Sink Marks in Injection Molding: Ribs, Bosses and the Packing That Cannot Reach

What a sink mark actually is

A sink mark is a shallow depression on the surface of a moulded part, and it is always the same story: a region of the part was still molten and shrinking after the surface skin had frozen solid, and it pulled the skin down with it. The skin is a thin solid shell; underneath it, the core is cooling and contracting; the shell cannot resist the tension, so it deflects inward and stays there.

The amount of contraction is not small. An unfilled polypropylene shrinks 1.5 to 2 percent linearly, which is 4 to 6 percent by volume. A polyamide shrinks more. A 4 mm thick section shrinking 5 percent by volume wants to lose 0.2 mm of thickness, and if the surface is already frozen, that 0.2 mm has to come from somewhere: it comes from the surface moving inward.

This is why sink marks are a thickness problem before they are a process problem. Uniform wall sections cool and shrink uniformly and the shrinkage is taken up by the part getting slightly smaller overall, which is what the mould shrinkage allowance is for. Where the wall is not uniform, the thick region shrinks more than the thin region around it, and the difference has to go somewhere visible.

Ribs, bosses and the half-wall rule

A rib is a thick section attached to a thin wall, and it is the most common source of sink marks in the industry. The rule that every designer is taught is that a rib should be no thicker than half the adjoining wall, and like most rules of thumb it is approximately right for a reason that can be quantified.

At a rib-to-wall ratio of 0.4 the sink is 2 microns, which is invisible. At 0.5 it is 6 microns, which is invisible on a textured surface and barely detectable on a polished one. At 0.6 it is 15 microns, which shows as a faint line on a gloss surface. At 0.8 it is 38 microns and at 1.0 it is 62 microns, and at that point the mark is obvious from a metre away.

Table 1 — Rib thickness against sink depth and the stiffness it buys.

The stiffness column is what makes the rule painful, because it shows what is being given up. A rib at half the wall gives roughly half the stiffness of a full-thickness rib, so following the rule costs real performance. The way out is not to thicken the rib but to add more of them: two ribs at 0.5 give more stiffness than one rib at 1.0, and neither of them sinks.

Why packing cannot reach a distant rib

The instinctive fix for a sink mark is more packing pressure, and it works when the sink is near the gate and fails when it is not. The reason is that packing only helps while the gate is open and the cavity is hydraulically connected. Once the gate freezes, the part is a sealed volume, and pressure applied at the sprue does nothing at all inside it.

Even before the gate freezes, pressure decays along the flow path. The melt is viscous, the channel is thin, and the pressure drop from gate to the far end of a 250 mm part is substantial. Measured sink depth against distance from the gate runs 8 microns at 50 mm, 14 at 100, 22 at 150, 32 at 200 and 45 at 250. The far end of the part is effectively unpacked even when the near end is fully packed.

There are three consequences. A sink near the gate is a packing problem and can be fixed with pressure and hold time. A sink far from the gate is a gate position problem and can only be fixed by moving the gate, adding a second gate, or thickening the feed path. And a sink that appears only on the far cavity of a multi-cavity tool is a runner balance problem, because the far cavity is seeing a lower pressure for the whole of the pack phase.

The three fixes that work

Every real fix falls into one of three families, and they are worth considering in this order because the cost rises sharply from one to the next.

Table 2 — The fixes, in the order they should be considered.

The texture option deserves a note because it is used more than it is admitted. A matte texture with a depth of 20 to 30 microns will hide a sink of 10 microns completely, and it is a legitimate engineering answer when the alternative is a tool change. What it is not is an answer for a 60 micron sink, which will still read as a glossy patch inside the matte field.

Bosses are worse than ribs

A boss is a cylindrical feature, usually around a screw hole, and it is worse than a rib for a simple geometric reason: the wall thickness at the base of a boss is the full diameter of the boss, not the wall of the tube. A boss 8 mm outside diameter with a 4 mm hole has a 2 mm wall, but where it meets a 2 mm plate the local section is 8 mm of material with a hole in it, and that is four times the plate thickness.

The standard mitigations are all geometric. Core the boss from the back if the design allows. Use a boss with a wall of 0.6 times the plate rather than a solid cylinder. Add gussets, which spread the section change over a longer distance and reduce the concentration. And keep the boss short, because a tall boss has more mass and shrinks more.

There is a process trick that works on bosses better than on ribs: core the boss out with a moving core or a secondary operation, so that the moulded feature is a tube rather than a cylinder. A tube of 2 mm wall on a 2 mm plate sinks almost not at all, and the hole is drilled afterwards. The cost is a secondary operation, and it is often cheaper than the sink mark.

Sink against void: the same cause, two symptoms

The same shrinkage that produces a visible sink mark can instead produce an internal void, and which one you get depends on how stiff the surface is relative to the pull of the shrinking core. A part with a strong, thick, cool skin pulls the surface in and shows a sink. A part with a hot, weak skin lets the core pull away from the skin and creates a void inside the thick section, with a perfectly good surface.

This matters because the two are confused constantly. A part that passes a visual inspection and fails a mechanical test may be full of voids. The way to tell is to cut the part through the suspect section: a sink shows as a depression on the surface with sound material behind it, and a void shows as a cavity inside with a surface that looks fine.

Table 3 — Four symptoms of the same shrinkage, and how to tell them apart.

Design rules that avoid it

Sink marks are almost entirely a design outcome. A part designed with uniform wall, ribs at half the wall and cored bosses will not sink even on a mediocre process. A part designed with a 4 mm rib on a 2 mm wall will sink on the best process in the building.

1. Keep the nominal wall as uniform as the function allows, and transition thickness gradually rather than in a step.
2. Ribs at 0.5 to 0.6 of the wall, and use more ribs rather than thicker ones to recover stiffness.
3. Bosses cored to a wall of 0.6 of the plate, with gussets, and kept as short as the screw length allows.
4. Put the gate where the thickest section is, so that packing reaches the mass before the gate freezes.
5. Avoid thick corners where two walls meet; a radius is better than a sharp corner, and a cored corner is better than either.
6. If the surface must be cosmetic, specify the texture before the tool is cut, not after the first samples sink.

The last point is the one that saves the most money. A texture specification written into the tool drawing costs nothing. A texture added to an existing tool costs a re-polish and a re-texture, and if the sink is deep it will not fix it anyway.