Skip to content
Design, materials & finishes

Injection moulding design guide: walls, ribs, draft, bosses and undercuts

An injection mould is a precision machine built around one part. Once it is cut, changes are slow and expensive, so the decisions that matter are made in CAD. Designing for moulding is about letting molten plastic fill the cavity evenly, cool evenly and leave the mould cleanly, shot after shot.

Rapid injection moulded ABS clips

Design starts with how plastic flows and cools

Plastic pelletsHeated barrel and screwmelt and push the plasticTwo-part steel mouldopens to eject the partMoulded part
An injection moulding machine melts plastic in a heated barrel and injects it into a closed mould under high pressure.

Molten plastic enters the mould through a gate, flows through the cavity, packs under pressure, cools against the steel and is ejected. Almost every moulding rule follows from that sequence: sections must fill before the plastic freezes; thick areas cool slowly and shrink more; and the part must slide off the mould cores without sticking or tearing.

1. Keep walls uniform

Uniform wall thickness is the most important moulding rule. Thick areas cool last and shrink more, which causes sink marks on the surface, internal voids and warping. Thin areas next to thick ones freeze first and can block flow. Many thermoplastics are moulded with walls of about 1 to 4 mm; the right value depends on the material, part size and flow length. Where thickness must change, make the transition gradual, over a length of about three times the change.

Uniform wallseventhick spot: sinkRibs0.5–0.6 × wall= wall: sinkDraftdraftedno draftGreen: easier to mould · Orange: likely to cause defects
Three core rules: uniform walls, ribs thinner than the wall, and draft on faces parallel to the mould opening.

2. Use ribs instead of thick walls

Ribs add stiffness without adding thick sections. Common guidance is a rib thickness of about 50 to 60 percent of the wall it joins (less for materials prone to sink), a height of up to about three times the wall thickness, a small root radius and draft on both faces. Space parallel ribs at least two wall thicknesses apart so the steel between them can be cooled.

3. Add draft

Draft is a slight taper on faces parallel to the direction the mould opens. Without it, the part drags on the mould, leaving scuffs, or sticks on the core. About 1 to 2° is common on most faces, with 0.5° as a practical minimum on smooth faces. Textured faces need more, commonly about 1 to 1.5° for each 0.025 mm of texture depth, because the texture forms tiny undercuts.

4. Round the corners

Sharp corners concentrate stress and disrupt flow. A common rule is an inside radius of about half the wall thickness and an outside radius of about one and a half times the wall thickness, which keeps the wall thickness constant around the corner.

5. Design bosses carefully

Bosses for screws and inserts are a common source of sink marks. Core them out so their wall matches the part wall, connect them to nearby walls with ribs rather than standing them alone, and follow the screw or insert manufacturer’s hole sizes for self-tapping screws and heat-set inserts.

6. Avoid undercuts, or plan for them

An undercut is any feature that stops the part being pulled straight out of the mould: a side hole, a snap hook, an internal groove. Each one needs a side action, lifter or collapsible core in the tool, which adds cost and maintenance. Alternatives include through-holes that let a shut-off form a hook from both sides, moving the feature to the mould opening direction, or a flexible snap that the part can spring over during ejection.

7. Think about gates, weld lines and ejection

Where plastic flows around a hole and meets itself, it forms a weld line, which is weaker and sometimes visible. The gate position decides where weld lines fall, so discuss gate positions with your toolmaker, especially for cosmetic faces and load-bearing features. Ejector pins leave small marks; indicate faces where marks are not acceptable.

8. Allow for shrinkage and set realistic tolerances

Every thermoplastic shrinks as it cools, from a few tenths of a percent for amorphous plastics such as ABS and PC to well over one percent for semi-crystalline plastics such as PP, nylon and acetal. Shrinkage also varies with flow direction and wall thickness. The toolmaker allows for it in the steel, but moulded tolerances are generally wider than machined ones. Tighten only the dimensions that matter, and expect to fine-tune the tool after the first samples.

General rules of thumb; follow the material supplier’s data for your grade.
FeatureCommon guidanceWhy
Wall thicknessUniform; transitions gradualAvoids sink, voids and warpage
RibsAbout 50–60% of the wall; height up to about 3× wallStiffness without sink
DraftAbout 1–2°; more for texturesClean ejection, no scuffing
Inside corner radiusAbout 0.5× wallLower stress, better flow
Outside corner radiusAbout 1.5× wallConstant wall around the corner
BossesCored, wall matched, tied to ribsAvoids sink and weak bosses
UndercutsAvoid or plan for side actionsLower tool cost and risk
Rapid injection moulded ABS clips
Rapid moulded ABS clips: a lower-cost tool for a few thousand parts.

Prototype before you cut steel

The cheapest way to find a design problem is before the tool exists. Common routes are:

  • CNC machined prototypes in the production plastic, for strength, fit and function testing. Machined parts are not moulded, so they will not show sink or weld lines, but they behave like the real material.
  • Vacuum cast parts for looks-like samples and small batches that imitate moulded parts, including colours and textures.
  • 3D printed parts for early form and fit checks.
  • Rapid moulding with aluminium moulds or inserts for a few thousand real moulded parts before committing to production tooling.

Our injection moulding service covers both rapid moulding and production tooling, and our guide to the moulding process explains the cycle.

FAQ

Common questions

Still unsure? Contact us or call +61 3 9764 2749.

What wall thickness should an injection moulded part have?

Many thermoplastics are moulded with walls of about 1 to 4 mm, but the right value depends on the material, size and flow length. Keeping the wall uniform matters more than the exact figure.

How much draft does an injection moulded part need?

About 1 to 2 degrees on most faces is common, with 0.5 degrees as a practical minimum on smooth faces. Textured faces need more draft.

What causes sink marks?

Thick sections cool and shrink after the surface has set, pulling it inwards. Uniform walls, thinner ribs and cored bosses prevent most sink marks.

Should I prototype before making a mould?

Yes. Machined, cast or printed prototypes find design problems before the tool is cut, when changes are cheap.

Ready to make your part?

Upload your CAD files for a free, obligation-free quote.