Two numbers on a casting drawing decide whether your parts assemble smoothly or generate a year of concession requests: the casting tolerance and the machining allowance. They are related but they are not the same thing, and buyers routinely conflate them. A tolerance tells the foundry how much variation is acceptable on a dimension it will not machine. An allowance tells the foundry how much extra metal to leave on a surface that will be machined later. Get either wrong and the cost shows up three months later - as scrap, as rework, or as a machining line that cannot hold cycle time.
This guide explains how tolerance grades work under ISO 8062, what tolerance ranges are realistic for each casting process, how much machining allowance to specify, and which points on your drawing package should be checked before you release a purchase order.
Why Casting Tolerance and Machining Allowance Are Different Decisions
A casting tolerance is a permission: it defines the window of variation the foundry is allowed on as-cast geometry. A machining allowance is a budget: extra material reserved so that the subsequent CNC operation can produce a clean, fully machined surface within the final print tolerance.
The two interact directly. If your allowance is smaller than the sum of the casting tolerance plus expected distortion, the cutter will not clean up the whole face on every part - some pieces will come out with a black patch of as-cast skin on a sealing surface. That is not a machining defect; it is a drawing defect. The rule of thumb is simple: allowance must be greater than casting tolerance plus distortion, with margin for pattern wear and heat-treat movement.
How Casting Tolerance Grades Work (ISO 8062)
ISO 8062-3 defines Dimensional Casting Tolerance Grades (DCTG 1-16) and Geometric Casting Tolerance Grades (GCTG 1-8). A smaller grade number means a tighter tolerance. The grade you specify should reflect the process, the size of the part, and how much machining follows - not an aspiration.
For a 100 mm dimension, typical as-cast linear tolerances look like this:
- Hand/green sand casting: roughly ±0.8 to ±1.8 mm (DCTG 10-13)
- Resin-bonded sand and shell molding: roughly ±0.5 to ±1.0 mm (DCTG 8-10)
- Investment (lost wax) casting: roughly ±0.10 to ±0.30 mm (DCTG 4-6), often quoted as ±0.25% of dimension with a 0.13 mm floor
- Aluminium die casting: roughly ±0.10 to ±0.25 mm, plus additional tolerance for moving dies
Two practical warnings. First, tolerance scales with part size: a 500 mm dimension cannot be held to the same grade as a 50 mm dimension, and any foundry that quotes otherwise is not being straight with you. Second, thin walls, long unsupported sections and asymmetric shapes distort independently of the dimensional grade, so specify flatness and straightness (GCTG) explicitly for those features rather than hoping the linear tolerance covers them.
Typical Machining Allowance by Process
Allowance is normally given per machined surface, not as a global value. The figures below are industry-standard starting points for carbon steel, stainless steel and iron castings; add margin for large parts, heat treatment, and any stress-relief cycle.
| Process | Typical casting tolerance (100 mm) | Machining allowance per surface | Notes for buyers |
|---|---|---|---|
| Green / resin sand casting | ±0.8 to ±1.8 mm | 3 mm small, 5 mm medium, 6-10 mm large | Allowance must exceed distortion on long, flat faces; add 1-2 mm if stress relief follows |
| Shell molding | ±0.5 to ±1.0 mm | 2.5-4 mm | Better surface finish, so smaller allowance is safe on sealing faces |
| Investment casting | ±0.10 to ±0.30 mm | 0.5-1.5 mm | Often 0.5-0.8 mm is enough; too much allowance wastes wax pattern cost and cycle time |
| Die casting (aluminium / zinc) | ±0.10 to ±0.25 mm | 0.3-1.0 mm | Keep allowance minimal; cast-in features should be designed near-net where possible |
| Closed die forging | ±0.3 to ±1.0 mm | 2-4 mm | Add for decarburised skin and die wear over the tool life |
Note the direction of the trade-off. Too little allowance causes incomplete cleanup and scrap. Too much allowance costs you twice: the casting is heavier (more melt, more freight), and every extra millimetre of stock means additional roughing passes on every part for the life of the program. On a 200,000-piece annual volume, 1 mm of unnecessary stock on a 120 mm bore is measurable money in both casting yield and machining hours.
Where Tolerances Usually Go Wrong on Real Drawings
1. Blanket tolerance notes
"General tolerance ±0.5 mm" on a sand casting drawing is a promise the process cannot keep on every feature. Split the drawing: define functional dimensions individually, and state a realistic general grade for the rest.
2. Hole patterns specified as cast features
Centre distance on as-cast holes is one of the least stable dimensions in any casting, because it combines pattern shrinkage, core shift and mould closure error. If two holes must align with a mating part, cast them with stock and drill them in the same CNC setup as the datum face.
3. Datum schemes that do not match the machining setup
If the drawing datums are functional surfaces but the machine shop clamps on a different face, every tolerance is being measured from somewhere the process never controlled. Send the machining datum intent with the RFQ - a short note beats a round of first-article arguments. Our precision casting and sand casting teams work from the same datum scheme the CNC department uses, which is why we ask for the machining sketch rather than only the finished print.
4. No allowance on heat-treated parts
Quenching and tempering move thin sections. If a part is heat treated between casting and machining, add 0.5-1.5 mm beyond the normal allowance, or specify stress relief before finish machining.
Drawing Package Checklist Before You Release the PO
- Tolerance grade stated by standard - e.g. "ISO 8062-3 DCTG 9, GCTG 5", not "commercial tolerance".
- Machined surfaces marked with the machining symbol and a per-surface allowance value.
- As-cast surfaces marked so the foundry does not add stock where none is needed.
- Critical dimensions flagged with the inspection method expected (CMM, gauge, functional check).
- Datum scheme consistent with the CNC fixturing plan.
- Wall thickness minimum stated, with any thin-section exceptions called out.
- Flatness / coaxiality / position specified for sealing faces, bores and bolt patterns.
- First article requirement - full layout inspection report with actual values, not pass/fail.
- Sampling and inspection level agreed (AQL, or 100% for safety-critical features).
- Surface finish and coating defined, including which surfaces are masked during coating.
What to Expect from a Reliable Supplier
A supplier who understands tolerance economics will push back on your drawing before quoting - not after the first article fails. Expect questions on which dimensions are functional, whether a feature can be cast or must be machined, and whether a tolerance can be relaxed to reduce scrap. That conversation usually saves more money than any price negotiation.
We produce sand castings, investment castings and die castings with in-house CNC machining to the tolerances above, and we quote against your finished drawing plus machining intent rather than a generic catalogue tolerance. If you are unsure which grade and allowance combination is realistic for your part, send the drawing with material, annual volume and the dimensions that actually matter functionally.
Email your 2D drawing (PDF with tolerances) or 3D model (STEP/IGES) to sales01@ythongshengindustry.com. Our engineering team will return a tolerance review, a proposed allowance per surface, and a quotation within 2-3 working days.