MIM Shrinkage and Tolerances: How to Specify Dimensions That Work
Updated 3 November 2026 · CSMFG technical guides
Metal injection molded parts shrink as they are sintered, so the mold cavity is designed for a larger green part. The exact change depends on feedstock, geometry and processing. A practical tolerance plan identifies the features that control assembly and validates them on production-representative parts.
One published MIM design reference describes additional sintering shrinkage in the approximate range of 15–25% for its discussion of common processes. That is an example, not a specification for a particular material or direction; the supplier must establish actual shrinkage and capability for the selected feedstock and part. See the MIM design discussion.
Watch: MIM Shrinkage and Tolerances
How is mold size estimated from shrinkage?

For a simplified one-dimensional example, suppose a finished length must be 20 mm and a trial process shows 20% linear shrinkage from the measured green length. The estimated green length is 20 ÷ (1 − 0.20) = 25 mm. Subtracting 20% from a 24 mm green dimension would give only 19.2 mm, not 20 mm.
This is a planning calculation, not a tool design rule. Actual shrinkage may differ by direction, feature, lot, furnace support and tooling. Mold shrinkage, tool construction and process variation also need to be considered separately. Tool correction and capability must be based on measured trials.
Does a single percentage tolerance apply to every dimension?
A single percentage tolerance is not a complete MIM tolerance plan. A bore diameter, a distance between features on separate mold inserts and a flatness requirement have different sources of variation. Sintering support, ejection, gate removal and later machining can change the final relationship between surfaces.
For example, the position of a pivot bore relative to an assembly contact face can matter more than the outside contour. Define functional datums and the inspection condition, then request a feature-specific capability assessment using representative cavities and furnace loads. Tighten noncritical dimensions only when the assembly requires it.
On a pivoting latch, the bore diameter and its position relative to the contact face may control assembly; the outside contour may only need clearance. Tolerancing those functions selectively can reduce needless machining while still protecting the mechanism.

What affects MIM dimensional consistency?
Dimensional consistency is the combined result of feedstock uniformity, mold condition, geometry, thermal processing and measurement. A fixed tool offset and broad part-to-part variation are different problems. The first may call for a tool correction; the second requires examination of the process and gauge system before dimensions are changed.
For example, the CSMFG Cam Lever detail specifies a 2.30 ±0.03 drilled diameter, giving limits of 2.27–2.33 in drawing units. The requirement belongs to that final feature, rather than every molded contour. First record the actual datum, fixture and measurement stage. Then compare results by cavity, feedstock lot and furnace position. According to CSMFG's special-process document, mixture consistency and sintering support affect shrinkage and distortion; the November 2026 part information supplies the specific lever context. Include later drilling, heat treatment and finishing in the final inspection plan. The design guide shows why a long arm, pivot boss and contact face need different dimensional questions.
What should an RFQ include?
A MIM tolerance RFQ should include the 3D model, dimensioned drawing, assembly datums, material condition, expected volume and inspection method. Identify the few dimensions that control the mechanism and state whether each limit applies before or after finishing. For example, a coated bore needs an agreed final size, masking plan and measurement condition; a noncritical outside contour may only require clearance.
Request sample measurements across cavities and representative furnace positions. A successful first article is useful, but a single measurement does not establish production capability or directional shrinkage behavior.

How should a tolerance stack be checked?
Consider a latch with two mounting holes and a cam face. Hole diameter, center distance and cam position may all affect assembly. If each is measured from a different arbitrary edge, the inspection report may pass individual dimensions while the assembly binds. Use datums that match how the part is located in the product, then evaluate the combined positional relationship.
Ask the supplier to identify potential mold insert offsets, setter contact and any post-sinter machining. A tolerance stack should include these manufacturing stages and the mating components. If the geometry cannot meet the required fit economically, change the datum strategy, machine a selected feature or adjust the assembly rather than tightening every dimension.
What is the difference between accuracy and repeatability?
A consistent dimensional offset may be corrected during tool development, but large part-to-part spread requires investigation of the process and measurement system. Sample across cavities, batches and production conditions. Agreement on how many parts to measure and how to evaluate the results is more useful than treating one successful first article as evidence of capability.
How should the Cam Lever bore tolerance be interpreted?
The CSMFG Cam Lever detail specifies a drilled diameter of 2.30 ±0.03, which gives drawing limits of 2.27 to 2.33 in the drawing's units. The same detail marks a diameter 2.80 × 90° countersink. These are feature requirements from the supplied drawing; they are not measured process-capability results or proof of an as-sintered MIM bore tolerance. Confirm units and general notes on the complete released drawing.
First establish the final datum scheme and whether the hole is accepted after drilling, heat treatment and any finish. Second, identify a fixture and gauge method appropriate to the lever profile and pivot function. The component's specified 17-4PH H900 condition must remain associated with the dimensional requirement. According to CSMFG's November 2026 part information, the same lever has a reference piece price above 2,000 pieces. The illustrated case links geometry, condition and commercial scope without treating a drawing tolerance as measured repeatability.

What do the original shrinkage and roughness references support?
CSMFG's special-process document describes 13–25% linear sintering shrinkage as a broad MIM reference and identifies feedstock uniformity as important to dimensional control. The embedded workbook in the material presentation separately lists Ra 0.8–1.5 µm as a surface-roughness reference. Neither figure is tied to a particular Cam Lever batch, cavity, gauge method or inspection sample.
Use these references to understand why the green part is oversize and why finishing allowances belong in the drawing review. Do not apply one shrinkage percentage to every axis or interpret a roughness range as a tolerance on a pivot hole. For example, a long lever arm can require different support considerations from a short cylindrical boss. The factory controls must connect mixing, molding, debinding, furnace loading and any secondary machining. See the MIM process controls and surface-treatment guide for the stages that can alter the final condition.
Shrinkage and tolerance questions
How do you calculate an estimated green dimension?
Divide the desired finished dimension by one minus the assumed linear shrinkage expressed as a decimal. For example, 20 mm divided by 0.80 gives 25 mm at an illustrative 20% shrinkage. Production tooling must use measured process-specific behavior and account for variation.
Is shrinkage identical in every direction?
MIM shrinkage is not guaranteed to be identical in every direction or at every feature. Feedstock uniformity, geometry, support contact and furnace loading can produce different dimensional responses. For example, a long arm resting on a setter may behave differently from a short unsupported wall on the same component.
Use representative trials to measure critical dimensions by cavity and furnace position, then decide whether tooling correction, support changes or selective machining are needed. The illustrative green-size formula in this article assumes a single linear shrinkage value; it is not a production tooling specification.
Related reading: See MIM design guidelines, MIM defects and causes, and MIM production costs.
Review a drawing with CSMFG’s powder metallurgy and MIM team.
For a coated feature, also account for the dimensional example in surface-treatment planning.