Tolerances by Manufacturing Process: What Accuracy to Expect and Specify

Xem Studio publishes exact nominal geometry with no tolerance added and no assumption about how you will make the part. If you have a nominal STEP file, this page lists the accuracy each manufacturing process typically delivers and the tolerance to specify, so you can apply your own allowance.

How to use this page

Xem Studio files are exact nominal geometry. We add no tolerance, shrink, kerf, or clearance. The accuracy you get depends on the manufacturing process and the shop, so you apply the allowance that matches your process.

The numbers below are published capability figures from vendors and standards bodies, each with its source. Vendors disagree in places; where they do we show the range and name both sources. These are typical or default values, not guarantees. Confirm against your shop's current quote or capability page, and tighten only the features that need it.

Quick reference by process

Published default or typical tolerances. Sources for each row are listed in the section for that process.

Sources: Protolabs: Fine-Tuning Tolerances for CNC Machined Parts · Xometry: CNC Machining Service capabilities · Protolabs Network (Hubs): Manufacturing Standards · Protolabs: Sheet Metal Tolerances (one-pager PDF) · Xometry: Metal Laser Cutting · Xometry: Waterjet Cutting · RapidDirect: Waterjet Cutting Tolerances · Protolabs: Understanding 3D Printing Tolerances · Protolabs Network (Hubs): 3D Printing Dimensional Accuracy · Xometry: Manufacturing Standards · Protolabs: Injection Molding Tolerances · RMC Foundry: Casting Tolerances by Process

CNC machining

Default shop tolerance for milled and turned metal parts is ±0.005 in (±0.127 mm). Xometry states ±0.005 in for metals and ±0.010 in for plastics and composites, per ISO 2768 unless the drawing says otherwise. Protolabs quotes ±0.005 in (±0.13 mm) for its automated factory, ±0.002 in (±0.051 mm) for standard precision, ±0.0005 in (±0.0127 mm) for reamed holes, and ±0.002 in for feature locations machined on the same side. Protolabs also cites ISO 2768-1 class f for metals and class m for plastics on its semi-automated and network service.

Tolerances below ±0.001 in are available on request with a drawing and GD&T callouts (Xometry). Protolabs says tighter is often possible depending on geometry and material but gives no figure; note the requirement on the design when you upload.

ISO 2768-1 general tolerances for linear dimensions, in mm (± values). A dash means the table gives no value. Below 0.5 mm nominal, state the deviation next to the dimension.

What to send: a STEP file for geometry plus a PDF or DXF drawing that lists only the critical dimensions with their tolerances. Use ISO 286 fit codes (for example 12 H7) on bores and shafts that mate. State the general tolerance class in the title block (for example ISO 2768-m) so everything else is covered.

Sources: ISO 2768-1 linear tolerance table (AmesWeb) · Protolabs Network (Hubs): Manufacturing Standards · Protolabs: Fine-Tuning Tolerances for CNC Machined Parts · Xometry: CNC Machining Service capabilities · Xometry: Manufacturing Standards · Xometry: ISO 2768

Sheet metal, laser cutting, and waterjet

Laser-cut features on one surface: Protolabs lists ±0.005 in (±0.127 mm) for edge to edge, edge to hole, and hole to hole, and ±0.010 in for features referenced to hardware. Xometry quotes ±0.010 in nominal edge to edge on the top face and auto-quotes ±0.005 in on most materials. Hubs lists ±0.2 mm (±0.00787 in) for cutting features. Range: ±0.005 to ±0.010 in.

Bends: all vendors list ±1 degree on bend angle. Protolabs lists ±0.010 in bend to edge and ±0.015 in bend to hole or bend to bend on one surface. Across more than one bend, Protolabs lists ±0.030 in (non-cumulative) for several feature pairs; Xometry lists ±0.015 in edge to bend and ±0.030 in across a bend.

Waterjet: Xometry gives no numeric figure on its capability page beyond kerf of about 0.062 in and a minimum feature size of 2x material thickness (0.125 in minimum), and points to its ±0.010 in nominal edge-to-edge standard for waterjet and laser sheet cutting. RapidDirect states ±0.002 in to ±0.001 in typical and up to ±0.003 in for abrasive waterjet. Material thickness follows the mill tolerance of the stock, and thick cuts can show taper.

What to send: a flat DXF (laser, waterjet) or STEP of the formed part (bending), plus a drawing that lists bend angles, bend radius, and the few critical hole positions. State the material and gauge.

Sources: Protolabs: Sheet Metal Tolerances (one-pager PDF) · Protolabs: Working with Sheet Metal Tolerances · Xometry: Metal Laser Cutting · Xometry: Waterjet Cutting · Xometry: Manufacturing Standards · Protolabs Network (Hubs): Manufacturing Standards · RapidDirect: Waterjet Cutting Tolerances

3D printing

Vendors differ widely here because tolerance depends on machine, material, part size, and orientation. Values below are published defaults; critical dimensions should be flagged to the shop. Protolabs does not publish an FDM tolerance on its tolerance page.

Percent figures apply to the nominal dimension and usually have a floor in mm. 'First inch plus' figures are a fixed tolerance for the first inch (25.4 mm) of nominal size plus an added tolerance per extra inch or per percent of nominal.

What to send: STEP or 3MF is preferred where the shop accepts it; STL is accepted everywhere but carries only a triangle mesh, so smooth curves are faceted and no units or feature intent are stored. Send a drawing or note for critical dimensions and mating features.

Sources: Protolabs: Understanding 3D Printing Tolerances · Xometry: Manufacturing Standards · Protolabs Network (Hubs): 3D Printing Dimensional Accuracy · Protolabs Network (Hubs): Manufacturing Standards · Xometry: 3D Printing Tolerances

Injection molding

Protolabs separates tool accuracy from part accuracy: the mold is machined to ±0.003 in (±0.076 mm), and finished resin parts hold no better than ±0.002 in per inch (±0.051 mm/mm), which can be greater depending on resin and geometry. Hubs lists molds machined to ±0.125 mm (±0.005 in) after shrinkage adjustment, a standard part tolerance of ±0.250 mm (±0.010 in), part-to-part repeatability typically under 0.100 mm (0.004 in), and treats anything tighter than ±0.125 mm as best effort. Xometry lists mold machining of ±0.005 in plus ±0.002 in per inch for shrink calculation and part-to-part repeatability under ±0.004 in.

What to send: STEP of the finished part at nominal size. The molder applies resin shrink to the tool, so do not scale or pre-compensate the model. Add a drawing for critical dimensions and datum scheme.

Sources: Protolabs: Injection Molding Tolerances · Protolabs Network (Hubs): Manufacturing Standards · Xometry: Manufacturing Standards

Casting

Casting accuracy is graded by ISO 8062 'CT' tolerance grades. A higher CT number is a looser tolerance, and the allowed deviation grows with the raw casting size. The standard's table gives the exact plus-or-minus value for each grade and size band; read it from the standard or your foundry rather than from a rule of thumb.

One foundry's published capability by process: green sand CT11 to CT14, shell (resin-coated sand) CT8 to CT12, lost foam CT8 to CT12, vacuum casting CT8 to CT12, water glass lost wax CT5 to CT9, silica sol lost wax CT4 to CT6, high pressure die casting CT4 to CT7. This is a single-source range; foundries differ.

Cast surfaces are rough and not finish-ready. Send a STEP of the finished part and mark which surfaces are machined after casting, so the foundry can add machining allowance there. A drawing is required for any ISO 8062 grade call-out.

Sources: RMC Foundry: Casting Tolerances by Process · Engineers Edge: Casting Tolerances (ISO 8062 CT grades)

ISO 286 fits: hole basis and shaft basis

ISO 286 describes a fit with a letter and an IT grade number for each part. Uppercase letters are holes and lowercase letters are shafts. In the hole-basis system the hole is fixed at H, so its lower deviation is zero and it is never smaller than nominal, and you change the shaft letter to pick the fit. Hole basis is common because holes are made with fixed-size tools such as reamers, so one hole class reduces tooling and gauge cost. The shaft-basis system fixes the shaft at h and varies the hole.

Lower IT numbers mean tighter tolerance, and the actual width grows with nominal size. Example: a 20 H7 hole runs 20.000 to 20.021 mm. The table below uses the AmesWeb summary of ISO 286-1 preferred fits.

Xem Studio's nominal sizes are the basic size for a fit. Apply the fit class to the part and let the shop hold it. Where a process cannot hold the grade the fit needs, ask the maker how they will reach it (for example finish machining the critical feature).

Sources: AmesWeb: ISO 286-1 preferred fits · Wevolver: H7 tolerance explained (ISO 286)

Which file to send to which shop

This is general, neutral guidance. Check the shop's upload page for what it accepts.

Sources: Protolabs: Fine-Tuning Tolerances for CNC Machined Parts · Xometry: CNC Machining Service capabilities · Xometry: Manufacturing Standards · Protolabs: Injection Molding Tolerances

Questions

Do Xem Studio files include tolerance or clearance?

No. Every dimension is exact nominal geometry. You add the allowance that suits your manufacturing process, and only to the features that press, slide, run, or mate.

What is the default CNC machining tolerance?

Xometry states ±0.005 in (±0.127 mm) for metals and ±0.010 in for plastics, and Protolabs quotes ±0.005 in (±0.13 mm) in its automated factory, with ±0.002 in (±0.051 mm) for standard precision work.

What is ISO 2768-m for a 50 mm dimension?

For a nominal size over 30 to 120 mm, class m is ±0.3 mm and class f is ±0.15 mm, per the ISO 2768-1 linear tolerance table.

What tolerance can I expect from FDM 3D printing?

Published values vary: Hubs lists ±0.5% with a ±0.5 mm floor for prototyping FDM and ±0.3% with a ±0.3 mm floor for industrial FDM; Xometry lists one build layer for the first inch plus ±0.002 in per inch. Protolabs does not publish an FDM figure.

Why do vendors give different tolerances for the same process?

Machines, materials, part size, orientation, and quoting tier differ. Treat published numbers as typical defaults, and confirm critical dimensions with your shop.

What is the difference between H7/h6 and H7/p6?

H7/h6 is a snug locational clearance fit for parts that assemble and disassemble easily. H7/p6 is an interference fit that gives rigid, aligned location.

Which file format should I send, STEP or STL?

Send STEP to machining, sheet metal, molding, and casting shops, and to 3D printing shops that accept it. STL is a mesh and loses exact curves and units. Use DXF for flat laser or waterjet profiles, and add a PDF drawing for critical tolerances.

Can I rely on these numbers as guarantees?

No. They are published typical or default capabilities from the sources cited. Shops can change them, so check the current capability page or quote.

Every file on Xem Studio is drawn at exact nominal size with no tolerance added; each object lists its mating features and fit class so you or your shop can apply the right allowance for the process.