Injection Molding Wall Thickness: Design Rules

Wall thickness is the one number that sets fill pressure, cooling time, part weight and warpage before any other decision is made. For most engineering thermoplastics the practical band is 1.2–3.0 mm, adjusted for flow length, fiber content and structural load. Thicker than that and you pay in cycle time; thinner and the cavity will not fill.

Key takeaways

  • Cooling time rises with the square of wall thickness — doubling the wall roughly quadruples cool-to-eject time.
  • The practical range for unfilled engineering resins is 1.2–3.0 mm; glass-filled grades run 0.8–2.0 mm because fiber raises viscosity even as it raises stiffness.
  • Judge thickness against flow length divided by wall thickness, not a nominal number. Ratios above 200:1 need a hot runner or a wider gate.
  • Thin walls stop saving money past a point: shear rate climbs as the square of the thickness drop, and at roughly 50,000 s-1 the gate starts to show jetting and splay.
  • Ribs at 50–60% of nominal wall and bosses at 40–60% add stiffness without the thick sections that cause sink.
  • Every transition should taper at 3:1 or shallower; a step change turns a filling problem into a cosmetic one.

Why wall thickness drives cost more than any other decision

Cooling is roughly 60–70% of a typical cycle, and cool-to-eject time scales with the square of the wall: double the wall and you roughly quadruple the seconds in the tool. That is why a 2.0 mm and a 2.6 mm version of the same footprint can differ by several dollars per part at volume. The mould costs the same; the press time does not. Going thinner saves cycle time until filling pressure and shear rate become the constraint; going thicker relieves pressure but adds seconds to every shot.

Practical wall thickness ranges by resin

The table below is the range we work inside when we review a drawing, assuming reasonable flow length and no aggressive thin bosses.

Resin Typical wall (mm) Flow length ratio Note on thickness
ABS 1.5–3.0 130:1 or better Forgives small variations; sink appears above a 60% rib
PC 2.0–3.5 90–120:1 High viscosity; thin walls need high melt temperature
PP 0.8–3.0 200:1 or better Excellent flow; the widest usable band of any commodity resin
PA6 / PA66 (unfilled) 1.0–2.5 140–180:1 Low viscosity, but prone to post-mould shrinkage
PA66-GF30 1.0–2.0 80–120:1 Fiber raises viscosity; thin walls and long flow do not mix
POM 1.0–2.5 120–160:1 Sharp transitions cause voids in thick sections
PET (thin-wall) 0.6–1.2 150–200:1 Packaging territory; demands a balanced gate layout

Two rows explain most design arguments. Glass-filled PA sits at the low end of wall thickness because fiber adds stiffness, yet it flows worse than unfilled PA at the same wall. PP runs at 0.8 mm in a packaging lid while PC needs twice that for the same geometry.

How to read a wall thickness on a real drawing

Most drawings show a section, not a thickness. Start at the gate and walk the flow front by hand. A 120 mm path through a 1.5 mm wall is 80:1 — comfortable for PC, generous for PP. The same path through 0.9 mm gives 133:1, workable in PP but marginal in PC. That calculation decides whether a design needs a hot runner, a wider gate or a moved gate.

“2 mm nominal” is not the same as 2 mm everywhere. Draft reduces the modelled wall at the base of a deep draw, texture eats into the cavity surface, and a long core sags under injection pressure so local walls go thin mid-part.

We measure thickness at three places in the DFM report: the nominal section, the thinnest point after draft and texture, and the section opposite any boss or rib. Those three catch the defects the nominal figure hides.

Transitions: why 3:1 is the number that matters

Where thickness changes, the change should taper at 3:1 maximum, and 4:1 if the drawing has room. The reason is flow hesitation. Plastic arriving in a thick section cools more slowly than plastic that has already arrived in a thin section. The thin section freezes while the thick one is still flowing, the flow front stalls, and you get a hesitation mark or a short shot. The hidden result is differential packing and a warp.

Above a 4 mm step a sink mark often appears on the thick side, because that section shrinks away from the tool while the thin side has already solidified. Tapering does not remove the shrinkage; it spreads it over a distance where the surface can follow. This is where “coring out” belongs — a 5 mm pad on a 2 mm wall is a 2.5:1 step, and hollowing it to a 2 mm rim with a 0.4 mm taper fixes the sink risk and the extra weight.

Ribs, bosses and the 60% rule

Bending stiffness rises with the cube of thickness, so doubling a wall is eight times stiffer and eight times the plastic and cycle time. A rib 1.5 mm wide and 4 mm tall adds most of that stiffness at a fraction of the material.

The constraint is sink. A rib root thicker than the wall it sits on creates a local mass that shrinks more than its surroundings, and the sink telegraphs to the opposite cosmetic face. Ribs at 50–60% of nominal wall, with a 0.25–0.5 mm root radius and 1–2° of draft per side, stay on the safe side.

Bosses follow the same logic: a boss wall at 40–60% of nominal, a cored-out centre, and a rib to the adjacent wall keep the mass down. A solid 4 mm boss on a 2 mm wall is a sink source on the face below it.

Where a boss must be full height for a thread, reduce the outer diameter first: a 5.0 mm boss can go to 6.0 mm with a 0.7 mm wall and still take the same 2.5 mm screw.

Thin walls and shear: the limit nobody puts on the drawing

Apparent shear rate at the gate scales inversely with the square of the gap, so halving the wall increases gate shear four times at the same fill time. Above roughly 50,000 s-1 at the gate, typical thermoplastics start to show jetting, blush, splay from shear-generated volatiles, and in glass-filled grades, fiber breakage. The part still fills, so the drawing looks satisfied, but the surface has to be reworked or the part rejected.

Thin walls also tighten the process window: a 0.9 mm wall in PC has perhaps 10 °C of usable melt temperature range before short shot or flash appears, a 2.0 mm wall has 25 °C. The workaround is to thin the wall where it saves the most and leave the gate region thick — a gate land 0.5 mm wider and 0.3 mm deeper than the wall it feeds adds little cycle time and moves the shear peak down the curve.

What thickness costs per millimetre: a worked comparison

The table below compares the same 100 × 80 × 25 mm ABS housing at three wall thicknesses. It shows the shape of the trade-off curve rather than any particular tool’s performance.

Nominal wall Part weight Cool-to-eject* Fill pressure Shear at gate Defect risk
1.2 mm ≈31 g ≈7 s High High Short shot, blush, splay
2.0 mm ≈51 g ≈20 s Medium Low Balanced; good cosmetic surface
3.2 mm ≈82 g ≈52 s Low Low Sink, voids, longer cooling

*Cool-to-eject scales with the square of wall thickness; illustrative for ABS at a 60 °C mould.

Read the last row against the middle. Going from 2.0 mm to 3.2 mm adds 60% to part weight and roughly 160% to cooling time, and buys nothing ribs cannot. Going down to 1.2 mm saves 13 seconds per shot but pushes fill pressure and gate shear into the range where surface defects appear. The 1.6–2.0 mm band where most ABS housings land is the widest part of that curve.

When a thin wall is the right answer

Thin-wall design is legitimate and often correct. Packaging, phone housings and disposable medical parts run at 0.6–1.2 mm because material cost and cycle time dominate the business case, and those parts carry no structural load.

What changes is the tool: thin-wall parts need higher injection pressure, so the mould needs a stiffer plate stack, better support under the cavity, and vents sized for a faster fill. Gate cross-sections grow and cooling channels move closer to the surface.

Not every press can hold that pressure, so the moulder has to be chosen for it. That is why we keep mold making in-house and run molding through vetted partners: we specify the tool to the wall the part needs, not to the press we happen to own.

Our answer for wall thickness on a new drawing

Our answer: we check wall thickness at the DFM stage against flow length ratio and gate shear, not against a nominal range, and we report the three measurements that matter before any steel is cut. Our designers model in UG, run the part through Moldflow, and return a written DFM report within 3 working days at no cost.

RCH Plastic reference: our machining tolerance is ±0.005 mm on critical mould dimensions, and the moulded part tolerance that tool can then hold is ±0.01 mm on critical dimensions, subject to the resin and the part geometry. Wall thickness variation inside a single part is the most common reason a tolerance that looked achievable on paper does not hold in production.

Every claim here is backed by a document issued against your mould number: the DFM report, the CMM dimensional report on trial samples, the process parameter sheet, and trial photos and video.

Related guides in this series

Get a wall thickness review before you cut steel

Send your 3D files and resin choice and we will return a marked-up DFM report: the sections that will sink, the flow paths that will not fill, and the thickness changes worth making now rather than after T1. Request a free DFM review.