What wall thickness should an injection molded part use?
- Share
- Issue Time
- Oct 20,2026
The short answer
Most moulded parts land between 1.5 and 3.0 mm: ABS 1.5 to 3.5 mm, PC 1.5 to 3.0, 30 percent glass-filled PA66 1.2 to 3.0. Keep the wall uniform, taper any change at 3:1, and hold ribs at 40 to 60 percent of the wall. Thin walls fail on flow length, thick ones on sinks.
Why the wall is the first number you fix
Wall thickness sets three things at once, and only one of them is strength. It sets how far the melt has to travel before the cavity is full, it sets how long the part has to stay in the tool before it is stiff enough to eject, and it sets how much material shrinks where. Because cooling time rises faster than thickness, roughly with the square of it, a wall that is twice as thick does not take twice as long to cool; it takes several times as long, and that time is paid on every shot for the life of the tool. This is why thickness is usually the first line of a DFM report and the last thing a designer wants to change.
The second effect is dimensional. A thick section cools from the outside in: the skin freezes while the core is still molten and shrinking, and the difference has to go somewhere. In a soft unfilled resin it pulls the surface in and leaves a sink mark; in a stiff or glass-filled resin it leaves an internal void instead. Uneven walls produce the same argument at a larger scale, because a thin section freezes before the adjacent thick one and the two shrink by different amounts. The result is warp, and warp is a tolerance problem that no amount of inspection sorts out after the fact.
A working range by resin
The numbers below are starting points for a normal part with a moderate flow path, not limits. They move with glass content, flow length, gate position and the mould's cooling design, and the resin data sheet plus a flow simulation always outrank a table.
| Resin | Common nominal wall | Practical floor | What usually goes wrong | Commercial tolerance |
|---|---|---|---|---|
| ABS | 1.5 to 3.5 mm | 0.75 to 0.8 mm | sink over bosses and ribs | plus or minus 0.10 mm |
| Polycarbonate | 1.5 to 3.0 mm | 1.0 mm | high viscosity, stress marks | plus or minus 0.12 mm |
| PA66 with 30 pct glass | 1.2 to 3.0 mm | 0.8 mm | warp from fibre orientation | plus or minus 0.15 mm |
| PP | 1.0 to 2.5 mm | 0.6 to 0.9 mm | high shrinkage, warpage | plus or minus 0.15 mm |
| POM | 1.0 to 3.0 mm | 0.5 to 0.8 mm | shrinkage along flow direction | plus or minus 0.10 mm |
| PEEK | 1.5 to 3.0 mm | 1.0 mm and up | needs hot tool, high melt | plus or minus 0.10 mm |
The tolerance column is there because thickness and tolerance are usually specified on the same drawing and priced together. A commercial grade of plus or minus 0.10 mm and a precision grade of plus or minus 0.025 mm are not a small step in tool cost; on a part with features on both faces they can be the difference between a two-plate tool and one with a ground, re-worked cavity. Put the tight tolerance only on the dimensions that touch another part.
Uniformity beats thinness
Given the choice between a part with a 2 mm wall everywhere and a part with 1.2 mm walls and a 4 mm boss, the first is easier to mould and usually cheaper, even though it weighs more. That is counter-intuitive until you watch a tool run: the thin part fills faster but warps, the thick boss stays molten after the rest has frozen and has to be packed, and the cycle is set by the slowest section to cool, not the fastest. Material saved in the wall is often paid back in cycle time and scrap.
When a thickness change is unavoidable, taper it. The standard rule is a transition length of about three times the thickness difference, so a step from 3 mm to 2 mm should spread over roughly 3 mm of length rather than happening at a shoulder. A gradual taper keeps the melt front moving as one front; a step creates a hesitation effect where the thin side freezes first and the thick side over-packs, and it concentrates stress exactly where the part will later crack.
Ribs, bosses and the 40 to 60 percent rule
A rib is a way to buy stiffness without buying thickness, and it only works if the rib is thin enough at its base. The usual band is 40 to 60 percent of the adjacent nominal wall: 60 percent is safe in low-shrinkage resins such as polycarbonate, while high-shrinkage grades such as PP and PE want the bottom of the band. A rib drawn at the full wall thickness is a thick section in disguise and will telegraph a sink mark onto the opposite face, which on a cosmetic part is a scrapped moulding.
The rest of the rib geometry follows the same logic. Height is usually capped at about three times the wall, because a taller rib is hard to fill and hard to vent at the tip. Spacing of at least twice the wall keeps enough steel between ribs for cooling channels and prevents a weak, hot core. A base radius of 0.25 to 0.5 of the wall reduces the stress concentration at the root and improves flow into the rib. Bosses are the same problem in cylindrical form: an outer diameter of about 2.5 times the screw's major diameter, wall thickness at 60 percent of the nominal wall or less, and a connection to the side wall by ribs or gussets rather than standing as an isolated column of hot plastic.
Thin walls and the flow-length limit
A thin wall is not simply a scaled-down version of a thick one, because the melt has to travel further relative to the section it is travelling through. The working measure is the flow path divided by the wall thickness. Most unfilled grades fill a ratio of roughly 100 to 200 before injection pressure runs out; glass-filled grades manage less because the fibres raise viscosity, and a long, thin part may need a second gate rather than a higher pressure.
When the ratio is exceeded, the failure mode is predictable. The part short-shots at the far end, or it fills but the last region to arrive is over-packed and stressed, which shows up as a weld line, a gloss difference or a crack in service. Raising melt temperature and pressure buys a little; moving the gate buys a lot. In thin-wall packaging the ratio is pushed far past these numbers on purpose, with high-speed injection and hot runners, but that is a different tool and a different machine, not a tweak to a standard mould.
When a thick section is the right answer
Some parts need mass, and pretending otherwise causes more problems than it solves. A section that carries a thread, a bearing, a press-fit insert or a wear surface needs enough material around it to take the load without cracking, and that is often 3 mm or more regardless of what the wall average says. The same applies to a part that must resist impact at low temperature, where a thin wall in a brittle resin will shatter rather than deform.
The correct response is to localise the thickness rather than spread it. Core out the middle of a thick boss and keep the walls, add ribs instead of a solid web, and place the thick section where it can be fed and cooled rather than in the middle of a large flat face. If the thick region cannot be avoided, expect a longer cycle and plan for it in the piece price rather than discovering it at first article.
What to put on the drawing
State the nominal wall, the tolerance on it, and the rule for changes. A note such as "nominal wall 2.0 mm plus or minus 0.10 mm; all thickness transitions 3:1" tells the toolmaker what the design intends and gives the inspector something to measure. Dimension the wall at a defined plane, not across a drafted face, and keep the critical dimensions on a separate list rather than applying a tight block tolerance to everything.
The process context for these numbers is on the injection moulding page, the parts made with them are listed under plastic injection moulding, and where a wall cannot be moulded thin enough, CNC machining covers the machined alternative.
Scope and sources. The common design ranges and practical floors for ABS, polycarbonate, nylon, POM, PP and PEEK, the 40 to 70 percent rib guidance and the worked example of a 2 mm wall with a 6 mm boss are from a wall thickness and rib design reference. The 3:1 transition taper, rib base radius of 0.25 to 0.5 of the wall, boss outer diameter of about 2.5 times the screw diameter and the rib height limit of three times the wall are from a moulding design guide. The commercial and precision tolerance classes of plus or minus 0.10 and plus or minus 0.025 mm, the nominal wall bands of 1.5 to 4.5 mm and the rib ratio of 40 to 60 percent are from a design for injection moulding guide. The flow-length-to-thickness ratio of roughly 100 to 200 for unfilled grades is a working planning figure rather than a specification and should be confirmed by flow simulation for the actual geometry. Thickness and tolerance figures are planning values, not a quotation.