DFM check list for injection mold design

Here’s a practical DFM (Design for Manufacturability) check list for injection mold design you can run before quoting / steel cutting. I’m writing it like a shop-floor checklist (pass/fail + numbers).

1) Part basics (must lock first)

• Material, shrink rate, filled % confirmed (supplier + grade).
• Target appearance standard (A/B/C surfaces) and defect acceptance (sink, weld lines, gate blush, flow marks).
• Annual volume + cavitation target (1, 2, 4, 8… cavities) and machine tonnage estimate.
• Nominal wall thickness defined, with min/max tolerance.

2) Wall thickness & geometry

• Keep uniform wall: aim ±10–15% variation across the part.
• Typical nominal wall (rule-of-thumb):
  • PP/PE: 1.2–2.5 mm
  • ABS/PC: 1.5–3.0 mm
  • PA/PA66: 1.0–3.0 mm (filled needs more attention)
• Thick sections: core out to avoid sink; use gradual transitions with radius not steps.
• Corner radii: inside radius ≥ 0.5× wall, outside radius = inside + wall.

3) Draft angles (release + cosmetics)

• Minimum draft (general): 1° per side.
• Textured surfaces: add +1° to +3° depending on texture depth.
• Deep ribs/bosses/features: 0.5°–1° minimum if space is tight, but expect higher ejection force.
• Any “no-draft” cosmetic wall = flag as high risk.

4) Ribs, gussets, bosses

• Rib thickness: 0.4–0.6× nominal wall (to avoid sink).
• Rib height: ≤ 2.5–3× wall (higher = fill/warp risk).
• Rib root radius: ≥ 0.25× wall.
• Boss OD: keep wall around boss ≤ 60% of nominal; core it out.
• Screw bosses: check pilot hole, thread engagement, and crack risk (esp. PC/PA).

5) Holes, slots, shutoffs

• Through-hole core pin: length/diameter (L/D) risk:
  • Steel core pin L/D > 10 = deflection/breakage risk (flag).
• Thin shutoff land: avoid knife edges; keep shutoff ≥ 0.5–1.0 mm robust where possible.
• Side holes/undercuts: confirm if slides/lifters needed and whether part can tolerate witness lines.

6) Undercuts & parting line strategy

• Identify all undercuts early; define: no action / hand-load insert / lifter / slide / unscrew.
• Parting line must avoid key cosmetic faces where possible.
• Confirm steel-safe areas (where you can add steel later).

7) Gate & runner concept (fill, cosmetics, strength)

• Gate type choice aligned with: appearance, weld line location, vestige limit, cycle time.
• Gate location rules:
  • Gate into thicker region when possible.
  • Avoid gating into thin long flow paths without venting.
  • Avoid weld line across high-stress zones.
• Vestige requirement (e.g., “≤0.2 mm”) must be stated.
• For multi-cavity: runner balance concept (naturally balanced preferred).

8) Venting (most missed DFM item)

• Ensure vents at end-of-fill, ribs, pin bosses, and knit line zones.
• Typical vent depth (ballpark; varies by resin): 0.02–0.05 mm with adequate land + exhaust.
• Add overflow / vent features if burn risk is high.

9) Ejection (marks, sticking, deformation)

• Confirm ejection on non-cosmetic faces.
• Ejector pin count/size adequate to avoid “banana” bending.
• Add strippers / sleeves / blade ejectors where pins would mark or punch through.
• Check deep cores: add air poppet or better draft.

10) Cooling & warpage risk

• Thick sections + asymmetry = warpage risk (flag).
• Cooling feasibility: can you cool close enough to hot spots (boss fields, thick ribs)?
• If flatness is critical: require a warpage simulation (Moldflow / Cadmould) or at least a cooling review.

11) Tolerances & metrology reality

• Call out only what matters: tight tolerances drive cost.
• Typical molding tolerance (rule-of-thumb): ±0.05–0.2 mm depending on size/material/process.
• GD&T only where functional; avoid stacking “tight everywhere”.

12) Mold build details (tooling DFM)

• Steel selection (P20 / H13 / S136 etc.) aligned with resin (glass-filled = wear).
• Surface finish spec (SPI A/B/C) + texture IDs.
• Wear inserts in high-abrasion zones (filled nylon / glass).
• Serviceability: can you replace gate insert, slides, lifters quickly?

13) Sampling & documentation (avoid disputes)

• Define deliverables:
  • T0/T1 sample plan
  • First Article Inspection (FAI) dimensions list
  • CPK/PPK requirements if any
  • Appearance approval method (lighting + distance)

DFM Check — Injection Mold Design (ABS, 2.5 mm Wall)

Deep cylindrical cavity + base ring + side “teeth” feature. Key risks are sink at thickness transitions, draft for release, venting at end-of-fill, and stable ejection to avoid whitening.

Material: ABS Nominal wall: 2.5 mm Primary risk: sink + drag marks Primary need: draft + venting + balanced ejection

1) Wall Thickness & Sink Control

• 2.5 mm is a good nominal wall for ABS, but thickness stacking at the cylinder-to-base transition can create sink and internal stress.
• Prefer coring-out thick areas and using ribs instead of solid mass.
• Rib thickness: 0.5–0.6 × 2.5 = 1.25–1.5 mm.
• Rib height: keep ≤ 3× wall (≤ 7.5 mm) unless draft/ejection is improved.
• Corner radii: inside radius ≥ 0.5× wall (≥ 1.25 mm); outside radius = inside + wall.

2) Draft Angles (Release & Cosmetics)

• Inner cylinder draft: ≥ 1.0° per side (more if the cavity is deep).
• Outer walls: 0.5–1.0° per side.
• Side “teeth” faces: ≥ 1.0° to avoid drag marks / scuffing.
• If textured, add +1° to +3° depending on texture depth.

3) Parting Line & Undercut Check

• Cost-friendly approach: parting line around the base ring; cylinder formed by a central core (often on the moving side for easier ejection).
• Verify whether the “teeth” geometry creates an undercut in the opening direction.
• If any undercut exists, plan for slide / lifter (tool cost and lead time increase).
• Rule: if the feature “shadows” material in the mold opening direction, it’s an undercut.

4) Gate & Runner Concept

• Prefer gating into the base ring (edge gate / fan gate) to fill upward and reduce cosmetic risk at the top opening.
• If appearance needs a smaller vestige, consider a submarine (tunnel) gate from the base side.
• Avoid gating near the cylinder opening (higher risk of flow marks / jetting and harder venting).
• Confirm acceptable gate vestige (example: ≤ 0.2 mm) before cutting steel.

5) Venting (Critical for Deep Cavities)

• Add vents at end-of-fill areas: cylinder top edge, far ends of the base ring, and around the “teeth” feature.
• Typical ABS vent depth (shop range): 0.02–0.05 mm with proper land and exhaust path.
• Consider overflow/vent pockets if burn marks appear during trials.

6) Ejection Strategy (Prevent Whitening / Ovality)

• For a deep cylinder, use sleeve ejection or a stripper ring where possible for even release.
• Place pins on non-cosmetic faces and avoid thin ribs near the root (pin push-through risk).
• Deep cores may benefit from air poppet assist to reduce sticking.