Which Tolerances to Put on a Casting Drawing
Most casting drawings are over-toleranced, and that is where the price comes from. Which dimensions to control, and how CT grades actually work.
10/18/20264 min read
A drawing arrived last week with ±0.05 mm on every dimension. Forty-one of them. The part was a pump housing, roughly 180 mm across, and the note at the bottom said "all dimensions critical".
Nobody's pump housing has 41 critical dimensions. What that drawing actually says is: we do not know which dimensions matter, so please hold all of them. The quote came back at two and a half times what the same part cost the previous year, and the buyer was surprised.
This is the most common commercial problem in casting, and it is not a foundry problem. It is a drawing problem.
What a casting can hold without trying
Investment casting is a precision process compared with sand casting, but it is still a process where molten metal shrinks about 2% while it solidifies. Tolerances come from a standard — ISO 8062-3, or GB/T 6414 in China — which sorts castings into grades.
CT4 to CT6 is the normal range for investment casting. In practice that means roughly ±0.10 mm on a 25 mm dimension and about ±0.25 mm at 150 mm. Below CT4 you are not casting any more, you are machining and then measuring what is left.
The number that matters is not the tolerance itself, it is the number of dimensions carrying one. An inspector has to touch every toleranced dimension on every part, or sample them in a way that has to be documented. Ten dimensions is a routine job. Forty-one dimensions is a full-time inspection station, and you are paying for it in the unit price.
Three ways drawings go wrong
Everything toleranced to the same value. This is the ±0.05 case. It signals that the design was not iterated against the process.
Tolerance applied across a parting line. Two mould halves do not align perfectly, and no amount of care changes that. A tight tolerance across a split is a gift to the reject pile.
No datum. If the drawing does not say what the part is measured from, the inspector picks something, and the customer's inspector picks something else. Both are right, and the parts do not fit.
What to do instead
Tolerate function, not geometry. Ask which dimensions actually affect assembly: a bore that takes a bearing, a face that seals, a hole pattern that bolts to something. Those get a real tolerance and a datum. Everything else gets the general tolerance in the title block.
Use one general note, then exceptions. "General tolerance ISO 8062 CT5, unless otherwise stated" plus five or six exceptions reads better to a foundry than forty individual callouts, and it prices lower because it tells us where to spend the effort.
Put the machining allowance on the drawing, not in an email. A face that will be machined needs 1.5–3 mm of stock, depending on size and how flat it has to end up. If it is not on the drawing, someone will quote the net shape and someone else will quote the cast shape, and the two prices will not be comparable.
Say what happens after casting. Stress relief, straightening, heat treatment, passivation — each one moves dimensions. A part that is straightened after casting cannot hold the same tolerance as one that is not.
A worked example
A 316 valve body, 90 mm, with a 32 mm bore and a flange face.
Overall length — What the drawing said: ±0.05 mm; What we would put: CT5 general
Bore — What the drawing said: ±0.05 mm; What we would put: Cast to +1.5 mm stock, machine to H8
Flange face — What the drawing said: flatness 0.05; What we would put: Cast with 2 mm stock, machine flat
Bolt holes — What the drawing said: ±0.1 mm position; What we would put: Drill after casting, jig located
Wall — What the drawing said: 4 mm ±0.3; What we would put: CT5, no callout needed
Outside profile — What the drawing said: ±0.05; What we would put: CT6 general
Same part. The first column costs about 40% more than the second, and the second one will have a lower reject rate, because the tight features are being made by a machine tool instead of by a shrink rate.
The conversation worth having
If a dimension is tight because a catalogue bearing has to fit, tell us the bearing. We will cast stock and bore it, and the tolerance problem disappears.
If a dimension is tight because it was tight on the previous supplier's drawing, question it. Drawings accumulate tolerances the way houses accumulate coats of paint.
And if you genuinely need CT4 across the whole part, that is a legitimate request — it just gets quoted as a different process route, usually with 100% inspection and a straightening step. We would rather quote it honestly than win the order and lose it at the first inspection report.
Tolerances we work to
The standard grades, minimum wall thickness, surface roughness and weight range are all on the investment casting data sheet. If your part has a thin wall next to a tight tolerance, read how thin a wall can be first — the two limits interact, and the thinner the wall, the more the part moves after casting.
Send the drawing with the critical dimensions marked, even roughly. Marking five dimensions as "these matter" changes the quote more than any negotiation will.
Questions we get on this
Can you hold ±0.05 mm on a casting? Not as cast. With machining on the critical features, yes, and that is how it should be specified. As-cast ±0.05 mm on a 100 mm part is outside what any investment foundry can do repeatably.
Does adding a general tolerance note reduce the price? Usually, yes — not because the tolerance is looser, but because it tells the foundry and the inspector where to concentrate. Fewer measured dimensions means less inspection time in the unit price.Related reading
Quality
Precision manufacturing for diverse industrial applications.
Services
Products
+8615912702921