← All Guides

DFM Checklist for Injection Molded Parts

Engineering

Why DFM before tooling

Design for manufacturing (DFM) review catches issues while they are free to fix. A wall-thickness change in CAD costs nothing; the same change after the mold is cut means re-machining steel. DFM is the highest-leverage step in any molding program — it decides whether the part fills cleanly, holds tolerance, and ships at the quoted cost.

Catching a defect in CAD is free; catching it after steel is cut costs a tool re-cut plus 1–2 weeks of schedule. A wall-thickness correction that takes minutes in CAD can add 10–30% to unit cost if the mold is already cut and re-machined. The DFM review is the single highest-ROI step — every hour spent here returns across the whole production run of 100K–5M units, so it is never the place to skip.

This checklist walks the items that most often break a first trial shot, with the numbers that the CAD review should hit before steel is cut.

The Snapshot

  • Wall thickness: hold 1–4 mm uniform; variation should stay within ±10–20% of nominal to avoid sink and void. Thick sections (>4 mm) sink; thin (<1 mm) short-fill.
  • Draft: 0.5–1° on smooth surfaces, 1–2° on textured; 0.5° per 0.025 mm of texture depth is a common rule.
  • Radii / fillets: minimum 0.25–0.5 mm; target 0.5× wall at re-entrant corners to cut stress concentration.
  • Ribs: thickness ≤ 0.5–0.6× wall; height ≤ 3× rib thickness to avoid sink on the opposite face.
  • Bosses: wall ≤ 0.6× main wall; gusseted, with 0.5–1° draft.
  • Tolerance: call ±0.1–0.2 mm general, ±0.05 mm only on critical locating/sealing features; mold steel ±0.02 mm.
  • Gate: land 0.5–2 mm; place to avoid weld lines at load-bearing features.

1. Wall thickness and uniformity

Non-uniform walls are the top cause of sink, void and warp.

  • Target: 1.5–3 mm for most resins (PA66, PPS, PP, PC/ABS, ABS); 1–2 mm thin-wall; up to 4 mm structural.
  • Variation: keep adjacent walls within ±10–20%; a thick boss next to a thin web sinks every time.
  • Section transitions: step or taper changes; never a sudden jump from 4 mm to 1 mm.
  • Thick features: use ribs/cored holes instead of solid mass to keep cross-section even.
  • Material-specific: POM and PA shrink more (1.5–2.5%), so wall balance matters more; PC needs thicker min walls (~1.5 mm) to fill.

2. Draft, radii and corners

Every vertical surface that pulls out of a cavity needs draft or it drags and scuffs.

  • Smooth surfaces: 0.5–1° minimum; 1° is a safe default.
  • Textured surfaces: 1–2°, scaling with texture depth (0.5° per 0.025 mm grain).
  • Undercut-free: if the part needs an undercut, plan a slide or lifter — it adds tool cost and cycle.
  • Cores: internal cores need draft too; springs and ejector pins assume it.

Sharp corners concentrate stress and block flow.

  • Minimum radius: 0.25–0.5 mm on all edges; 0.5× wall at internal corners.
  • Flow: radii help melt reach distant cavities; sharp corners cause hesitation marks.
  • Ejector side: break all sharp edges to avoid drag and flash at parting lines.
  • Cosmetic: fillets read cleaner than sharp intersections on visible parts.

3. Ribs, bosses, gates and weld lines

Stiffening without thickening the base wall — the core DFM skill.

  • Rib thickness: ≤0.5–0.6× wall; at 0.7× wall you start to see sink on the opposite face.
  • Rib height: ≤3× rib thickness; taller ribs need taper and may need a vent.
  • Bosses: wall ≤0.6× main wall, gusseted; 0.5–1° draft; don’t land a boss on a thin wall without support.
  • Spacing: keep ribs off the gate side where packing pressure is highest.

Gate and runner design decides fill, packing and where the part’s weak lines land.

  • Gate land: 0.5–2 mm; too long a land freezes early and starves the cavity.
  • Gate location: at the thickest section, away from critical dimensions and appearance faces.
  • Weld lines: form where flow fronts meet (around holes, opposite the gate); keep them off load-bearing and sealing features.
  • Venting: 0.01–0.03 mm vent depth at parting lines prevents burn and short fill on long thin features.
  • Multi-cavity: balance runners so all cavities fill equally — our 5M units/year button program depended on high-cavitation balance.

4. Tolerances and shrink

Tolerance is a function of the material, not a number you stamp on every feature.

  • Shrink: amorphous (ABS, PC, PEI) 0.4–0.8%; semi-crystalline (PP 1.0–2.5%, PA 1.0–2.0%, POM 1.8–2.5%, PEEK 1.0–1.5%); LSR 2–3%.
  • General tolerance: ±0.1–0.2 mm is the workable band at production volume.
  • Critical features: ±0.05 mm on locating/sealing surfaces (mold steel ±0.02 mm); our connector ran ±0.005 mm critical / ±0.02 mm general.
  • Steel-safe: cut the tool to nominal and finish the critical surfaces last, so you can trim to the measured shrink.
  • Over-tolerance: calling ±0.05 mm everywhere adds 10–30% cost with no functional gain.

5. Undercuts, threads, inserts and surface

  • Undercuts: each adds a slide, lifter or collapsible core — more tool cost and cycle; design them out where possible.
  • Threads: molded-in threads need unscrewing action; cut or chased threads are cheaper at low volume.
  • Inserts: metal inserts (our HV busbar: C11000 copper + PA6 GF30) need placement and thermal-expansion planning to avoid cracking.
  • Snap-fits: keep strain below the material’s flex limit; PP and PEI flex well, POM and PS crack if over-stressed.
  • Texture: adds draft requirement and can hide sink; specify grain depth early.
  • Gate vestige: plan to trim or locate away from appearance faces.
  • Ejector marks: position ejector pins on non-critical, hidden faces.
  • Weld-line appearance: on visible parts, gate placement controls where the line shows.

DFM review workflow

  1. CAD check — wall uniformity, draft, radii, ribs/bosses against the numbers above.
  2. Mold-flow sanity — fill, pack, warp and weld-line prediction before steel.
  3. Tolerance markup — mark only the features that locate or seal as critical.
  4. Gate plan — location, type and vestige handling agreed with the toolmaker.
  5. Steel-safe release — cut tool to nominal; finish critical surfaces post-first-shot.

Where DFM goes wrong

  • Uniform-wall skipped → sink, void, warp on first shot.
  • No draft → drag marks, scuffed surfaces, ejection damage.
  • Ribs at 0.7× wall → sink on opposite face; cosmetic reject.
  • Every feature ±0.05 mm → 30% cost premium, no benefit.
  • Gate at a weld-line on a seal → leaks in the field.

Checklist pass

Send the CAD and the material. We return a DFM report with wall/draft/rib/gate/tolerance callouts and a steel-safe tooling plan — fixing the design in CAD, not after the first trial shot.

Get a Quote