/ KNOWLEDGE · DESIGN FOR MOULDABILITY

Design for mouldability — the rules that decide your part cost

Most of an injection-moulded part’s cost is decided before any moulder sees the drawing. Wall thickness sets the cycle time, corners set the stress, ribs and bosses set the sink marks, and draft sets whether the part leaves the mould at all. The rules below are the moulding handbooks’ consensus — Harper’s Handbook of Plastic Processes, Rosato’s Injection Molding Handbook and the ARBURG practical guide — translated into what each one saves you. Bring us a drawing that follows them and the quote drops; bring us one that doesn’t and our DFM reply will show you exactly where the money is hiding.

Rule 1 — One wall thickness, everywhere you can manage it

The nominal wall is the first line on the design checklist and the most expensive thing to change later. A uniform wall fills predictably, shrinks uniformly, and comes out flat; walls that jump in thickness shrink at different rates and pull the part into warp. Where a transition is unavoidable, make it gradual, never abrupt. The handbooks even quantify how much variation a part forgives: for materials shrinking less than 0.010 in/in, keep wall variation within about ±25%; for higher-shrinkage materials, within about ±15% (Harper). One more trap with a name: a thin field surrounded by a thick perimeter makes the melt race around the frame and trap gas in the middle — racetracking. Uniform walls are the cure.

Rule 2 — Stay under 4 mm, and core out the rest

Above a nominal wall of about 4 mm (0.150 in), two bad things compound: cooling time — which grows with the square of wall thickness — stretches the cycle, and the thick core cools last, shrinks last, and leaves voids or sink. The handbook advice is blunt: avoid walls above 4 mm; if the geometry seems to demand them, core out the thick sections or consider a different process. Thickness is not strength — geometry is. Which brings us to ribs.

Rule 3 — Ribs: half the wall, three times the wall

A rib delivers the stiffness of a thick wall without the cycle time or the sink. The numbers are settled: rib thickness about 0.5× the nominal wall — thicker ribs print sink marks on the show surface — and rib height up to about 3× the nominal wall. Beyond that, use two or three narrow ribs rather than one tall one: several short ribs stiffen more, cool faster, and mould cleaner. Ribs also need their own small draft and a smooth, radiused connection to the wall they stiffen.

Rule 4 — Bosses: 2 to 2.4 times the screw

Bosses live a harder life than the rest of the part — screws, inserts and drive pins load them in ways the surrounding wall never sees. The guideline: boss outside diameter between 2.0 and 2.4× the outside diameter of the screw, insert or pin it receives, with the boss wall at 0.5× the nominal wall — the same sink-prevention logic as ribs. And keep holes at least one hole-diameter apart from each other and from edges, for strength and clean melt flow.

Rule 5 — Radius every corner

A sharp inside corner concentrates stress and chokes flow; a radius relieves both. Harper’s minimum: inside radius at least a quarter of the wall thickness. Rosato’s good-design picture goes further — inside radius around half the wall, outside radius around 1.5× the wall — because that pairing keeps the corner’s section thickness uniform, which is Rule 1 wearing armour. Either way: no sharp internal corners, anywhere, ever.

Rule 6 — Draft: the half-degree that saves the surface

Every vertical wall needs taper so the part can leave the mould. Rosato’s range: from a quarter-degree up to several degrees as circumstances allow, with a fair average of half to one degree per side. The trade is explicit: the smaller the draft, the finer the mould polish needed to release the part — you pay for missing degrees in tooling finish and ejection trouble. Textured surfaces need more draft, not less. Our draft-angle calculator converts angle to offset for your part height in seconds.

Rule 7 — Let the gate be sized by the wall

The gate is the last thing the melt passes and the first thing designed wrong. The handbooks put gate depth in proportion to the wall it feeds — Harper at no more than 50% of the nominal wall, Rosato up to about two-thirds — and the choice within that range belongs to the toolmaker, the material and the cosmetics of the gate vestige. What a buyer should check is simpler: that the quote names the gate type and location, and that the location was chosen with the flow length in mind — the distance from gate to the farthest point the melt must fill, judged against the wall thickness carrying it.

The five-minute self-check before you send a drawing

• One nominal wall, transitions gradual, variation inside the ±15–25% band for your material’s shrinkage.
• Nothing over 4 mm that couldn’t be cored out or ribbed instead.
• Ribs at 0.5× wall, no taller than 3× — several short beats one tall.
• Bosses at 2–2.4× their screw, walls at 0.5× nominal.
• Every corner radiused; every wall drafted; and — Rosato’s crude-but-effective sink test — roll an imaginary ball down each wall junction: anywhere it settles into extra mass is where a sink mark will print.

Send the drawing before you freeze it

The cheapest DFM change is the one made before the tool is cut. Send us the CAD at the draft stage — our engineers return a design-for-moulding review against exactly these rules, with the cost consequences of each finding stated plainly. Request a quote and attach the drawing; the review is part of the reply.