How to Design a Plastic Part for Injection Moulding — The DFM Guide

Rule 1 — Uniform wall thickness

This is the single most important rule in injection moulding design. Keep wall thickness as uniform as possible throughout the part. Thick areas cool slower than thin areas, causing shrinkage differentials that lead to sink marks (visible dents on the surface) and internal stress that warps the part.

Recommended wall thicknesses by material: PP: 1.0–2.5 mm. ABS: 1.2–3.0 mm. PC: 1.0–3.5 mm. Nylon: 0.8–3.0 mm. HDPE: 1.0–3.0 mm. POM: 0.8–3.0 mm.

If you must transition between a thick and thin section, do it gradually — use a taper over at least 3× the wall thickness difference, not an abrupt step. Abrupt transitions create stress concentrations and flow marks.

Common mistake: making a section thicker 'for strength.' In injection moulding, thickness ≠ strength. A well-placed rib on a thin wall is always stronger than a thick wall — and moulds faster, shrinks less, and costs less material.

Rule 2 — Draft angles

Every vertical wall needs a draft angle — a slight taper — so the part can release cleanly from the mould when it opens. Without draft, the part grips the mould surface and either sticks, scuffs, or requires excessive ejector force that distorts it.

Minimum draft: 1° per side for smooth surfaces. 1.5°–2° for textured surfaces (the texture acts like sandpaper — more grip = more draft needed). 0.5° is sometimes possible on short, smooth walls, but risky.

How to apply it: the draft always tapers in the direction of mould opening (the 'pull' direction). Inside walls usually draft inward; outside walls draft outward. Your moulder will advise on the pull direction during DFM review.

Common mistake: designing a part with perfectly vertical walls in CAD. It looks clean on screen but is physically impossible to eject from a mould without draft. Always add draft before sending the file out for quoting.

Rule 3 — Ribs for strength (not thick walls)

When you need to stiffen a panel or wall, add ribs on the back side instead of making the wall thicker. A rib 60% of the nominal wall thickness, 3× the wall in height, with 0.5° draft and a generous root radius, will dramatically stiffen the part without adding sink marks or cycle time.

Rib sizing rules: Rib thickness at base ≤ 60% of adjacent wall (to avoid sink on the opposite face). Rib height ≤ 3× nominal wall. Draft on ribs: 0.5°–1° per side. Root radius: 0.25–0.5× wall thickness (too sharp = stress crack; too large = thick section = sink).

Rib spacing: keep ribs at least 2× wall thickness apart. Closer ribs can trap air and cause short shots or burn marks in the valley between them.

Common mistake: ribs thicker than the wall they sit on. This creates a thick-section lump at the base of the rib → guaranteed sink mark on the visible surface.

Rule 4 — Bosses for assembly

Bosses are the cylindrical protrusions used for self-tapping screws, press-fit inserts, or locating pins. Good boss design is critical because bosses are thick features attached to thin walls — exactly the kind of thickness variation that causes sink marks.

Boss design rules: Outside diameter: 2× to 2.5× the screw diameter. Inside diameter (hole): sized to the screw/insert spec. Wall thickness of the boss itself: 60% of nominal wall (same as ribs). Connect the boss to the nearest wall with a gusset rib — never let it stand alone on a flat panel (it will sink the panel).

Common mistake: putting a boss in the middle of a large flat panel with no ribs or gussets connecting it. The thick boss creates a visible sink mark on the opposite face that no amount of process tuning can fix.

Rule 5 — Gate location and type

The gate is where molten plastic enters the mould cavity. Its location determines how the plastic fills the part, where weld lines form, and where a small gate vestige (mark) appears on the finished part.

General gate rules: Place the gate at the thickest section of the part so plastic flows from thick to thin (prevents short shots and ensures the thick area is packed under pressure while it cools). Gate into a non-cosmetic surface where possible — the gate vestige is always visible. Avoid gating directly opposite a pin or obstacle — the flow will split around it and create a weak weld line.

Gate types. Edge gate: enters from the parting line, easy to trim. Sub gate (tunnel gate): enters below the parting line, automatically shears off on ejection — cleaner but harder to tool. Pin-point gate (hot runner): leaves the smallest vestige, used for cosmetic parts and multi-cavity tools.

Common mistake: gating into a thin section because it's 'hidden.' The thin section freezes first, preventing the thick section from packing → sink marks, shrinkage, dimensional variation.

Rule 6 — Runners and cooling

The runner system delivers plastic from the machine nozzle to the gate(s). Cold runners solidify with the part and are trimmed off (material is wasted unless regrind is used). Hot runners keep the plastic molten in the runner, so only the part solidifies — zero runner waste, faster cycles, but more expensive tooling.

For multi-cavity moulds (making 2, 4, 8+ parts per cycle), balanced runners ensure all cavities fill simultaneously. Unbalanced runners → some cavities fill before others → inconsistent part quality.

Cooling channels inside the mould carry water to quench the steel. Cooling accounts for 60–80% of total cycle time. Well-designed cooling = faster cycles = lower per-part cost. Conformal cooling (channels that follow the part's contour) is the gold standard but costs more to machine.

Rule 7 — Parting line placement

The parting line is where the two halves of the mould meet. Every injection-moulded part has a parting line — it leaves a faint witness line on the part surface. Good parting-line placement hides this line on a non-cosmetic edge, avoids undercuts, and simplifies the mould.

Best practice: place the parting line at the largest cross-section of the part (the 'equator') so both halves of the mould can pull straight apart with no side actions. Avoid placing it across a cosmetic face — even a well-finished parting line is visible under close inspection.

Rule 8 — Avoiding undercuts

An undercut is any feature that prevents the part from pulling straight out of the mould. Examples: a hole perpendicular to the mould opening direction, a snap-fit hook, an internal thread. Undercuts require side actions (cams, lifters, collapsible cores) in the mould — which increase tooling cost and maintenance.

Design tips to avoid undercuts: reorient the feature to align with the pull direction. Use a bump-off (a flexible feature that deforms over the undercut during ejection, then springs back). Redesign the feature as two-piece assembly instead of a single undercut.

When undercuts are unavoidable: side actions work and are common in production moulds. Just be aware they add cost and are wear points in the tool. Discuss with your moulder early — a good DFM review will suggest alternatives before steel is cut.

Rule 9 — Radii everywhere

Sharp internal corners are the enemy of injection moulding. They concentrate stress (leading to cracks in service), impede plastic flow during filling, and create hot spots that slow cooling. Radius every internal corner — minimum 0.5× wall thickness, ideally 1× wall thickness.

External corners can be sharper (0.25× wall) because they don't concentrate stress the same way. But even external corners benefit from a small radius — it helps the plastic flow smoothly and reduces wear on the mould edge.

Rule 10 — Surface texture and finish

The mould cavity surface transfers directly to the part. A polished mould produces a glossy part. A textured mould produces a matte or patterned part. Specify the finish you want early — changing it after the mould is built means re-machining the cavity.

Key consideration: textured surfaces need more draft (1.5°+ per side) because the texture grips the part during ejection. Glossy surfaces need careful mould maintenance — any scratch on the cavity shows on every part.

Rule 11 — Tolerances — what's realistic

Injection moulding can hold tighter tolerances than most people expect — but not as tight as CNC machining. Typical achievable tolerances: ±0.05 mm on critical dimensions (with careful process control). ±0.1 mm on general dimensions. ±0.2 mm on non-critical features.

Tolerances depend on material (amorphous plastics like ABS hold tighter tolerances than semi-crystalline ones like PP), part size (bigger parts shrink more), and tool quality. Specify tight tolerances only where functionally necessary — over-tolerancing inflates tooling and QC cost.

Rule 12 — Material selection drives design

Your choice of plastic determines shrinkage rate, achievable wall thickness, snap-fit viability, surface finish quality, strength, and cost. Choose the material before finalising the design — or at least narrow it to 2–3 candidates. Designing a part in 'generic plastic' and picking the material later is a recipe for DFM revisions.

Discuss material with your moulder. A good one will recommend the cheapest plastic that meets your functional requirements — not the most expensive.

The DFM review process

Before any mould steel is cut, your moulder should review your part design for manufacturability. This is the DFM review — and it's free at any reputable moulder (including Rehman Industry). The review checks every rule above against your specific design and flags issues that would cause problems in production.

What you provide: a 3D CAD file (STEP, IGES, Parasolid) or a dimensioned 2D drawing + a physical sample if available. What you get back: a marked-up report showing: areas that need draft added, walls that are too thick or thin, rib sizing adjustments, gate location recommendation, parting line placement, undercut solutions, and estimated cycle time.

A thorough DFM review takes 1–3 days. It saves weeks in tooling rework. At Rehman Industry, DFM is the first step on every job — we won't cut steel until the design is right.

Bottom line

Good DFM doesn't limit your design — it makes it producible. Parts designed with these 12 rules in mind mould faster, cost less, look cleaner and last longer than parts designed without them. The best time to apply DFM is before the mould is built. The second best time is now.

Need a DFM review on your part? Send us the file — STEP, IGES, drawing or even a photo of a sketch. We'll review it, flag anything that needs adjustment, and quote the tooling. No charge for the review. Usually within a business day.