What is the recommended wall thickness for injection moulding?

For most engineering thermoplastics the practical range is 1.5-3.5 mm, with uniformity more important than the exact value. Walls below about 0.8-1.0 mm need short flow paths and high-flow grades; walls above 4-5 mm extend cycle time and risk sink and voids.

How much can wall thickness vary within one part?

Keep variation within about 15-25% of the nominal wall where the design allows it, and make unavoidable transitions gradual — a taper of roughly 3:1 length-to-thickness-change. Abrupt steps cause flow hesitation, sink marks and residual stress.

How does wall thickness affect cost per part?

Cooling time — the largest share of cycle time — scales roughly with the square of wall thickness. A 3.0 mm wall cools about 4x slower than a 1.5 mm wall, so unnecessary thickness directly multiplies unit cost at production volume.

What is the minimum wall thickness for injection moulding?

Standard parts bottom out around 0.8-1.0 mm depending on material flow and part size; thin-wall packaging processes reach 0.4-0.6 mm with high-flow PP and dedicated tooling. Feasibility depends on flow length — long, thin flow paths are the limiting factor.

Why do thick walls cause sink marks and voids?

Thick sections stay molten long after the surface skin forms. As the core finally cools it contracts and either pulls the skin inward (sink mark) or separates internally (void). Coring out thick regions to a uniform shell removes both risks and shortens the cycle.

How do I add strength without thicker walls?

Use ribs at 40-60% of the nominal wall thickness, with height below about 2.5-3.0x the wall, plus gussets at bosses and corners. A ribbed 2.5 mm shell is stiffer, lighter and faster to mould than a solid 5 mm wall. Nordmould checks rib geometry in every DFM review.

Injection Moulding Wall Thickness: Recommended Ranges for 20+ Materials

Uniform wall thickness is the first rule of injection-moulding design because it controls fill, cooling, shrinkage, strength and cost at once. The target for most parts is a constant wall in the 1.5-3.5 mm band, cored-out thick regions, and gradual transitions where thickness must change. Nordmould measures wall-thickness distribution on every STEP file in its free DFM review.

What wall thickness should each material use?

Recommended ranges for typical parts at normal flow lengths. Thin end needs short flow paths; thick end raises cycle time and sink risk.

Material	Recommended wall (mm)	Material	Recommended wall (mm)
ABS	1.5-3.5	PBT	1.3-3.0
ASA	1.5-3.5	PBT-GF30	1.0-3.0
PC	1.0-3.5	PET	1.5-3.0
PC/ABS	1.5-3.5	PPS	1.0-3.0
PMMA	1.5-3.5	PEEK	1.5-3.0
SAN	1.5-3.5	PEI (Ultem)	1.5-3.0
PS (GPPS/HIPS)	1.2-3.5	PSU	1.5-3.5
PP	1.5-4.0	LCP	0.5-2.0
HDPE / LDPE	1.5-4.0	PVC (rigid)	1.5-4.0
PA6 / PA66	1.0-3.0	TPE / TPU	1.5-5.0
PA-GF30	1.0-3.0	PA12	1.0-3.0
POM (acetal)	1.5-3.5	PLA	1.5-3.5

Why does uniformity matter more than the number?

Cooling is the problem. A thick section next to a thin one stays molten longer, shrinks more, and drags on its neighbour as it freezes. The visible results are sink marks over thick zones, warpage across the boundary, and residual stress that appears later as cracks.

The working limits: hold thickness variation to roughly 15-25% of nominal where possible, and where a change is unavoidable, run it through a taper of about 3:1 — 3 mm of transition length per 1 mm of thickness change. Sharp steps also cause flow hesitation: the melt races down the thin channel and stalls at the thick one, leaving flow lines and weld lines in the wrong places.

How does wall thickness drive cost?

Cooling time is the largest single share of the moulding cycle, and it scales roughly with the square of wall thickness. The arithmetic is brutal: a 3.0 mm wall cools about four times slower than a 1.5 mm wall, and a 4.5 mm wall about nine times slower.

At production volume that is a direct unit-cost multiplier — machine time is billed by the hour. Reducing a housing wall from 3.0 mm to 2.0 mm can cut cycle time by 30-50% while also saving resin. Wall thickness is the biggest single part-cost lever a designer controls; the cost-per-part guide shows the full calculation.

How do you design thick regions correctly?

Core them out. Replace any solid mass above about 4-5 mm with a uniform shell supported by ribs — the classic example is converting a solid bossed block into a hollow shell with gussets. Where a functional thick feature is unavoidable, isolate it from cosmetic faces and expect a longer cycle.

Ribs are the strength substitute for thickness: 40-60% of nominal wall in rib thickness, height up to about 2.5-3.0x the wall, root radius around 0.25x rib thickness, and 0.5-1° of draft per side. A correctly ribbed 2.5 mm shell usually beats a 5 mm solid wall on stiffness-to-weight, cycle time and cosmetic quality simultaneously.

What about very thin walls?

Below about 1.0 mm the question shifts from cooling to filling: can the melt reach the end of the flow path before it freezes? The limit is the material's flow-length-to-thickness ratio against your longest flow path — high-flow grades (high-MFI PP, thin-wall PA, LCP) and multiple gates extend it.

Practical floors for standard tooling: around 0.8 mm for small parts in flowing materials, 1.0-1.2 mm for medium parts, and 1.5 mm as a safe default for large housings. True thin-wall work (0.4-0.6 mm packaging) needs dedicated high-speed machines and is a specialist process. If your design sits near the floor, raise it in the DFM review — gating strategy decides whether it fills.