A sink mark is a shallow depression on the outside of a molded part, sitting directly opposite a rib, boss, or thick section on the inside. It appears because the thick region cools and shrinks after the surface has already frozen, pulling the skin inward. On a matte-textured back surface it is invisible. On a gloss front panel under retail lighting it is the first thing a customer notices, and the defect most likely to trigger a mold rework at $3,000 to $8,000 after T1 samples come back.

Sinks are a design problem that shows up as a process problem. Molders can reduce them with pressure and cooling time, but if the geometry is wrong they can only trade a sink for a longer cycle, a warped part, or voids. Almost every durable fix happens in CAD.

Why Thick Sections Sink

Thermoplastics shrink as they cool — roughly 0.4 to 0.7 percent for ABS and polycarbonate, 1.0 to 2.5 percent for semi-crystalline materials like polypropylene, acetal, and nylon. The skin against the cold mold wall solidifies within a second or two. The core of a thick section stays molten far longer, and when it contracts it takes that volume from somewhere. If the gate is still open, it pulls fresh material in. If the gate has frozen, it pulls the nearest surface inward instead.

Two consequences follow. Higher-shrink materials sink more. And anything locally thicker than its surroundings — a rib intersection, a boss, a screw column, a raised logo — is a sink candidate.

Rib-to-Wall Ratio: The Rule That Does Most of the Work

Rib thickness at the base should be 50 to 60 percent of the nominal wall it attaches to. For a 2.5 mm wall, that is a 1.25 to 1.5 mm rib base, and high-gloss work pushes it to 40 percent. Going to 75 percent, which looks structurally sensible, produces a visible sink on almost any cosmetic surface.

The rest of the rib rules follow from the same logic:

  • Height no more than 3 times the nominal wall. Taller ribs need draft that thins the tip toward nothing and are hard to fill.
  • Draft of 0.5 to 1.5 degrees per side, which tapers the rib and reduces mass away from the base.
  • Base radius of 0.25 to 0.5 times the wall. A sharp corner is a stress riser; a generous fillet adds mass and causes the sink you were avoiding.
  • Spacing of at least twice the nominal wall between ribs, so the steel between them can cool.
  • More ribs, not thicker ribs. Three thin ribs stiffen more than one thick one and sink less, as worked through in ribs and bosses in plastic parts.

All of this presumes a nominal wall that is uniform in the first place, which is the precondition for everything else and is covered in wall thickness for injection molded parts.

Bosses: The Worst Offender

A screw boss is a solid cylinder of plastic attached to a wall — a mass concentration by definition:

  • Outer diameter roughly 2 to 2.5 times the screw diameter; boss wall 50 to 60 percent of nominal, same as a rib.
  • Never attach a boss directly to a cosmetic wall. Stand it off and connect it with thin gussets, or attach it to a rib. This single change eliminates most boss sinks.
  • Core the boss from the base rather than leaving a solid pillar.
  • Add three or four gussets at 50 percent wall for bending strength instead of thickening the boss.

Where the boss carries a threaded insert, the insert changes both the wall requirement and the mass distribution; installation methods are described in threaded inserts in plastic.

Gate Location and Flow

Packing pressure reaches a thick section only while the path to it is still molten. Gate into the thickest area so material flows thick to thin — gate into a thin wall feeding a thick boss and the thin section freezes first, cutting off the pack and guaranteeing a sink.

Distance matters too. Pressure drops along the flow path, so a boss 180 mm from the gate receives far less packing than one 30 mm away. On a large panel a second gate near the problem region is often cheaper than redesigning the part, though it introduces a weld line you then have to place acceptably. Gate placement, parting line, and draft get decided together, as described in draft angles and parting lines.

Process Levers the Molder Actually Has

When geometry is close but not perfect, the molder can usually close the gap:

  1. Raise packing pressure and extend pack time until the gate freezes. The primary control; too much brings flash and ejection problems.
  2. Lower melt and mold temperature to reduce shrinkage, at the cost of fill pressure and possible short shots.
  3. Extend cooling time so the part is more rigid at ejection. Raises cycle time and piece price.
  4. Improve cooling in the thick region with a conformal or baffled water line, or a beryllium-copper insert to pull heat out locally.
  5. Switch to a lower-shrink or filled grade. A 20 percent glass-filled resin shrinks far less, though it changes stiffness, finish, and cost.

Every one of these is a trade. A molder who kills your sink by adding eight seconds of cooling has raised your per-part cost roughly 20 percent.

Hiding What You Cannot Eliminate

Sometimes the structure genuinely requires mass. Then make the sink invisible rather than absent. A textured surface scatters light and hides shallow depressions that a gloss finish would advertise; the texture families and their depths are compared in mold texture selection. Alternatives include breaking the surface with a shallow step or decorative grooves so the eye has no continuous reflection to read, or moving the feature behind a label or lens.

Catch It Before the Tool Is Cut

Run a mold-flow analysis on any part with a cosmetic A-surface. It predicts sink depth in microns and shows which rib intersections will show, for a fraction of a mold rework. Then check the first shots under raking light rather than overhead diffuse light, as part of the review described in what to check in the first mold trial. Sinks that fall in the same family as warpage, voids, and short shots are catalogued in injection molding defects.

Get the Geometry Right the First Time

Projects House designs molded parts against the rib, boss, and gating rules that keep tooling revisions out of your schedule, and reviews existing CAD before steel is cut. Send your part files and target finish through our contact form.