The most common reason a MIM quotation comes back higher than expected is not tooling or material — it is tolerance. A drawing that applies a tight tolerance across every dimension pushes the part into a machining-dominated process chain, and the economics that made MIM attractive disappear before the quote is issued.
This guide covers what MIM holds as-sintered, where the practical limits sit for walls, holes and threads, and how to structure a drawing so the tight tolerances land only where they are needed.
Why MIM tolerances differ from CNC tolerances
A CNC machine positions a tool against a workpiece and holds the result to the machine's accuracy. Material is removed after the shape is fixed, so tolerance is a machine property.
MIM is the reverse. The shape is set in the mould, then the part shrinks by 15–20% during sintering. Tolerance is therefore the sum of mould accuracy, feedstock consistency, injection repeatability, shrinkage behaviour and furnace variation. Because shrinkage is proportional, the resulting tolerance is proportional too — which is why MIM tolerance is expressed as a percentage of the dimension rather than as a fixed band.
Once that is understood, the rest of MIM design guidance follows logically. Errors scale with size. Thin and thick sections behave differently. Features formed by thin core pins are as fragile as the pins. And anything requiring absolute accuracy rather than relative accuracy has to be machined after sintering.
The percentage rule, in numbers
Percentage-based tolerances are sometimes used for early comparisons. The table below shows the arithmetic at ±0.3% and ±0.5%; it does not establish an achievable tolerance. Review feature size, geometry, alloy, datums and any minimum absolute tolerance with the manufacturer.
| Dimension | At ±0.3% | At ±0.5% | Practical reading |
|---|---|---|---|
| 5 mm | ±0.015 mm | ±0.025 mm | Arithmetic only; minimum practical tolerance must be reviewed |
| 10 mm | ±0.030 mm | ±0.050 mm | Arithmetic only; confirm with the supplier |
| 20 mm | ±0.060 mm | ±0.100 mm | Illustrative calculation; verify process capability |
| 40 mm | ±0.120 mm | ±0.200 mm | Illustrative calculation; verify process capability |
| 60 mm | ±0.180 mm | ±0.300 mm | Illustrative calculation; verify process capability |
a tight tolerance on a small feature needs a specific capability review and an agreed control route; it may require secondary finishing
Wall thickness
Wall thickness is reviewed with material, flow length, local mass, debinding and distortion risk. Avoid abrupt transitions and unsupported features where practical; do not use one wall-thickness band as a universal tooling rule.
The more important rule concerns variation rather than absolute thickness. Where a thick boss or hub meets a thin wall, the two regions densify at different rates. Keeping the ratio between the thickest and thinnest section below roughly 3:1 avoids most defects; cores and lightening features are the standard way to bring a heavy section closer to the surrounding wall.
Design the section, not just the shape. A part with 2 mm walls and one 8 mm hub will sinter unevenly no matter how good the furnace is. Coring the hub, or accepting that it will need machining, is a design decision that belongs in the first drawing rather than the third sample.
Holes and bores
Hole feasibility depends on diameter, depth, core-pin support, orientation and material. Compare molded holes with drilling or other finishing where tooling becomes fragile or the required fit is critical.
Holes that run parallel to the mould opening direction are straightforward. Cross-holes are also possible in MIM — this is one of its advantages over press-and-sinter PM — but they require side-action tooling or additional mould complexity, which affects tooling cost. Where a cross-hole exists only to pass a pin or a wire and the tolerance is loose, forming it in the mould is usually cheaper than drilling later.
Threads
Small internal threads can be moulded using unscrewing cores, but the tooling is more complex and the thread form must tolerate the shrinkage. External threads can be formed when they are coarse enough to survive sintering without distortion.
For most industrial parts, threads tighter than about M3 or requiring a specific class of fit are cut or rolled after sintering. The general approach: state the thread on the drawing, expect the supplier to propose whether it is moulded or machined, and confirm which one appears in the quotation.
Undercuts, draft and radii
Undercuts and side features are formable in MIM using split tooling or side actions, unlike press-and-sinter PM where they generally are not. The cost is tooling complexity, so the design question is whether the feature can be moved to a direction that avoids a side action — often it can, with a small change to the surrounding geometry.
Draft angles let the part release from the mould cleanly. MIM generally requires less draft than die casting or forging, but surfaces parallel to the mould opening direction still benefit from a small amount — commonly about 0.5° to 1° on walls, more on textured surfaces. Where the drawing shows a zero-draft wall, expect the supplier to raise it.
Radii serve the same purpose at internal corners, where a sharp corner concentrates stress during cooling and can cause cracking. A practical minimum inside radius is around 0.2–0.5 mm, and it is usually cheaper to add one than to argue about it.
How material affects tolerance
Shrinkage varies by alloy and by powder specification, so tolerance capability varies with the material. Austenitic 316L is well characterised and behaves predictably. Martensitic grades such as 420 and 440C are more sensitive to carbon content and atmosphere, and their sintering window is narrower. Magnetic grades require tighter control of carbon and oxygen, which can affect dimensional consistency as well.
The practical takeaway: the tolerance figures quoted above are a working baseline for well-characterised stainless grades. For less common alloys, the supplier should be asked what capability has actually been demonstrated, rather than what is theoretically possible.
Specifying tolerances in an RFQ
A drawing that produces a competitive MIM quotation usually has three tiers of tolerance.
- Critical features — fits, bores, sealing surfaces, bearing journals. Mark these explicitly, and expect them to be machined after sintering.
- Functionally significant dimensions — assembly clearances and general fits. Typically ±0.1 mm to ±0.3 mm, which is achievable as-sintered on most part sizes.
- General dimensions — leave these at a general tolerance note rather than dimensioning every one. This is where a drawing either keeps MIM economical or makes it expensive.
Also state the datum structure. MIM parts are measured against datums established after sintering, and a well-defined datum scheme makes first-article inspection straightforward rather than a debate.
Design mistakes that cost money
- Applying ±0.05 mm generally. It converts an economical forming part into an expensive machining part.
- Heavy sections without coring. Thick hubs and bosses next to thin walls sinter unevenly and generate sink or porosity.
- Very small or very deep holes. Thin core pins deflect and break, which shows up as tooling cost and downtime.
- Sharp internal corners. They concentrate stress during cooling and cause cracking in the green or brown part.
- Zero draft on tall walls. Ejection becomes difficult and surface finish suffers.
- Tolerancing a feature that is not measured. Adding a tight tolerance to a cosmetic dimension buys inspection cost with no functional benefit.
Material standards and dimensional capability are different references. MPIF Standard 35-MIM and ASTM B883 address MIM materials; they do not establish one tolerance for every feature. The percentages in this guide are illustrative arithmetic, not a SINTS capability guarantee. Agree feature tolerances, datums and inspection methods from the actual drawing.
Conclusion
MIM tolerance is proportional, and that single property explains most of the design guidance: small dimensions are relatively accurate, large ones are not; section variation causes distortion; thin core pins set the hole limits; and only a handful of features should carry machining tolerances.
A well-structured MIM drawing concentrates precision where it functions, leaves general dimensions general, and states density, material and datums explicitly. That drawing is cheaper to make, cheaper to inspect and far less likely to require a tooling change after the first samples.
Related component families
These pages apply the tolerance framework to specific component types.
Precision Small Components
Where small feature sizes work in favour of as-sintered accuracy.
Component guide →Component Design Notes
DFM notes by feature type, from wall sections to threads and radii.
Component guide →Shafts, Pins and Plungers
Where bearing journals typically need a machining pass after sintering.
Component guide →Mechanism Components
Feature-rich parts where tolerance allocation decides the process chain.
Component guide →Have a drawing to discuss?
Send it to our engineering team. We review process fit and identify the information needed for a quotation.
Send Drawing for Review