{"id":11163,"date":"2026-06-02T01:48:21","date_gmt":"2026-06-02T01:48:21","guid":{"rendered":"https:\/\/nylonplastic.com\/engineering-tolerance-guide-plastic-parts\/"},"modified":"2026-06-03T04:49:21","modified_gmt":"2026-06-03T04:49:21","slug":"engineering-tolerance-guide-plastic-parts","status":"publish","type":"post","link":"https:\/\/nylonplastic.com\/pt\/engineering-tolerance-guide-plastic-parts\/","title":{"rendered":"Guia de Toler\u00e2ncia de Engenharia para Pe\u00e7as Pl\u00e1sticas: Padr\u00f5es de Projeto e Melhores Pr\u00e1ticas"},"content":{"rendered":"

Plastic parts do not hold tolerances like metal parts \u2014 and expecting them to is the single most common cause of production delays, cost overruns, and supplier disputes in injection molding and CNC machining. A turned aluminum part can reliably hold plus or minus 0.025 mm; an injection molded PA66 part in the same geometry will struggle to hold plus or minus 0.15 mm once moisture conditioning, mold wear, and process variation are factored in.<\/p>\n

This guide translates ISO 2768, DIN 16901, and decades of production data into practical tolerance tables for each manufacturing process and material. Use these numbers at the design stage to avoid the expensive discovery that your plus or minus 0.05 mm drawing note was never achievable in the first place.<\/p>\n

Tolerance Capability by Manufacturing Process<\/h2>\n\n\n\n\n\n\n\n\n\n\n
Processo<\/th>\nTypical Tolerance<\/th>\nBest Case<\/th>\nWorst Case<\/th>\nKey Limiting Factor<\/th>\n<\/tr>\n<\/thead>\n
CNC Machining (plastic)<\/td>\nplus or minus 0.05-0.10 mm<\/td>\nplus or minus 0.025 mm<\/td>\nplus or minus 0.25 mm<\/td>\nThermal expansion during cutting<\/td>\n<\/tr>\n
CNC Machining (metal)<\/td>\nplus or minus 0.025-0.05 mm<\/td>\nplus or minus 0.005 mm<\/td>\nplus or minus 0.15 mm<\/td>\nTool deflection<\/td>\n<\/tr>\n
Injection Molding (unfilled)<\/td>\nplus or minus 0.10-0.30 mm<\/td>\nplus or minus 0.05 mm<\/td>\nplus or minus 0.50 mm<\/td>\nShrinkage variation 0.1-0.3%<\/td>\n<\/tr>\n
Injection Molding (GF30)<\/td>\nplus or minus 0.08-0.20 mm<\/td>\nplus or minus 0.05 mm<\/td>\nplus or minus 0.40 mm<\/td>\nAnisotropic shrinkage; mold wear<\/td>\n<\/tr>\n
3D Printing (SLS nylon)<\/td>\nplus or minus 0.15-0.30 mm<\/td>\nplus or minus 0.10 mm<\/td>\nplus or minus 0.50 mm<\/td>\nLayer resolution; powder bed shrinkage<\/td>\n<\/tr>\n
3D Printing (SLA resin)<\/td>\nplus or minus 0.10-0.20 mm<\/td>\nplus or minus 0.05 mm<\/td>\nplus or minus 0.30 mm<\/td>\nPost-cure shrinkage; support marks<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

Material-Specific Tolerance Guidance<\/h2>\n

Not all plastics are created equal when it comes to dimensional stability. The key differentiators are: shrinkage<\/strong> (higher = wider tolerance band), moisture absorption<\/strong> (nylon swells, PP does not), and coefficient of thermal expansion (CTE)<\/strong> (determines how much a part changes size between molding and room temperature). The table below shows realistic tolerance expectations for a 100 mm long feature in a well-designed production mold.<\/p>\n\n\n\n\n\n\n\n\n\n\n\n
Material<\/th>\nTolerance (100mm feature)<\/th>\nShrinkage Range<\/th>\nCTE (10^-6\/deg C)<\/th>\nMoisture Effect<\/th>\n<\/tr>\n<\/thead>\n
ABS (unfilled)<\/td>\nplus or minus 0.08-0.15 mm<\/td>\n0.4-0.7%<\/td>\n70-90<\/td>\nMinimal (under 0.1%)<\/td>\n<\/tr>\n
PC (unfilled)<\/td>\nplus or minus 0.08-0.15 mm<\/td>\n0.5-0.7%<\/td>\n65-70<\/td>\nMinimal (under 0.15%)<\/td>\n<\/tr>\n
PA66 (unfilled, dry)<\/td>\nplus or minus 0.12-0.25 mm<\/td>\n1.5-2.0%<\/td>\n70-90<\/td>\n+0.5-1.5% dimension at 50% RH<\/td>\n<\/tr>\n
PA66-GF30<\/td>\nplus or minus 0.08-0.18 mm<\/td>\n0.2-0.6%<\/td>\n20-30<\/td>\n+0.3-0.8% (reduced by glass content)<\/td>\n<\/tr>\n
PP (unfilled)<\/td>\nplus or minus 0.15-0.35 mm<\/td>\n1.0-2.5%<\/td>\n100-150<\/td>\nNegligible<\/td>\n<\/tr>\n
POM (Delrin, acetal)<\/td>\nplus or minus 0.08-0.20 mm<\/td>\n1.8-2.5%<\/td>\n100-120<\/td>\nMinimal (under 0.2%)<\/td>\n<\/tr>\n
PEEK (unfilled)<\/td>\nplus or minus 0.10-0.20 mm<\/td>\n1.0-1.5%<\/td>\n47-55<\/td>\nMinimal (under 0.1%)<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

DIN 16901: The Plastic-Specific Standard<\/h2>\n

DIN 16901 defines tolerance grades specifically for plastic molded parts, recognizing that plastics have larger and more variable shrinkage than metals. It uses a series of tolerance groups based on nominal dimension range. For a 100 mm feature, DIN 16901 fine tolerance corresponds to approximately plus or minus 0.18 mm for unfilled semi-crystalline materials like PA66 \u2014 roughly 6x the tolerance that ISO 2768-m (medium) specifies for machined metal of the same size. This standard, not ISO 2768, should be referenced on plastic part drawings to establish realistic expectations with mold makers and molding suppliers.<\/p>\n

Design Rules for Plastic Tolerances<\/h2>\n
\n
    \n
  1. Specify tolerances only where needed:<\/strong> Do not apply blanket tolerances to entire parts. Every tolerance on a drawing costs money \u2014 the mold maker must hold it, the molder must verify it, and both will charge for it. Use general tolerances for non-functional surfaces (ISO 2768 or DIN 16901 reference) and specific tolerances only for bearing fits, seal surfaces, and assembly interfaces.<\/li>\n
  2. Add 0.05 mm per 100 mm for moisture-sensitive materials:<\/strong> Nylon (PA6\/PA66) parts change dimension by 0.5-1.5% between dry-as-molded and 50% RH equilibrium. A 100 mm PA66 feature that measures 100.00 mm fresh from the mold will measure 100.50-101.50 mm after conditioning. Either specify the measurement condition (dry or conditioned) or widen the tolerance to absorb the moisture effect.<\/li>\n
  3. Mold tolerance is not part tolerance:<\/strong> A mold cavity machined to plus or minus 0.01 mm will not produce parts at plus or minus 0.01 mm. The molding process adds variation from: shrinkage (1-2% of dimension), mold temperature fluctuations (plus or minus 3 deg C = plus or minus 0.03 mm on 100 mm), and packing pressure variations. Budget 3-5x the mold tolerance for the final part tolerance.<\/li>\n
  4. Critical tolerances go near the gate:<\/strong> Dimensions closer to the gate see higher packing pressure and lower shrinkage variation. A 100 mm long part with tolerance-critical features at the far end (opposite the gate) will have 2-3x the dimensional variation of the same features located near the gate. Design the gate location to feed critical features first.<\/li>\n
  5. Account for mold wear over life:<\/strong> Mold cavities erode 0.001-0.003 mm per 10,000 shots for unfilled plastics, and 0.005-0.015 mm per 10,000 shots for glass-filled grades. Over a 200,000-shot life, GF30 can open a cavity by 0.1-0.3 mm. Design to the middle of the tolerance band at mold launch so the part stays in-spec as the cavity wears toward the upper limit.<\/li>\n
  6. GD&T for plastics: use profile, not position:<\/strong> Plastic parts flex, shrink unevenly, and have draft angles. True position (plus or minus circular zone) is physically meaningful for rigid metal parts but not for a molded plastic boss that tilts after ejection. Use surface profile tolerances instead \u2014 they define a 3D zone the surface must lie within without assuming it is perfectly oriented. Concentricity and symmetry should be avoided entirely on plastic parts; they are not physically verifiable on non-rigid parts.<\/li>\n<\/ol>\n<\/div>\n

    Industry Application Matrix<\/h2>\n

    Industry Application Matrix<\/h2>\n\n\n\n\n\n\n\n\n
    Ind\u00fastria<\/th>\nTypical Parts<\/th>\nMaterial\/Grade<\/th>\nKey Requirement<\/th>\n<\/tr>\n<\/thead>\n
    Dispositivos m\u00e9dicos<\/td>\nSyringe plungers, luer fittings, inhaler bodies<\/td>\nplus or minus 0.05-0.10 mm on critical seals<\/td>\nISO 13485; functional rather than dimensional validation<\/td>\n<\/tr>\n
    Autom\u00f3vel<\/td>\nConnector housings, sensor brackets, fluid fittings<\/td>\nplus or minus 0.10-0.20 mm<\/td>\nTemperature range -40 to +120 deg C; must fit after thermal cycling<\/td>\n<\/tr>\n
    Eletr\u00f3nica de consumo<\/td>\nPhone cases, laptop housings, wearable bands<\/td>\nplus or minus 0.08-0.15 mm on cosmetic gaps<\/td>\nGap-and-step visible quality metric; 0.1 mm gap visible to user<\/td>\n<\/tr>\n
    Equipamento industrial<\/td>\nGear housings, bearing seats, pump bodies<\/td>\nplus or minus 0.10-0.25 mm<\/td>\nMust maintain fit after oil\/chemical exposure and temperature cycling<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

    Cost Decision Framework<\/h2>\n
    \n

    Tolerances drive mold cost non-linearly:<\/strong> A mold designed for plus or minus 0.20 mm might cost $12,000. The same part geometry tightened to plus or minus 0.10 mm adds $5,000-8,000 for higher-precision machining, hardened steel, and conformal cooling. Tightening further to plus or minus 0.05 mm adds another $8,000-15,000 \u2014 bringing the total to 2-3x the cost for a 4x tighter spec.<\/p>\n

    The process trade-off:<\/strong> If the part truly needs plus or minus 0.05 mm or better, injection molding may be the wrong process. CNC machining from plastic stock achieves plus or minus 0.05 mm at lower tooling cost ($0 mold, $15-50\/part machining) for volumes under 500. Above 5,000 pcs, the per-part machining cost usually exceeds the amortized mold cost.<\/p>\n

    Decision rule:<\/strong> Design parts at plus or minus 0.15 mm for injection molding as the baseline. Tighten only the features that absolutely require it \u2014 bearing seats, seal grooves, snap-fit engagement surfaces. Each tightened tolerance adds cost; each unnecessary tolerance guarantees disputes.<\/p>\n<\/div>\n

    Common Defects and Solutions<\/h2>\n\n\n\n\n\n\n\n\n
    Defect<\/th>\nAppearance<\/th>\nRoot Cause<\/th>\nSolu\u00e7\u00e3o<\/th>\n<\/tr>\n<\/thead>\n
    Out-of-tolerance after conditioning<\/td>\nPart measures in-spec dry but out-of-spec after moisture<\/td>\nNylon absorbed 1.5-2.5% moisture, swelling 0.5-1.5%<\/td>\nSpecify conditioning before measurement; widen tolerance or use GF grade<\/td>\n<\/tr>\n
    Mold shrinkage variation<\/td>\nCavity-to-cavity or shot-to-shot variation over 0.1 mm<\/td>\nProcess instability: melt temp plus or minus 5 deg C, hold pressure drift<\/td>\nStabilize process within plus or minus 3 deg C and plus or minus 50 PSI; add SPC on critical dimensions<\/td>\n<\/tr>\n
    Warpage causing out-of-spec<\/td>\nPart twists after ejection, dimensions shift<\/td>\nDifferential cooling; anisotropic GF orientation<\/td>\nUse mold flow analysis; balance cooling; reposition gates for symmetric fill<\/td>\n<\/tr>\n
    Tool wear exceeding tolerance<\/td>\nCavity dimensions growing over production run<\/td>\nGF abrasion on soft steel; high injection velocity at gate<\/td>\nUpgrade to H13\/D2; hard chrome wear surfaces; monitor every 25K shots<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

    Why Choose Nylon Plastic for Your Project<\/h2>\n
    \n
    \n
    🏭<\/div>\n

    Precision Manufacturing<\/h4>\n

    30+ CNC & injection molding cells under one roof<\/p>\n<\/div>\n

    \n
    🔬<\/div>\n

    ISO 9001:2015<\/h4>\n

    Certified quality system, full inspection reports<\/p>\n<\/div>\n

    \n
    ⚡<\/div>\n

    15-25 Day Lead Time<\/h4>\n

    Fast turnaround with expedited options available<\/p>\n<\/div>\n

    \n
    🌍<\/div>\n

    Global Shipping<\/h4>\n

    Air & sea freight to North America, Europe, Asia<\/p>\n<\/div>\n<\/div>\n

    \n

    Download Our Engineering Tolerance Guide<\/h3>\n

    Free PDF reference guide with technical data, design rules, and supplier checklists.<\/p>\n

    📥 Download Engineering Tolerance Guide (PDF)<\/a><\/div>\n

    Artigos relacionados<\/h2>\n
    \n
    Core and Cavity Design<\/a><\/div>\n
    Chamfer vs Fillet Guide<\/a><\/div>\n
    Die Casting vs Injection Molding<\/a><\/div>\n
    SPI Surface Finish Standards<\/a><\/div>\n<\/div>\n

    Perguntas mais frequentes<\/h2>\n
    \nWhat is the tightest achievable tolerance for plastic injection molded parts?<\/strong><\/summary>\n

    For unfilled amorphous materials (ABS, PC) on a well-designed mold: plus or minus 0.05 mm is achievable on features under 50 mm near the gate. For semi-crystalline materials (PA66, POM, PP): plus or minus 0.08-0.10 mm is the practical floor. These numbers assume: hardened mold steel (H13+), tight process control (plus or minus 3 deg C, plus or minus 50 PSI), and measurement at a defined moisture content. Commercial molding at competitive prices should budget plus or minus 0.15 mm as the standard tight tolerance \u2014 anything tighter requires negotiation, higher cost, and documented capability studies.<\/p>\n<\/details>\n

    \nWhy are plastic tolerances wider than metal tolerances?<\/strong><\/summary>\n

    Three physical reasons: (1) Shrinkage \u2014 plastics shrink 0.5-2.5% during cooling, and that shrinkage varies with process parameters and part geometry. Metals shrink far less and at a consistent rate. (2) Moisture absorption \u2014 nylon absorbs 2-8% water by weight, swelling 0.5-1.5% in dimension. Metals do not absorb water. (3) Viscoelasticity \u2014 plastics creep under load and relax after ejection. A molded plastic part measured 5 minutes after ejection will measure differently 24 hours later as internal stresses relax. None of these three factors apply to metals in the same magnitude.<\/p>\n<\/details>\n

    \nCan I use GD&T (geometric dimensioning and tolerancing) on plastic parts?<\/strong><\/summary>\n

    Yes, but with caution. Standard GD&T (ASME Y14.5) assumes rigid parts \u2014 a valid assumption for metals but not for plastics that flex, creep, and change shape with temperature and moisture. Recommendations: (1) Use surface profile for form control instead of flatness\/straightness \u2014 it defines a 3D tolerance zone without assuming rigidity. (2) Avoid concentricity and symmetry \u2014 they require simultaneous measurement of opposing points, which is physically meaningless on a compliant part. (3) Specify the measurement condition (temperature, moisture, time after molding). (4) Reference DIN 16901 for plastic-specific tolerance grades alongside GD&T callouts.<\/p>\n<\/details>\n

    \nDo different plastic materials require different tolerance expectations?<\/strong><\/summary>\n

    Yes, significantly. Amorphous plastics (ABS, PC, PS) shrink less and more uniformly than semi-crystalline plastics (PA, PP, POM, PEEK). For the same 100 mm feature, ABS can hold plus or minus 0.08-0.15 mm while unfilled PP needs plus or minus 0.15-0.35 mm. Glass-reinforced grades shrink less but more anisotropically \u2014 the flow-direction tolerance may be tighter than unfilled while the cross-flow tolerance is wider. Nylon adds moisture-driven dimensional change that must be accounted for regardless of glass content. Always specify tolerances by material, not as a blanket note \u2014 the supplier needs to know which material the tolerance applies to.<\/p>\n<\/details>\n\t\t\t

    \n\t\t\t