injection molding interactive simulator online

Cooling time scales with the square of thickness. An 8 mm (0.31 in) mass needs 7.1× longer to freeze than the 3 mm (0.12 in) wall beside it. The skin solidifies first, then the core shrinks away from it — so you get a sink mark on the outside, a vacuum void on the inside, or both.

Hold one nominal wall and keep every transition inside ±10 %. Core out anything thicker and replace the lost stiffness with ribs. Typical nominal walls: ABS 2.0–3.0 mm (0.079–0.118 in), PP 1.5–3.0 mm (0.059–0.118 in), PC 2.0–3.5 mm (0.079–0.138 in).

Cost hook: cooling is 60–80 % of the cycle. Dropping the thickest section from 8 mm to 3 mm can cut a 60 s cycle to 25–30 s — on 100,000 parts that is more money than the mold.

Plastic shrinks onto the core as it cools, so a 0° wall is an interference fit by the time the mold opens. Ejector force spikes, the part hesitates, then tears free with drag marks down the full depth. Push harder and you get stress whitening, blush, or pin punch-through.

Minimum 1.5° per side on smooth walls; 3°+ on deep ribs and cores. Add roughly 1.5° per 0.025 mm (0.001 in) of texture depth. On a 25 mm (0.98 in) deep wall, 1.5° opens 0.65 mm (0.026 in) of clearance the moment the part lifts.

Exception: a shallow, polished, 0.5 mm-tall feature can run at 0.5° if the toolmaker can draw-polish it. Below that you are paying in scrap.

A sharp inside corner does three bad things at once. The inscribed circle is 1.41× the wall, so the corner is a hot spot. The melt front stalls and shears there. And in service the stress concentration factor is about 3.0, so the corner is where the part cracks.

Inside radius 0.5 × wall, outside radius 1.5 × wall — that pair keeps the wall constant round the bend. On a 3 mm (0.12 in) wall: Ri 1.5 mm (0.059 in), Ro 4.5 mm (0.177 in). Kt drops from ~3.0 to ~1.5 and impact strength roughly doubles.

Below Ri/t = 0.3 the Kt curve climbs steeply. Above 0.8 you are only adding mass.

A full-thickness rib doubles the material at the root. That root freezes last, pulls the opposite skin inward, and the sink shows up as a line in the reflection — the one place your customer looks. On a 3 mm ABS wall expect roughly 0.08–0.12 mm (0.003–0.005 in) of sink.

Rib thickness 0.5–0.6 × wall (0.4 × for high-gloss or glass-filled), height ≤ 3 × wall, draft 0.5–1° per side, root radius 0.25 × wall, spacing ≥ 2 × wall. Need more stiffness? Add ribs, never thickness — stiffness goes with height cubed.

If the face is cosmetic and the rib still shows, texture the face or move the rib off the sightline before you argue about process.

A solid boss blended straight into the wall is the thickest point in the part. The void opens right under the screw, so the thread strips at half the torque you designed for, and the sink shows on the outside face directly opposite.

Boss OD 2.0–2.4 × hole diameter, boss wall 0.6 × nominal, root radius 0.25 × wall, and carry the load with 4 gussets rather than a solid stem. Stand the boss 0.3–0.5 mm (0.012–0.020 in) clear of a side wall and tie it in with a rib instead of merging it.

For a M3 self-tapping screw in ABS: hole 2.5 mm, boss OD 5.5–6.0 mm, boss wall ~1.8 mm on a 3 mm wall.

The hole sits in the middle of a side wall, so its axis is at 90° to the draw. A core pin carried on a slide has to pass through the wall and shut off on the core, then withdraw sideways before the part can lift. The angle pin drives it out at 25°: 36 mm of mold opening buys 18 mm of travel. Every slide adds tooling cost, witness lines on the part, extra opening stroke, and one more thing to wear or seize at 300,000 shots.

Before you accept a slide, ask whether the opening can run out to an edge of the wall. Then core steel bypasses the wall from below, forms the same opening, and pulls in the draw direction. Same function, two-plate mold. Where the hole must stay closed on all four sides, the other escapes are a lifter (internal undercuts only) or a hand loader on low volumes. Budget a typical slide at US$1,200–3,000 of tooling plus 0.5–1 s of cycle; a lifter is cheaper but only solves inside undercuts.

Honest exception: a shallow snap in a flexible material can sometimes strip off the core — roughly ≤ 5 % strain for PP or PE, almost never for glass-filled grades.

The melt splits round the hole and rejoins behind it. Where the two fronts meet, the chains are already cooling and never fully entangle — that is the weld line. It runs straight into the snap-fit. Strength there is 85–95 % of base resin for unfilled amorphous grades, but only 40–60 % once the material is glass-filled.

You cannot delete a weld line behind a hole — you can only choose where it ends up. Move the gate so the line points away from loaded or cosmetic areas, keep flow length-to-wall ratio under about 150:1, and add an overflow or thicker flow leader if it must land somewhere critical.

Fix it in the gate drawing, not at T1. Moving a gate after the mold is cut means welding and re-cutting the cavity.