How to Hold ±0.002mm: Precision Mold Tolerances

0.002 mm is about one thirty-fifth of a human hair's width. It is also the distance between a lot that passes and a lot that gets sorted by hand for three shifts. A core pin ground 2 µm oversize makes the molded hole 2 µm small. On a 0.8 mm connector terminal wall, that is the difference between a clean fit and press-fit damage.

Mold shops quote ±0.002 mm easily. Holding it is a different game. It is a chain: tolerance class, steel stability, machine capability, EDM parameters, measurement temperature, assembly stack-up and trial discipline. Break any link and the part drifts. DieStrike runs this chain every week on IATF 16949 work for customers like TE Connectivity, Amphenol, Luxshare and Dongshan Precision, and this guide is the sequence we actually use. It is written for engineers who buy precision injection molding and precision machined parts, and for anyone who has seen a ±0.002 call-out and wondered what it really takes to hit it.

Skip the discipline and the costs surface fast. Flash at the parting line means manual deflashing on every shot. Short shots in a 0.8 mm wall mean scrap. A pin that drifts 2 µm in an eight-cavity tool means eight cavities of dimensionally drifting parts, which means a sorting line, a delayed launch or a warranty claim nobody can pin to one supplier. Precision mold work fails in public, and the failure is rarely one dramatic event. It is a thousand small misses that each measured fine.

The Snapshot: What ±0.002mm Actually Demands

Read the numbers the way a buyer would. The tolerance is only as good as the tightest link, and the tightest link is usually not the machine. It is the measurement system and the temperature around it. Every step below exists to protect one 2 µm number.

Work through the ten steps below in order. Then send your part file and get a DFM that says exactly where ±0.002 mm is needed, and where it is not. Start with our injection mold manufacturing overview if you want the full process context first.

How to Set the Right Tolerance Class Before Steel Is Cut

The fastest way to blow a mold budget is to draw a ±0.002 mm circle around every feature. Tolerance class is a cost driver. Tighter costs machining hours, inspection time and rework risk, and it buys nothing on features that do not need it.

Start with the part, not the tool. ISO 20457:2018 (published) is the reference standard for tolerances and acceptance conditions of molded plastic parts, and buyers apply it whenever a drawing has no tolerance block. The working rule for tooling: the cavity must hold a fraction of the part tolerance, commonly one-third or tighter (published design guidance). A part at ±0.05 mm wants a cavity around ±0.015 mm or better. A part at ±0.006 mm pushes the tool toward ±0.002 mm.

It helps to know which grade you are actually writing. At a 10-18 mm basic size, ISO 286-1 (published) sets IT5 at 4 µm and IT6 at 6 µm of total tolerance. A ±0.002 mm call-out is 4 µm wide, which is IT5 territory, the grade used for precision bearing fits. That is the neighborhood you enter when you write ±0.002 mm.

Tolerance class also decides how the mold gets quoted. A ±0.005 mm tool runs on standard CNC cycles and standard inspection. A ±0.002 mm tool spends its hours on jig grinding, wire EDM trim passes and CMM verification, and those hours have a price. When two shops quote differently on the same drawing, the difference is usually tolerance class: one plans for the call-out, the other plans to argue about it later.

← swipe to scroll →

Published reference: at 10-18 mm basic size, ISO 286-1 IT5 = 4 µm and IT6 = 6 µm total tolerance. A ±0.002 mm feature is 4 µm wide.

We assign tolerance classes during the free 24-hour DFM review. If a feature does not need ±0.002 mm, we say so on the first pass. That is where lead time and cost come back to you.

How to Specify ±0.002mm on the Drawing Without Ambiguity

A tolerance without a datum is a debate. Establish datums A, B and C per ISO 1101 or ASME Y14.5 (published) before writing any position call-out, and make sure the datums are features the shop can actually measure.

• Use true position instead of coordinate ±. A coordinate ±0.002 mm creates a square zone and lets diagonal error grow to ±0.0028 mm. A Ø0.004 mm position zone (published GD&T practice) describes the same intent with no loophole.
• Apply maximum material condition to hole positions where the fit allows it. MMC gives the machinist tolerance exactly where the assembly can afford it.
• Use profile of a surface for complex 3D geometry. A line call-out on a 2D view cannot control a curved surface.
• Remember shrink. Plastics shrink 0.3-2% (published polymer data), so the cavity is cut oversized by the shrink factor, and the cavity tolerance must absorb the variation. A ±0.002 mm molded part often means ±0.001 mm or better on the tool.
• Apply tight call-outs selectively. A connector terminal position at ±0.002 mm matters; the logo depth on the same part does not. Selective tolerancing keeps the drawing honest and the quote competitive.

One more habit: document the shrink factor on the drawing. When the cavity is cut oversized by the published shrink factor (0.3-2% for typical molding grades) and that factor is not on the drawing, every later adjustment is guesswork. Writing it down turns a trial-time argument into a verification step.

Every critical call-out should survive one question: can the measuring instrument resolve it? If not, fix the drawing before the tool, not after.

How to Choose Steel That Holds Its Geometry

Steel is not static. Heat-treatment distortion, residual stress release and grinding heat all move a part after you have cut it. The grade and the process sequence decide whether the part stays where you left it.

• P20 (28-32 HRC typical, published) for low-volume and prototype cavity work.
• 718H pre-hardened (33-38 HRC typical, published) for general production inserts, where stability beats machinability.
• S136 (48-52 HRC typical, published) for transparent and corrosive applications.
• H13 (44-52 HRC typical, published) for high-temperature resins and high cycle counts.
• D2-class tool steel (58-62 HRC typical, published) for punches and wear components.

The pins that carry the tightest numbers run hardened. Ejector and core pins at ±0.002 mm are heat-treated to HRC 62. A soft pin wears, and a worn pin is a drifted tolerance. Our core pins and inserts are a catalog item at this grade, so the hard part is not a special order.

Process order matters more than grade choice. Rough machine, stress relieve, then finish. Deep cutting removes the pre-stressed layer, and if you finish first, the steel relaxes into a different shape. Finish grinding on hard steel also generates heat: a burned surface is a re-tempered soft layer, and the pin polishes itself round after the first 10,000 shots. Coolant, light passes and spark-out are not optional at 2 µm. For the full grade comparison, read our P20 vs H13 vs S136 guide.

Stress relief is not a checkbox. Between roughing and finishing, the block should see a full stress-relief cycle so the locked-in machining stress leaves before the final cuts, not after. On hardened work we verify hardness on every heat-treatment batch instead of trusting the certificate, because a batch at HRC 58 behaves differently from one at HRC 62.

How to Match Machine Capability to the Tolerance

A machine must hold three to five times tighter than the feature it makes (published process-capability practice). Automotive buyers typically demand Cpk of 1.67 or higher on critical characteristics. A ±0.002 mm feature therefore wants a process centered inside roughly ±0.0007 mm of machine capability. If you need ±0.002 mm and the shop's most capable wire EDM is rated ±0.01 mm, the argument is over before it starts.

← swipe to scroll →

All 120+ machines sit in one factory, and nothing that touches a critical dimension is outsourced. That is how the chain stays intact. Precision machining at this grade is a discipline, not a feature list. The same floor that makes a sprue bushing makes the guide pins that align it. Every one of these is a precision machined part with its own process sheet, its own inspection step and its own traceability record. The full equipment list is on our capabilities page.

Capability is also maintained, not assumed. Machines hold their ratings only if they are qualified on a schedule: test cuts, thermal checks and positioning verification against a laser interferometer or equivalent (published machine-tool qualification practice). A jig grinder that drifted 1 µm since its last calibration is a tolerance leak nobody sees until the part fails.

How to Run Wire and Sinker EDM Without Giving Back the Microns

EDM is where most shops lose the 2 µm, usually after the machine reported the job done. The machine cuts to ±0.002 mm positioning; the process decides whether that survives.

• Plan trim passes. The first cut removes material and leaves a recast layer; three to five skim passes (standard published practice) bring geometry and surface integrity back.
• Compensate wire diameter and kerf in the program. A fresh wire spool and a worn one cut differently on the same block.
• Control flushing and clamping. A 0.3 mm rib deflects if flush pressure pushes on it, and a clamp that slips once ruins straightness.
• Run the workpiece and the machine at a stable temperature. Wire EDM is a thermal process; ±0.002 mm positioning means the tank and the block must agree on temperature.

On the sinker side, mirror finish is a parameter set, not a promise. Sodick machines finish to Ra 0.02 µm, which sits inside the published SPI A-1 mirror band of roughly 0.012-0.025 µm Ra. Electrode wear and orbital motion are managed so the final pass removes the recast layer instead of re-depositing it. And do not EDM what grinding does better: jig grinding beats EDM on roundness for pin bores every time.

EDM also decides internal geometry the way milling cannot. Deep ribs down to 0.1 mm, sharp internal corners and hardened-steel openings are wire EDM territory; milling either cannot reach them or would need the steel soft. The trade is speed: EDM is slower than milling, so the process plan reserves EDM for the features that need it and roughs the rest with the end mill.

How to Finish Critical Features with Jig Grinding and SPDT

On Waida jig grinders rated to 0.0005 mm, we finish ejector-pin bores, core-pin diameters and guide bores. Jig grinding controls roundness and taper in a way a reamer cannot guarantee at this scale.

• Spark-out passes, cutting with zero infeed, let the wheel stabilize. Skipping the spark-out is how a bore finishes 1 µm oval.
• Coolant and light infeed keep heat out of the surface. A bearing surface with grinding burn fails early no matter what the gauge says.
• Order matters: size first, surface second, size again. Polishing removes material, so a mirror finish always re-opens the dimensional question.

For optical and lens work, Toshiba SPDT at 0.0001 mm is the only process that lands mirror surfaces in nanometers of roughness. That is a different tolerance world, and it belongs on the drawing as its own class rather than as an afterthought to a machining note.

Cylindrical pins and punches follow the same logic in round. We rough-turn, heat-treat to HRC 62, then finish-grind the OD to the 2 µm class, with lapping where the print calls for bearing-grade roundness. A pin is a precision machined part with a start and an end: grinding at one end, measurement at the other.

How to Measure a 2-Micron Claim (And Not Fool Yourself)

Published metrology guidance says instrument resolution should be one-tenth of the tolerance or better. A ±0.002 mm feature is 4 µm wide, so you need 0.4 µm resolution. A caliper does not measure 2 µm. A calibrated CMM does, and only when the temperature is under control.

Tool steel expands about 11.5 µm per meter per degree Celsius (published physical constant). On a 100 mm feature, 1 °C of drift is 1.15 µm, more than half your tolerance. A part measured at 21 °C and one measured at 23 °C are two different parts. This is why parts and gages soak in the metrology room at 20 °C, the ISO 1 reference temperature (published), and why we log room temperature on every CMM run.

In-process inspection is where 2 µm is actually caught. Final inspection tells you the part is bad; in-process inspection tells you before the next operation buries the evidence. On critical features we check between EDM, grinding and polishing, because each operation can undo the previous one.

Two more habits separate real measurements from hopeful ones. Run gage R&R before trusting a new fixture: if the measurement system eats 30% of the tolerance, the part never had a chance. And for 0.5-2 mm bores, air gages beat touch probes, because there is no contact force and no stylus deflection (published practice). Under IATF 16949, every critical feature ships with calibration records, CMM reports and traceability, so the numbers are auditable, not anecdotal.

How to Manage Assembly and Tolerance Stack-Up

A mold is an assembly of precision machined parts, and the assembly has its own tolerance budget. The parting line closes flat only if every plate is flat and parallel.

• Do the stack-up math. Worst case, five plates at ±0.005 mm flatness stack to ±0.025 mm before you measure anything. Statistical stacking (root-sum-square, published engineering practice) is fairer, but only if the shop actually controls each plate.
• Use standard mold bases. HASCO, DME and MISUMI bases keep plate flatness and parallelism predictable; custom plates get surface-ground and verified before assembly.
• Dowels locate, screws pull. Dowel holes are jig-ground after heat treatment, never before, so the holes and the hardened geometry agree.
• Leader pins and bushings set repeatable alignment. A guide system at ±0.002 mm or better keeps core and cavity centered shot after shot.
• Ejector clearance is a designed gap, not a mystery. Too tight and pins gall; too loose and you get witness marks and drifted hole positions.

Shut-off areas deserve their own attention. A shut-off that seals at 0.02 mm of interference holds flash back; one that seals at zero is a flash waiting for a heat wave. We fit shut-offs for a controlled interference and verify them at trial temperature, not at room temperature.

How to Verify on the First Trial and Make T0 Count

The mold is not done until parts prove it. Trial discipline is simple: T0 checks fill, ejection and function; T1 measures critical dimensions on the CMM against the drawing. Our mold trial and sampling service runs both stages with written defect records, so the verdict is data, not opinion.

• Set the process window before judging the tool. Injection pressure, hold time and mold temperature come first; dimensions second. A part shot at the edge of the window is not a verdict on the tool.
• Design steel-safe. Gate and runner changes should remove steel, never add it. A trial correction that adds material is a re-cut.
• Measure every cavity, not the first one out. Eight cavities that differ by 3 µm between cavities is a balance problem in the process, not a cavity-size problem in the steel.
• Treat shrink as a prediction to confirm. DFM should forecast shrinkage before steel is cut; the trial either confirms the correction factors or corrects them for the next tool.

The cooling circuit gets verified in the same trial. Balanced cooling is what keeps cavity-to-cavity dimensions stable across a shift; a 5 °C difference between cavities shows up as size scatter even when every cavity is machined identically. Cycle time and dimension stability are the same measurement, viewed from two ends.

Plastic molds build in 2-4 weeks and stamping dies in 2-5 weeks, which means the trial usually arrives faster than buyers expect. That is exactly when the tolerance chain pays off, or leaks.

How to Keep the Tolerance for the Life of the Mold

A mold that holds ±0.002 mm on day one and drifts by 30,000 shots is a recurring cost, not a finished asset. Precision is a maintenance plan.

• Watch the wear parts. Ejector pins, core pins and guide components wear first. Stocked spares ship in 3-7 days, so the mold stays on its numbers instead of waiting on a re-make.
• Monitor molded parts on a schedule, not just at approval. A 1 µm creep on a core pin shows up in the part before it shows in the tool.
• Re-polish shut-offs before they flash and re-certify guide alignment at set intervals. Record every intervention so drift becomes visible history.
• Standardize the spares. HASCO, DME and MISUMI-compatible pins and springs with a minimum order quantity of one mean a worn pin is a replacement, not a re-engineering project.

The mold ships with a maintenance file: spare parts list, wear limits, inspection intervals and the CMM baseline from T1. When a cavity drifts 1 µm at 50,000 shots, the baseline tells you whether the mold moved or the process did. That document is what makes precision reproducible instead of accidental.

Frequently Asked Questions

← swipe to scroll →

The Bottom Line

A 2 µm miss becomes flash, short shots, sorting lines and a mold that never stops costing. The fix is not one magic machine. It is a controlled chain from tolerance class to trial, and that chain is what DieStrike is certified to run.

Send us your part file and get a 24-hour DFM review with a firm quotation, with ±0.002 mm reserved for the features that actually need it.