Front page / What is the minimum wall thickness for injection moulding?

What is the minimum wall thickness for injection moulding?

There is no single minimum wall thickness: it depends on the resin and on how far the plastic has to flow, but Protolabs' published ranges for common resins start at roughly 0.6 to 1.1 mm.

The useful question for a first part is not "how thin can it go?" but "what nominal wall should I pick, and can every feature stay close to it?" This article walks through the published ranges, the flow-length check that sets the practical floor, and the uniformity rules that matter more than the minimum itself.

Published ranges by resin

Protolabs publishes a recommended wall thickness range for each resin family on its injection moulding design guidelines page. Komaspec publishes a "typical nominal wall" table in its plastic part design guide. The two are compared below (Protolabs' inch figures converted to millimetres, rounded to one decimal place).

For polypropylene, Protolabs' own pages disagree. Its design guidelines page lists 0.035 to 0.150 in (about 0.9 to 3.8 mm), while its article on uniform wall thickness lists 0.025 to 0.150 in (about 0.6 to 3.8 mm). Aprios also gives the lower 0.025 in figure. Komaspec gives 0.8 to 3.0 mm. Treat the lower end as something to confirm with your moulder for your exact grade.

Two general starting points are also published. Aprios suggests 1.2 to 3 mm as a reasonable range for most applications and advises keeping walls below 5 mm where possible. Wise Plastics gives roughly 1.0 to 3.5 mm (0.040 to 0.140 in) for most thermoplastics.

These are planning ranges from moulding suppliers, not guarantees. The resin data sheet and your toolmaker have the final say for a specific grade, gate layout and part size.

Flow length sets the practical floor

A wall that sits inside the published range can still fail to fill if the plastic has to travel too far. The check is the ratio of flow length (the distance from the gate to the furthest point) to wall thickness.

Komaspec gives these figures:

• Unfilled polypropylene: a flow-length-to-wall ratio of 250:1 or better.
• Polycarbonate: closer to 100:1.

Its worked example is a 300 mm polycarbonate part with a single gate and a 1.2 mm wall, which it says will not fill properly. The arithmetic shows why: 300 divided by 1.2 is 250, well past the roughly 100:1 that polycarbonate allows.

If your ratio is too high, the options are a thicker wall, a more free-flowing grade, more gates, or a gate moved closer to the centre of the part. Each has knock-on effects (gate marks, weld lines, cost), so it is worth discussing with the toolmaker before the design is frozen.

Uniformity comes first

A part with one consistent wall moulds more predictably than one that is thin in some places and thick in others. Thick sections cool last and keep shrinking after the surrounding skin has frozen, which shows up as sink marks, voids and warp.

Komaspec's guidance on uniformity:

• Pick one nominal wall for the part and hold it within about ±10 % along its length.
• Where the thickness must change, taper the transition over at least three times the wall thickness.

Wise Plastics words its transition rule slightly differently: taper over at least three times the difference in thickness. Both say the same thing in practice: no sudden steps.

Features that hang off the wall should be thinner than the wall itself. Protolabs advises that ribs, bosses and gussets should be about 40 to 60 % of the adjacent wall to avoid sink. Komaspec's design guide gives 40 to 60 % for rib bases, and its defects guide gives 50 to 60 %. Aprios says adjacent walls should be no less than 40 to 60 % of the primary wall. The article on what causes sink marks covers rib proportions in more detail.

Thicker is not a free fix

Adding thickness is the obvious answer to a weak part, but it costs cycle time. Komaspec notes that bending stiffness rises with the cube of thickness while cooling time rises with the square, so doubling a wall roughly quadruples the cooling portion of the cycle. Ribs usually give the needed stiffness with far less cooling penalty than a thicker wall.

A step-by-step check before you send a design for quote

1. Choose the resin family first, because the published range depends on it.
2. Pick one nominal wall inside the published range, ideally away from the very bottom of it.
3. Measure the longest flow path from the likely gate position and divide it by the wall; compare with the supplier's flow ratio for that resin.
4. Look for any section much thicker than the nominal wall (bosses, junctions, solid blocks) and core it out.
5. Make ribs and bosses thinner than the wall, within the published percentages.
6. Taper every change in thickness instead of stepping it.
7. Ask the toolmaker whether a mould flow analysis is worthwhile for long, thin or cosmetic parts.

Questions buyers ask

Can the toolmaker go thinner than the published range?

Sometimes, with a free-flowing grade, short flow paths and more gates, but each of those has a cost. The published ranges are where suppliers expect parts to fill reliably, so going below them is a conversation to have before the mould is cut, not a surprise afterwards.

Why does my quote say the wall is too thick?

Very thick walls are slow to cool and prone to sink marks and voids, which Komaspec ties to thick sections shrinking after the gate freezes. Aprios advises keeping walls below 5 mm where possible. A moulder will usually suggest coring out the section and adding ribs.

Does wall thickness affect part price?

Indirectly, yes. Komaspec's point that cooling time grows with the square of thickness means a thicker wall lengthens the cycle, and cycle time drives the per-part cost. More material per part adds to it as well.

Is glass-filled material different?

Komaspec lists 30 % glass-filled nylon at 1.0 to 3.0 mm, a slightly higher floor than unfilled nylon. Filled grades also shrink differently along and across the flow, so confirm the wall and the gate position with the resin supplier's data and the toolmaker.

Sources

• Protolabs, Injection molding design guidelines: https://www.protolabs.com/services/injection-molding/plastic-injection-molding/design-guidelines/
• Protolabs, Improving part design with uniform wall thickness: https://www.protolabs.com/resources/design-tips/improving-part-design-with-uniform-wall-thickness/
• Komaspec, Plastic part design for injection molding: https://www.komaspec.com/about-us/blog/plastic-part-design-for-injection-molding/
• Komaspec, Injection molding defects: https://www.komaspec.com/about-us/blog/injection-molding-defects/
• Aprios, Optimizing wall thickness in injection molding for part success: https://www.aprios.com/insights/optimizing-wall-thickness-in-injection-molding-for-part-success
• Wise Plastics, DFM 101: wall thickness and ribs: https://wiseplastics.com/blog/dfm-101-wall-thickness-and-ribs