Ask a supplier what tolerance they can hold, and you will almost always get a range. Push further and ask what that range looks like in practice — on your material, your geometry, your production volume — and the conversation gets more interesting. Tolerance charts by process exist precisely to anchor that conversation with real numbers before a single tool path is written or a mold is cut.

Specifying tolerances that are too tight adds cost, extends lead times, and sometimes pushes a part beyond what the chosen process can physically deliver. Specifying them too loosely creates assembly failures, functional problems, and expensive rework downstream. The goal is not maximum precision — it is appropriate precision, matched to what each manufacturing method can consistently and economically achieve.

This guide covers the most widely used manufacturing processes — CNC machining, 3D printing, plastic injection molding, pressure die casting, vacuum casting, sheet metal fabrication, and compression and silicone molding — with realistic, production-grounded tolerance numbers for each. Whether you are selecting a process for a new product, reviewing a drawing before RFQ, or transitioning from prototyping to volume production, the numbers in this article give you a practical starting reference.

Why Tolerance Numbers Actually Matter

A tolerance is the total permissible variation around a nominal dimension — the band within which a finished part is still considered acceptable. It is not an aspirational target; it is a contract between the designer and the manufacturing process. Every dimension on a drawing that carries a tolerance is a purchase order for a specific level of precision, with real consequences for cost, lead time, and scrap rate if that specification does not match what the process can actually deliver.

The relationship between tighter tolerances and manufacturing cost is not linear — it is exponential. The relationship between engineering tolerance and manufacturing cost is exponential rather than linear. A dimension that is routine at ±0.25 mm can require specialized fixturing, additional inspection passes, and climate-controlled environments once it tightens to ±0.025 mm. Tighter-than-standard tolerances require specialized manufacturing approaches, with additional machining passes, enhanced measurement systems, and increased inspection frequency all contributing to higher costs. Secondary operations often become necessary when standard processes cannot achieve required tolerances.

The practical implication for engineers is straightforward: apply tight tolerances only to the features where function genuinely requires them, and let non-critical dimensions rest at the natural capability of the process. For critical dimensions, the drawing should clearly identify the functional features that truly need tight control. This allows the machining process and inspection plan to focus on the right areas. With that principle in place, the following process-by-process reference gives you the numbers to work with.

CNC Machining Tolerances

CNC machining is the benchmark process for tight dimensional control across both metals and engineering plastics. Because the part is cut from solid stock with a precisely controlled cutting tool, the process is not subject to the shrinkage, warping, and mold-related variation that affects forming and molding processes.

CNC machined metallic components typically achieve standard tolerances of ±0.25 mm (±0.010"), making them suitable for precision applications requiring consistent dimensional accuracy. On precision-critical features such as bearing bores, mating faces, and locating datums, the numbers tighten considerably. CNC machines are renowned for their ability to achieve extremely tight tolerances, often as precise as ±0.025 mm.

The practical tiers for CNC machining are:

• Standard (commercial): ±0.25 mm (±0.010") — suitable for most structural and non-critical features
• Precision: ±0.025–0.05 mm — appropriate for mating surfaces, sliding fits, and precision assemblies
• Tight (high-precision): ±0.005–0.013 mm — achievable on selected critical features with dedicated setups, temperature-controlled environments, and enhanced inspection

An important qualifier: a number such as ±0.005 mm may be achievable on a short precision bore, a bearing seat, or a controlled mating feature, but it may be unrealistic across a long thin-wall part, a large flat surface, or a soft plastic component. It is realistic only for selected critical features when the design, material, fixture, toolpath, machine condition, and inspection method all support that requirement. Material also plays a role — metals generally hold tighter tolerances than engineering plastics, and harder alloys behave more predictably under cutting loads than soft or gummy materials.

For CNC turning (cylindrical parts such as shafts and pins), turning can hold cylindrical features more consistently because the workpiece rotates around a fixed central axis, while the cutting tool moves along the length, gradually removing material. This geometry-specific advantage means turned features often hit the tighter end of the precision range more reliably than milled faces of equivalent size.

3D Printing Tolerances by Technology

3D printing covers a wide range of technologies with significantly different tolerance capabilities. Treating "3D printing" as a single tolerance category is one of the most common and costly mistakes in early-stage product development. The right number depends on the specific process.

FDM (Fused Deposition Modeling)

FDM is the most accessible and economical 3D printing process, but it carries the loosest tolerances of the common industrial technologies. As a baseline, expect ±0.3 mm on any dimension below 100 mm, and ±0.5% on dimensions above 100 mm. Hole diameters print 0.1–0.3 mm undersize due to filament shrinkage. FDM is well suited for visual prototypes, fit-check models, and early-stage concept validation where dimensional precision is secondary to speed and cost.

SLA (Stereolithography)

SLA is the most accurate polymer 3D printing technology available at production scale. SLA is the most accurate plastic 3D printing technology available at production scale. It suits dental models, jewelry casting patterns, and fine mechanical parts where surface detail and fit matter. Typical tolerance for SLA is ±0.2% with a lower limit of ±0.1 mm. For small features under 25 mm, ±0.1 mm is reliably achievable with a well-calibrated industrial machine and appropriate resin selection.

SLS (Selective Laser Sintering) and MJF (Multi Jet Fusion)

SLS and MJF are powder-bed processes that deliver consistent functional tolerances without requiring support structures, making them well suited for complex geometries and functional prototypes. Enclosed powder maintains consistent temperature during cooling, minimizing warping. For most applications, ±0.2 mm tolerance is achievable with SLS and MJF, better than FDM by a full 0.1 mm. For SLS functional prototypes, ±0.15 to 0.2 mm is achievable and reliable.

To summarize 3D printing tolerance tiers by process:

• FDM: ±0.3–0.5 mm (standard); best for visual and concept prototypes
• SLA: ±0.1–0.2 mm; best for fine-detail parts, master patterns, and tight-fitting assemblies
• SLS / MJF: ±0.15–0.3 mm; best for functional prototypes and low-volume end-use parts requiring isotropic strength

One practical note: the Z dimension is quantized to the layer height, and each layer introduces a small positioning error. For FDM, Z tolerance is ±0.1–0.3 mm; for SLA, roughly ±0.05 mm. The rule of thumb is to orient critical dimensions in the X/Y plane.

Plastic Injection Molding Tolerances

Plastic injection molding tolerances are inherently tied to material shrinkage — the dimensional change that occurs as molten polymer cools and solidifies in the mold cavity. This means injection molding tolerances are not a fixed number; they scale with part size, resin selection, geometry, and mold quality.

In general, a typical tolerance for injection molding is ±0.1 mm, while a very tight tolerance is ±0.025 mm. The industry commonly divides these into three tiers:

• Commercial: ±0.1–0.25 mm — suitable for most consumer goods and non-critical housing features
• Fine (standard precision): ±0.05–0.075 mm — for mating surfaces, snap fits, and functional interfaces
• Precision: ±0.025–0.05 mm — for medical devices, optical components, and high-performance mechanical assemblies

A molded part shrinks as it cools, typically 0.3% to 2.5% depending on the resin, and that shrink varies with process conditions and wall thickness. The tool is cut oversize to compensate, but the residual variation is what sets the achievable tolerance, so it scales with size and resin rather than being a fixed value.

Material selection has a direct impact on what is achievable. Lower-shrinkage amorphous materials such as ABS and PC can make tight tolerances easier to maintain. Amorphous materials such as ABS, PC, PMMA, and PS generally have lower and more predictable shrinkage. Semi-crystalline materials such as PP, nylon, POM, and PET typically shrink more. For this reason, amorphous materials often make tight dimensional control easier.

Parting line placement is another critical variable: features that cross the parting line need looser tolerances than features in one mold half. Wherever possible, keeping tightly toleranced features within a single mold half significantly improves achievable precision. For applications requiring tolerances tighter than ±0.025 mm, tolerances tighter than about ±0.025 mm usually call for precision machining after molding. For those features, the part is molded close to size and then machined to final specification.

Pressure Die Casting Tolerances

Pressure die casting uses high-pressure metal injection into hardened steel tooling, which gives it notably tighter as-cast tolerances than sand casting or investment casting. Die casting tolerances are typically tight and highly repeatable due to hardened steel tooling and controlled high-pressure metal injection.

The NADCA (North American Die Casting Association) standard is the most widely referenced framework for die casting tolerances. Standard NADCA tolerances for aluminum often range from ±0.002 in/in (±0.05 mm/25 mm) for linear dimensions, with a minimum limit around ±0.005 in (±0.13 mm) for small features. In practice, the working tiers are:

• Standard (NADCA): approximately ±0.25 mm for the first 25 mm, plus ±0.05 mm for each additional 25 mm
• Precision: approximately ±0.05 mm on small, well-controlled features in a single die half — requires tighter die construction and enhanced process control

Alloy choice matters significantly for die cast tolerances. Zinc offers higher dimensional accuracy — it flows well and is less likely to change shape. Aluminum is more likely to shrink and warp during cooling. Magnesium is somewhere in between. If a part has tight fits, zinc is easier to work with.

Dimensions that cross the parting line always carry wider tolerance allowances than dimensions contained within a single die half — this is a fundamental characteristic of die casting, not a supplier limitation. Dimensional accuracy in die casting depends on the interaction of material properties, part design, mold precision, and process stability. Each of these factors can cause variations that affect how well parts meet specified tolerances. When critical precision is required beyond the as-cast capability, secondary CNC machining of specific features is a proven and cost-effective hybrid approach.

Vacuum Casting Tolerances

Vacuum casting uses a silicone mold made from a master pattern — typically an SLA 3D print — to produce small batches of polyurethane parts that closely simulate injection-molded properties. The process is widely used for pre-production validation, user testing, and bridge production before hard tooling is committed.

Vacuum casting tolerances are commonly planned around ±0.2 mm for general dimensions, while simple and well-supported features may approach ±0.1 mm under favorable geometry, resin, mold condition, and inspection conditions. For tight-fitting parts and mating interfaces, keeping tolerances below ±0.35 mm is recommended.

Two process-specific factors are worth understanding. First, the master pattern sets the ceiling for accuracy: the final part can never be more accurate than the master pattern it was molded from. The quality of the initial SLA 3D print and the skill of the model maker who hand-finishes the pattern are paramount. Second, silicone molds wear progressively over their production life: for a low-volume production run, there will be very slight dimensional variations from the beginning to the end of the run. Because vacuum casting uses a soft silicone mold, there will be very slight dimensional variations from the first part to the 25th part. The repeated mechanical and thermal stresses of the process cause the mold to wear slightly with each cycle.

When critical features require tighter control than the vacuum casting process can provide, the best practice is to combine processes. The part can be designed with these features slightly undersized. After casting, it can be put on a CNC machine to have those critical features machined to a very high tolerance. This hybrid approach gives you the best of both worlds: the speed and low cost of vacuum casting for the overall shape, and the high precision of CNC machining for the critical features.

Sheet Metal Fabrication Tolerances

Sheet metal fabrication tolerances are fundamentally different from machining tolerances because the achievable precision depends on both the feature type and the manufacturing operation used to create it. A dimension between two laser-cut holes on the same flat blank can be held much tighter than a dimension that spans multiple bends. Sheet metal tolerances are specified by feature type rather than as one blanket number.

Practical reference values by operation:

• Laser cutting (cut features on the same plane): ±0.1–0.15 mm standard; ±0.05 mm precision on thin material (under 3 mm)
• CNC bending (bend angle): ±1° standard; ±0.5° with coining and enhanced tooling
• Bend-to-edge dimensions: ±0.25 mm standard; wider for multi-bend features due to stack-up
• Welded assemblies: typically ±0.75 mm or greater due to thermal distortion
• Hole position (same flat surface): ±0.1–0.13 mm with modern fiber laser equipment

Standard commercial practice is ISO 2768-m (medium): ±0.15 mm for dimensions up to 30 mm and ±0.5° angular — the grade used on 95% of all commercial and industrial sheet metal parts. For general drawings, calling out "GENERAL TOLERANCES: ISO 2768-m" in the title block and reserving individual tighter callouts for the two to five dimensions that are functionally critical is both the most cost-effective and the most manufacturer-friendly approach.

One common mistake is applying machining-grade tolerances to formed sheet metal parts. Expecting machined-part tolerances (±0.01 mm) from sheet metal is unrealistic, since springback, material grain variation, and thermal effects from cutting and welding all introduce dimensional variation that machining processes do not encounter. Sheet metal tolerances are broader than those achievable in CNC machining. Design with that in mind when a sheet metal part interfaces with a machined component.

Compression and Silicone Molding Tolerances

Elastomeric processes — including compression molding, silicone molding, and liquid silicone rubber (LSR) molding — present inherently wider tolerance requirements than rigid-material processes because the parts are compressible and measurement itself introduces variation. Soft, flexible parts deform under the pressure of measuring instruments, which means stated tolerances always carry an implicit measurement caveat.

Practical tolerance expectations for elastomeric molding processes:

• Compression molding (rigid materials such as BMC/SMC): ±0.1–0.2 mm for dimensions in a single die half; wider across the parting line due to flash and die-closure variation
• Liquid silicone rubber (LSR) molding: ±0.1–0.2 mm on critical functional features with well-designed tooling and process control; softer durometers require wider allowances
• Standard silicone molding: ±0.2–0.5 mm depending on part size, durometer, and feature complexity

Elastomeric materials present more complex tolerance considerations due to their compressible nature. Film materials under 6.3 mm thickness can achieve ±0.25 mm tolerance for dimensions under 25 mm, while sponge materials in the same thickness range require ±0.63 mm tolerance. For high-precision sealing or functional interfaces in LSR parts, it is good practice to work with your toolmaker during the DFM stage to identify which features can be held in a single mold half, where parting line placement will introduce additional variation, and which features may require post-mold trimming or secondary operations to achieve final specification.

Choosing the Right Process for Your Tolerance Requirements

The right manufacturing process for a given tolerance requirement is not always the one that can achieve the tightest numbers — it is the one that can consistently hold the tolerance you actually need at the volume and cost point your project requires. Matching process capability to design intent, rather than defaulting to the tightest option available, is what separates efficient product development from expensive rework cycles.

A practical framework:

• Tolerances tighter than ±0.05 mm in metal: For parts requiring tolerances tighter than 0.05 mm in metal, CNC machining is the only viable process. Injection molding and 3D printing cannot reliably achieve this level of control at production volumes.
• Tolerances of ±0.1–0.25 mm in plastic: Multiple processes are viable — CNC machining for low volume, injection molding for high volume, and SLA or SLS 3D printing for prototyping.
• Tolerances of ±0.1–0.3 mm in die cast metal: Pressure die casting is well suited for medium-to-high volume production, with secondary machining available for critical interfaces.
• Tolerances of ±0.2–0.5 mm for elastomeric parts: Compression molding, silicone molding, or LSR molding, with material hardness and feature location as primary variables.
• Sheet metal parts with mixed tolerance requirements: Accept process-natural tolerances (ISO 2768-m) for general dimensions and apply tight callouts only to the few features where fit or alignment is functionally critical.

Transitioning between processes as a product moves from prototype to production also changes the tolerance baseline. A staged approach — 3D print to prototype, CNC to validate function, injection mold for final production — is standard practice, not a compromise. Each stage has its own tolerance profile, and design drawings should reflect the tolerances appropriate to the production method, not the prototyping method. The full range of manufacturing services available — from early-stage rapid prototyping through low volume, mid volume, and high volume manufacturing — means that the tolerance strategy should evolve alongside the product development stage.

Conclusion

Tolerance charts by process are most useful when treated as a working reference, not a guarantee. Every number presented here represents realistic production capability under normal conditions — real tolerances for a specific part depend on its geometry, material, feature placement, and the tooling and process maturity behind it. Published capability charts disagree, sometimes by a factor of two, because different sources assume different part sizes and different definitions of achievable. Treat every number as the middle of a band.

The practical takeaway is consistent across all processes: specify tolerances that match what your design actually needs, matched to what your chosen process can reliably deliver. Apply tight callouts to the features that govern fit, function, and assembly. Let non-critical dimensions rest at the process-natural tolerance. And when a part requires a combination of capabilities — the geometric freedom of casting with the precision of machining, or the speed of 3D printing with the accuracy of secondary CNC work — hybrid approaches are not just acceptable, they are often the most cost-effective path forward.

Understanding these numbers at the design stage eliminates the most common and costly source of tolerance problems: the assumption that any process can hold any tolerance if you just ask firmly enough on a drawing.