If you fix only one thing on a molded part design, fix wall thickness. More molding problems trace back to it than to any other design decision, and unlike most manufacturing constraints it costs nothing to get right.
The reason is straightforward. Plastic shrinks as it cools, and thicker sections cool more slowly and shrink more. Any variation in thickness therefore produces variation in shrinkage, which produces internal stress, which shows up as sink marks, warpage, voids and dimensional instability.
Uniform walls avoid all of that at once. This guide covers what uniform means in practice, how to handle the features that inevitably break uniformity, and what ranges apply to common materials.
The Core Principle
Aim for uniform wall thickness throughout the part.
Not approximately uniform in the places you thought about, but uniform everywhere, including at corners, around bosses, at rib intersections and where features meet the wall.
Where variation is unavoidable, transition gradually rather than abruptly, and keep the variation as small as the design allows.
This single principle prevents the majority of common molding defects. The rest of this guide is essentially about how to maintain it in the presence of features that want to break it.
Typical Ranges by Material
Wall thickness ranges vary by material because flow characteristics and shrinkage differ. Broad guidance:
| Материал | Typical wall thickness range |
| Полипропилен (PP) | 0.9 to 3.8 mm |
| Полиэтилен (ПЭ) | 0.8 to 3.0 mm |
| ABS | 1.1 to 3.5 mm |
| Поликарбонат (PC) | 1.0 to 3.8 mm |
| Nylon (PA) | 0.8 to 3.0 mm |
| POM (acetal) | 0.8 to 3.0 mm |
| PC-ABS | 1.1 to 3.5 mm |
| Thermoplastic elastomers | 0.6 to 3.0 mm |
Treat these as orientation rather than specification. Actual limits depend on flow length, gate location, geometry and the specific grade. A long thin flow path may not fill at a thickness that would be perfectly adequate over a short distance.
Two general observations hold across materials. Thinner walls cool faster, which shortens cycle time and reduces sink and warpage risk. Thicker walls fill more easily over long distances but bring shrinkage problems and longer cycles.
The practical implication is to design at the thinner end of the acceptable range where the part’s structural requirements allow, and to use ribs rather than thickness to achieve stiffness.
Ребрышки
Ribs stiffen a part without adding wall thickness. They are the primary tool for keeping walls thin while meeting structural requirements, and they are also a common source of sink marks when proportioned wrongly.
Thickness. A rib should be roughly 50 to 60 percent of the wall it joins. Thicker than that and the rib base becomes a thick section, which sinks on the opposite surface.
For materials that show sink readily, or on visible surfaces, err toward the lower end. For structural ribs on hidden surfaces, the upper end is acceptable.
Height. Generally up to about three times the wall thickness. Taller ribs are possible but become difficult to fill and eject, and offer diminishing structural return.
Draft. Ribs need draft on both faces, which means a tall rib tapers noticeably. Combined with the base thickness limit, this constrains how tall a rib can practically be.
Base radius. A small radius where the rib meets the wall reduces stress concentration and improves filling, typically around 25 percent of the wall thickness. Too large a radius creates a thick section, defeating the purpose.
Spacing. Ribs should be spaced at least twice the wall thickness apart. Closer spacing creates thin steel between them in the tool, which is fragile and cools poorly.
Multiple ribs beat one thick rib. Several appropriately sized ribs provide more stiffness than one oversized rib, without the sink.
Боссы
Bosses receive screws, locate components or provide mounting points. They are inherently a thick feature attached to a thin wall, which makes them the second most common source of sink marks.
Do not attach a solid boss directly to a wall. The junction becomes a thick section and sinks visibly on the opposite face.
Standard approach: stand the boss slightly off the wall and connect it with ribs or gussets. This provides support without creating a mass of material at the junction.
Wall thickness of the boss should follow the same 50 to 60 percent guideline relative to the nominal wall.
Coring. Bosses should be cored rather than solid, both to avoid a thick section and because the core creates the hole the screw needs.
Проект applies to both the inside and outside of the boss.
Base radius at the boss junction reduces stress concentration, which matters because bosses carry load.
Where a boss must carry significant load, consider a molded-in threaded insert rather than a self-tapping screw into plastic, which is covered in our guide to формовка вкладышей.
Corners and Transitions
Sharp internal corners are a problem for three separate reasons. They concentrate stress, which is where parts crack. They restrict flow. And the corner itself is effectively a thicker section, since a sharp corner has more material than a radiused one at the same nominal wall.
Apply a radius at internal corners, typically around 0.5 times the wall thickness at minimum, with the outer radius equal to the inner radius plus the wall thickness. This maintains uniform thickness through the corner, which is the point.
Transitions between thicknesses should be gradual. Where a wall must change thickness, taper over a distance of at least three times the thickness difference rather than stepping abruptly.
A step change produces a shrinkage discontinuity, which is a stress concentration and a warpage source.
Coring Out Thick Sections
Where a design genuinely requires bulk, core it rather than leaving it solid.
A solid block of plastic cools from the outside in, shrinks internally, and produces either a deep sink on the surface or a void inside. Neither is acceptable in most applications.
Coring converts a thick section into walls of appropriate thickness. It also reduces material cost and cycle time, since less material must cool.
This applies to handles, bases, thick structural features and anywhere a designer has drawn a solid volume without considering how it will cool.
Flow Length and Filling
Wall thickness interacts with how far the material must flow.
A thin wall over a short distance fills easily. The same thickness over a long flow path may not, because the melt cools and viscosity rises as it travels.
Where a part has long flow paths, either the wall must be thicker, the gate must be repositioned, or multiple gates must be used. This is a discussion to have with your molder rather than a calculation to guess, since it depends on material, temperature and geometry together.
Where a part has both thick and thin regions, the melt preferentially fills the thick regions, potentially leaving thin regions short. Uniform thickness avoids this, which is another reason it matters.
Filled Materials
Glass-filled and mineral-filled grades change the picture.
Shrinkage becomes directional. Fibres orient along the flow direction, and shrinkage differs along and across that orientation. This makes warpage harder to predict and more sensitive to gate location.
Stiffness is higher, so thinner walls may be structurally adequate.
Flow is generally poorer, which can require slightly thicker walls than the unfilled equivalent despite the stiffness advantage.
For filled materials, flow simulation is more valuable than for unfilled, because the directional effects are difficult to reason about intuitively.
Checking a Design
Before releasing a molded part:
- Check nominal wall thickness is within the range for your material
- Look for any section noticeably thicker or thinner than nominal
- Check rib thickness against the wall they join
- Check boss junctions for thick sections
- Radius all internal corners
- Taper any necessary thickness transitions
- Core out any solid volume
- Check rib spacing
- Check the longest flow path against the wall thickness
- Confirm draft has been applied, since drafted walls vary in thickness over their height
Most designs fail at least three of these on first review. Catching them in CAD costs an afternoon. Catching them at T1 costs a tool modification.
Why This Matters More Than It Seems
Look at the causes of the most common molding defects. Sink marks come from thick sections. Warpage comes from differential shrinkage, usually driven by uneven thickness or uneven cooling. Voids come from thick sections. Short shots often come from thin regions competing with thick ones for flow.
Four of the most common defects share one root cause. Getting wall thickness right eliminates most of them before a tool exists, which is why it repays attention out of proportion to the effort involved. Our guide to injection molding defects covers what each one looks like when it appears.
Getting a Design Reviewed
Wall thickness problems are cheap to fix in CAD and expensive to fix in steel, and they are easy to miss in a model that looks reasonable.
Elite Mold Tech provides DFM review before quoting on производство пластмассовых деталей, covering wall thickness, ribs, bosses, draft and gating together, since these interact rather than being independent. Sending a part file with the intended material produces specific comments on where thickness varies and what to do about it.
Часто задаваемые вопросы
Q: What is the ideal wall thickness for an injection molded part?
A: It depends on material, with common engineering plastics typically falling between roughly 0.8 and 3.8 mm. More important than the absolute figure is uniformity, since variation causes most common defects.
Q: How thick should ribs be on a molded part?
A: Around 50 to 60 percent of the wall they join. Thicker ribs create a thick section at the base, which produces sink marks on the opposite surface.
Q: Why do bosses cause sink marks?
A: A solid boss attached directly to a wall creates a thick section at the junction that shrinks more than the surrounding material. Standing the boss off the wall and supporting it with ribs avoids this.
Q: Can I make a plastic part stronger by increasing wall thickness?
A: Usually the wrong approach. Thicker walls bring sink, warpage, voids and longer cycles. Ribs provide stiffness far more efficiently while keeping wall thickness uniform.
Q: What happens if wall thickness varies across a part? A: Thicker areas cool and shrink more slowly, creating internal stress that produces sink marks, warpage and voids. Thicker regions also fill preferentially, which can leave
