Guide
What flatness tolerance can you put on an aluminum die casting?
A flatness tolerance is a form control that limits how far every point of a single surface may depart from a perfect plane, without reference to any datum. On an aluminum die casting it answers one practical question: can this face be used as cast, or does it need a machining pass before it seals, mounts or locates anything?
By Saola Manufacturing engineering team · Published · Updated
This guide is for engineers and sourcing managers who put flatness callouts on die-cast housings, covers and heat sinks. It covers what the symbol means, why die castings move out of flat, where published as-cast values come from, a worked way to size the tolerance, and how to write it on the drawing so an overseas supplier measures the same thing you do.
The NADCA Product Specification Standards, ASME Y14.5 and the ISO geometric standards are paid documents. This page does not reproduce their tables. The one table shown below comes from a design guide its publisher makes freely available, and its source is named in the caption.
On this page
What does a flatness callout actually control?
It controls form only: the whole surface must lie between two parallel planes whose separation is the tolerance value, and those planes may float to any angle. Flatness says nothing about where the face sits, how it is tilted relative to other features, or how thick the wall behind it is.
A cover flange can be perfectly flat and still be tilted relative to the bore it closes; that is a parallelism or perpendicularity problem, which needs a datum reference. It can also be flat and in the wrong place, which is a location or profile problem. ASME Y14.5, the US standard for geometric dimensioning and tolerancing, defines flatness as a form tolerance with no datum (ASME Y14.5-2018); ISO 1101 does the same on ISO drawings.
Three details of the definition trip up casting drawings:
- Size limits may already control it. Under the Y14.5 envelope principle, a feature of size such as a plate thickness cannot exceed perfect form at its maximum material size, so a flatness callout on one side of that plate is only useful if it is tighter than the size tolerance.
- It can be applied per unit area. A callout can limit flatness over any small square of the surface as well as over the whole face, which suits large faces where local waviness matters more than overall bow.
- It says nothing about the measuring state. Unless the drawing says otherwise, a casting is checked in its free state, unclamped. A thin cover that pulls flat when bolted down may still fail a free-state check.
Why do aluminum die castings go out of flat?
Mostly because different parts of the casting cool and shrink at different rates, and the stresses that creates bend the part as soon as it leaves the die. Ejection, trimming and later machining add their own smaller distortions on top.
The International Zinc Association’s design rules put the mechanism plainly: castings with a low section modulus find it hard to stay flat as they cool, and castings with large differences in section distort because thin sections cool faster than thick ones (IZA, design rules). The same physics applies to aluminum, and NADCA’s advice to keep walls as consistent as possible, with gradual transitions where they must change (NADCA, uniform walls), is as much a flatness rule as a filling rule.
Other contributors to watch for on an aluminum part:
- Geometry. Large, thin, open faces such as covers and trays bow more than boxy parts. A flange that is thick on one edge and thin on the other tends to curl toward the thick side.
- The parting line. NADCA notes that flash at the parting line changes dimensions measured across it and recommends keeping critical dimensions in one die half (NADCA, parting line). A flat face that straddles the parting line inherits that mismatch.
- Ejection and trim. Uneven ejection or trimming while warm can leave a permanent set.
- Stress release during machining. Cutting away the skin on one side of a thin section removes stressed material and lets the part relax into a new shape. A face can measure flat on the machine and move after unclamping.
What flatness does published industry guidance allow as cast?
Published die-casting guidance ties the as-cast flatness tolerance to the size of the surface, usually its longest dimension or diagonal, and allows more on surfaces formed in opposite die halves. For aluminum, the reference North American die casters quote against is the flatness standard in the NADCA Product Specification Standards.
NADCA publishes standard and precision tolerance grades, with geometric dimensioning in its own section of the Product Specification Standards (NADCA, Product Specification Standards). The document is sold by NADCA and updated between editions, so the drawing should name the edition, the grade and the alloy family rather than copy a number from a secondary website. Foundry websites that publish their own flatness rules describe that foundry’s offer, not an industry standard.
The International Zinc Association publishes a free table for zinc die castings that shows how this kind of rule is built. It is reproduced below because it is openly available; it is zinc data, not aluminum data.
| Longest diagonal (mm) | Surfaces in the same die half (mm) | Surfaces in opposite die halves (mm) |
|---|---|---|
| up to 80 | 0.13 | 0.20 |
| 81 to 100 | 0.15 | 0.23 |
| 101 to 125 | 0.18 | 0.27 |
| 125 to 160 | 0.21 | 0.32 |
| 161 to 200 | 0.25 | 0.38 |
| 201 to 250 | 0.30 | 0.45 |
| 251 to 315 | 0.37 | 0.55 |
| 316 to 400 | 0.45 | 0.68 |
| 401 to 500 | 0.55 | 0.83 |
Two lessons carry over to aluminum. First, the opposite-die-half column is roughly half as large again as the same-half column in every row of the table, so where a flat face sits relative to the parting line matters as much as its size. Second, the allowance grows with size, so the same callout that is easy on a small boss can be unrealistic on a large cover.
Do not assume aluminum can match the zinc column. NADCA notes that magnesium, zinc and ZA alloys may reduce or eliminate finish machining when precision features are needed (NADCA, alloy selection), which is a polite way of saying aluminum often needs the machining pass. The ADC12 vs A380 guide covers how the common aluminum grades compare.
How do you work out a realistic flatness tolerance for one face?
Measure the size the rule is based on, read the published value for that size and die-half condition, and compare it with what the function actually needs. If the function needs less than the published as-cast value, the face needs machining or a design change, not a tighter number on the drawing.
A worked example using the open zinc table above: a Zamak cover with a flat sealing face measuring about 120 by 90 mm has a longest diagonal of about 150 mm, which falls in the 125 to 160 mm row of the IZA table, giving 0.21 mm if the face and the rest of its geometry are in one die half and 0.32 mm if it is formed across both (IZA, design rules).
For an aluminum part the steps are the same, with the numbers taken from the NADCA edition on your drawing:
- Find the governing size. Use the dimension the standard names, typically the longest dimension or diagonal of the flat surface, not of the whole part.
- Pick the grade. Start from the standard grade. Precision grades cost more process control and belong only on features that need them.
- Apply the size rule. NADCA-style rules are written as a base value for the first increment of size plus an added amount for each further increment, so the tolerance for a face is the base value plus the increment value multiplied by the number of increments beyond the first.
- Check the die-half condition. If the face crosses the parting line or is formed by a slide, expect the looser case and ask the die caster before you commit.
- Compare with the function. Take the flatness the gasket, O-ring, thermal pad or mating part actually tolerates, from its own maker’s data. If that is tighter than the result of step 3, the face should be machined.
When should a face be machined flat instead of left as cast?
Machine a face when its function needs less flatness error than the published as-cast value for its size, or when it is a datum that other machined features are located from. Leave it as cast when it only clears other parts or carries a compliant seal that tolerates the as-cast value.
Faces that usually end up machined on aluminum die castings:
- Sealing faces for thin or hard gaskets and for O-ring grooves, where a leak path opens wherever the gap exceeds what the seal can take up.
- Thermal contact faces on heat sinks and electronics housings, where an air gap under a component raises its temperature.
- Mounting and datum faces that set the position of bores, dowel holes or a mating assembly.
Machining is not free of flatness risk either. It removes the dense skin, which can open porosity on a sealing face, and it releases stress, so a thin part may move after unclamping. Good practice is to rough and finish in separate passes, clamp lightly on cast pads close to the cut, and keep the face and its locating surfaces in the same die half. Ask the supplier which faces will be finished on CNC milling equipment after die casting, and in what order.
Design changes can remove the machining pass altogether: split a large flat face into raised pads that are small enough to hold as cast, even out wall thickness behind the face, or add ribs in a balanced pattern to stiffen it. NADCA cautions that unnecessary ribs add complexity and cost (NADCA, ribs), so add them where stiffness is the goal, not by default.
How should flatness be called out on a die-casting drawing?
Put a flatness feature control frame only on the faces that need it, state whether the value applies as cast or after machining, and say how and in what state the part will be measured. A blanket flatness note across a whole casting drawing forces the supplier to quote the worst face everywhere.
A clear callout set for a cast-and-machined housing usually includes:
- Separate conditions. Mark machined faces with the surface texture symbol requiring material removal and tolerance them as machined; leave cast faces to the casting standard. The tolerance guide explains how NADCA and ISO general tolerances cover the faces you do not call out.
- The standard and edition. A general note such as “unless otherwise specified, as-cast tolerances per NADCA Product Specification Standards, [edition], standard grade” tells the die caster which table to quote against.
- Unit-area control where needed. On a large face, a per-unit-area flatness refinement limits local waviness under a seal without demanding the same value across the whole face.
- Measurement state. If the part is meant to be checked bolted down, state the restraint: which holes, which fasteners, what torque. Y14.5 recognizes a restrained condition when the drawing specifies it; otherwise inspection is in the free state.
- Inspection method. Agree whether flatness is measured on a coordinate measuring machine and with how many points, or on a surface plate. A casting that rocks on a plate is not being measured for flatness in the Y14.5 sense.
What should you agree with an overseas die caster before the die is built?
Agree which faces are machined, which die half each flat face sits in, and how first-article flatness will be reported, because the die fixes the as-cast flatness for its whole life. Changing a parting line or adding a pad later means changing die steel.
When castings come from Vietnam or anywhere else far from your plant, ask for three things in the first-article report: a flatness map of each critical face rather than one number, measurements from several shots and every cavity, and the same face measured after trimming, after machining and after any coating, so you can see where movement happens.
Saola Manufacturing sources die casting in ADC12 aluminum and Zamak 3 zinc and surface finishing from partner plants it manages and runs CNC milling and CNC turning at its lead CNC plant, so one party is responsible for collecting the cast, machined and coated measurements of a face for that kind of review; the quote names where each step is done. ISO 9001 certification is in progress, not yet held. The RFQ preparation guide lists what else to send, and you can send the drawing for a quote with the flat faces and their functions marked.
Frequently asked
Does flatness need a datum?
No. Flatness is a form tolerance and never references a datum. If the face must also be square or parallel to another feature, add a perpendicularity or parallelism callout with a datum.
Is flatness the same as parallelism?
No. Parallelism controls a surface relative to a datum and also limits its flatness. Flatness alone lets the face tilt freely.
Can I use the zinc table for an aluminum part?
Only as an illustration of how size and die half affect flatness. For aluminum, use the flatness standard in the NADCA edition named on your drawing, and confirm it with the die caster.
Will straightening fix a warped die casting?
Sometimes, on ductile parts and when the drawing allows it. It adds an operation and can crack less ductile high-silicon alloys, so ask whether it is planned before you rely on it.
Does anodizing or powder coating change flatness?
A coating follows the surface, so it rarely improves flatness, and heat in a cure oven can let a stressed thin part move. Measure critical faces after finishing as well as before.
Sources
- ASME Y14.5-2018 (reaffirmed 2024), Dimensioning and Tolerancing, ASME, accessed September 2026
- ASME Y14.8-2022, Castings, Forgings, and Molded Parts, ASME, accessed September 2026
- Zinc Die Casting design rules, section 5: alignment of plane surfaces, International Zinc Association, 2019
- Product Specifications Standards for Die Castings (table of contents), NADCA Design, North American Die Casting Association, accessed September 2026
- Parting Line, NADCA Design, accessed September 2026
- Uniform Walls, NADCA Design, accessed September 2026
- Ribs, NADCA Design, accessed September 2026
- Alloy Selection, NADCA Design, accessed September 2026