 0.38 | 0.64 |
| 251 to 315 | 0.37 | 0.55 | 0.97 |
| 401 to 500 | 0.55 | 0.83 | 1.54 |
Read across a row and the pattern is the point: the same surface costs more tolerance the further it is, in die terms, from its datum. The same source applies the same logic to cored holes, giving a larger allowance for a hole whose datum is in the opposite die half (IZA, design rules). Aluminum die castings follow the same physics, and the NADCA Product Specification Standards publish their own parting-line and moving-die-component allowances for each alloy family.
For datum planning, the practical takeaway is to put the datum targets in the die half that forms the features they control. If a critical as-cast feature has to come from a slide, either accept the larger band or plan to machine it from the machined frame.
What does the machining fixture need to match the datum targets?
The first-operation fixture should put its locators exactly where the drawing puts the datum targets, with the same contact type and size, and apply clamping force directly over those locators. A fixture that locates somewhere else is quietly defining a different datum system from the one on the drawing.
- Match contact type. A point target means a spherical or crowned locator, a line target a knife-edge or narrow rest, an area target a flat pad of the stated size.
- Clamp over the locators. Clamping between supports bends a thin-wall casting, the part springs back when released, and the machined face is no longer flat to the cast datums.
- Seat in datum order. Load the primary targets first, then push against the secondary, then the tertiary. The order of contact is part of the datum definition.
- Share the scheme with inspection. The checking fixture or the coordinate measuring machine program for the raw casting should use the same targets, so the die caster’s report and the machinist’s setup describe the same part.
The International Zinc Association points out that die castings can be given accurate datum surfaces for clamping, which makes accurate machining easier than on parts formed by less precise processes (IZA, machining economics). That advantage only appears when the targets are designed in.
What should first article inspection check on a cast-then-machined part?
A first article report for a cast-then-machined part should cover two states: the raw casting measured from its datum targets, and the finished part measured from its machined datum reference frame. It should also show that machining stock cleaned up on every machined face.
- Raw casting. Target locations, the as-cast dimensions that feed machining stock, and the dimensions that stay as cast.
- Handoff. Evidence that each machined face cleaned up fully, with no as-cast skin left, and that remaining wall thickness is within limits where machining approaches a cored feature.
- Finished part. Every characteristic on the machined drawing, measured to the machined frame, with the datum letters in the report matching the drawing.
- Porosity at machined faces. Any agreed porosity limits on sealing or cosmetic machined surfaces, since machining opens up subsurface voids.
The quality requirements guidance from the International Zinc Association makes the underlying point well: most supply disputes come from different understandings of what was required, so critical dimensions should be specified in measurable terms and agreed with the die caster (IZA, specifying quality requirements). A datum scheme that both the caster and the machinist sign off on is the most concrete version of that agreement.
How should the drawing show datums when casting and machining are sourced overseas?
Send one drawing package that defines the casting datum targets, the machined datum frame and the link between them, and ask the supplier to confirm the first-operation fixture against the targets before tooling is finished. That applies whether the die casting and the machining happen at one supplier in Vietnam or at two different companies.
Splitting casting and machining between suppliers is where datum problems usually surface, because each party is inspecting to a different state of the part. If the die caster measures to one set of points and the machinist fixtures on another, both can report conforming parts while the finished part fails. A single casting drawing with datum targets, referenced by the machining drawing, removes that gap.
Saola sources die castings from partner foundries it manages and machines them on the CNC milling centers at its lead CNC plant, and plans the casting datums and the first-operation fixture together on one drawing set. The same drawing discipline still applies: the targets should be on the drawing, not only in the supplier’s process notes, so that any future source can reproduce them. The RFQ package guide covers the rest of what to send, and when the drawing is ready you can send it for a quote, with datum questions answered feature by feature in the reply.
Frequently asked
Can a raw cast surface be a datum without datum targets?
It can, but the result depends on which high spots touch the fixture, so it varies from part to part and from fixture to fixture. Datum targets remove that ambiguity by naming the contacts.
Should the finished part drawing still show the cast datum targets?
Show them on the casting drawing or on the as-cast view, and reference that drawing from the machined one. The finished-part characteristics should be toleranced to the machined frame, with only the as-cast features tied back to the targets.
Where do ejector pin marks go relative to datum targets?
Away from them. Ejector pin marks can stand slightly proud or below the surface and may carry flash, so ask the die caster for the ejector layout and keep targets clear of it.
Do the same rules apply to sand castings and investment castings?
Yes. The datum target method in ASME Y14.5 and the casting conventions in ASME Y14.8 are process-neutral. Rougher processes simply make targets more important, because full surfaces are even less repeatable.
Who should design the first-operation fixture?
The machining supplier builds it, but the design engineer should approve that its locators match the drawing’s datum targets before production parts are cut.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ASME Y14.8-2022, Castings, Forgings, and Molded Parts, ASME, 2022
- Parting line design guidance, NADCA, accessed September 2026
- Draft design guidance, NADCA, accessed September 2026
- Product Specification Standards for Die Castings, NADCA, accessed September 2026
- Zinc die casting design rules, International Zinc Association, 2019 web edition
- Machining economics of zinc die castings, International Zinc Association, 2019 web edition
- Specifying quality requirements, International Zinc Association, 2019 web edition