Sink Marks in Injection Molding: Causes, Prevention, and DFM Rules for Engineers

Sink marks are shallow surface depressions caused by localized shrinkage during cooling. They appear as visible dimples on the cosmetic side of a molded part—often directly opposite ribs, bosses, thick wall sections, or abrupt thickness transitions on the hidden B-side. For mechanical and product engineers preparing a CAD release or reviewing first-shot samples, sink marks sit at the intersection of design geometry, mold engineering, and process control.

This guide explains why sinks form, which DFM rules prevent them with the highest return on investment, and how to decide whether to redesign, modify tooling, or tune process parameters. The focus is practical prevention before steel is cut—not cosmetic rework after production starts.

What Are Sink Marks in Injection Molding?

How they appear on molded parts

On injection molded parts, sink marks typically show up as shallow concave patches on Class A surfaces. Under angled or raking light, they disrupt specular reflection and read as quality defects even when depth is measured in fractions of a millimeter. The pattern is rarely random: sinks almost always align with heavy cross-sections on the opposite face—ribs stiffening a flat panel, bosses receiving fasteners, lens housings with thick mounting pads, or step transitions between nominal wall and structural features.

Sinks differ from scratches or polish defects because they follow the part's internal geometry. A rib that is 80% of nominal wall thickness on the inside will often produce a visible dimple on the outside, even when the outer skin appears dimensionally correct in CAD. That is why engineers search for sink mark guidance during DFM review rather than after cosmetic inspection fails.

When sinks matter vs when they may be acceptable

Whether a sink mark is a reject depends on surface class and product context. Consumer electronics housings, medical device enclosures, and branded packaging typically require sink-free A-surfaces. Internal structural ribs, hidden mounting zones, and utility covers may tolerate shallow sinks if they do not affect assembly, sealing, or customer perception.

Sink marks are related to—but distinct from—other shrinkage-driven defects. Warpage bends the whole part when cooling stresses are unbalanced across the geometry. Voids are internal air pockets or unfilled regions inside thick sections. Sinks are surface manifestations of the same underlying shrinkage mechanism, but they are judged on appearance rather than structural integrity alone. A part can meet dimensional tolerances and still fail cosmetic acceptance because of sinks opposite hidden ribs.

Why Sink Marks Happen: Shrinkage and Differential Cooling

The cooling sequence at thick sections

Injection molding is a differential cooling process. Molten polymer fills the cavity, and the outer skin against the mold wall begins to solidify first. In thin, uniform sections, heat extracts quickly and shrinkage distributes evenly. In thick sections, the core stays molten longer while the frozen skin constrains it. As the core continues to contract, it pulls material inward from the opposite surface, creating a localized depression visible as a sink mark.

The mechanism is thermal mass driven: more polymer volume means longer cooling time, greater total shrinkage, and higher risk of opposite-surface pull. This is why a seemingly small rib on the B-side can produce a surprisingly visible defect on a 2 mm cosmetic wall.

Common geometric triggers

Three geometry patterns account for most sink mark cases in production troubleshooting:

1. Rib and boss intersections — Where two structural features meet, local wall thickness can exceed nominal wall by 150–200% or more, creating a hot spot that cools last.
2. Non-uniform wall thickness — Abrupt transitions—such as jumping from 1.5 mm to 4 mm without coring—concentrate shrinkage at the transition zone.
3. Solid bosses without coring — A full-diameter boss for a self-tapping screw can double local thickness unless cored from the back side.

Material shrinkage rate amplifies the effect. Semi-crystalline resins such as PP and PA tend to shrink more than amorphous grades such as ABS or PC, which increases sink severity for the same geometry. Glass-filled grades often reduce sink visibility because fillers resist surface pull, though they introduce other design constraints.

Design-Phase Prevention (Highest ROI)

Design changes made before tooling release cost far less than cavity rework, texture masking, or sustained process tuning on a geometry-limited part. The following rules are the highest-ROI levers for sink mark prevention.

Uniform wall thickness and coring

Target a consistent nominal wall thickness across cosmetic regions. When structural depth is required, core out thick sections from the non-cosmetic side rather than adding solid mass behind an A-surface. A cored pocket removes thermal mass while preserving stiffness through perimeter walls and ribs.

Avoid abrupt thickness steps greater than roughly 3:1 between adjacent sections. When a step is unavoidable, use gradual transitions, coring, or relocate the thick section away from cosmetic faces. For engineers working through plastic injection molding DFM, wall uniformity checks should run before rib and boss sizing—not after.

Rib design rules to prevent sink marks

Ribs add stiffness without doubling nominal wall, but only when sized correctly. Use the following DFM thresholds as a starting point; cosmetic A-surfaces should target the conservative end of each range.

Keep rib spacing adequate so adjacent ribs do not create overlapping thick zones. Orient ribs to allow melt flow along the rib direction where possible, reducing weld-line formation at rib bases. On cosmetic housings, consider reducing rib height or splitting one tall rib into two lower ribs rather than pushing height limits.

Boss design and boss-rib tie-ins

Bosses for screws, pins, or alignment features follow the same thickness logic as ribs. Boss wall thickness should be 40–60% of nominal wall. Core bosses from the B-side when depth exceeds one nominal wall thickness. Add base fillets to reduce stress concentration and improve melt flow around the boss root.

Boss-rib tie-ins—connecting a boss to a nearby wall with a thin rib—can reduce sink risk compared to a standalone thick boss pad, because the rib ties the boss into the wall without a solid disc of material behind the A-surface. The tradeoff is mechanical: thinning the boss base improves cosmetics but reduces pull-out strength and torsional resistance. Document load requirements alongside cosmetic class so DFM reviewers can recommend cored bosses, metal inserts, or relocated bosses rather than arbitrary thickening.

Radii, draft, and cosmetic surface planning

Internal corner radii affect both flow and cooling. Sharp internal corners restrict flow and create localized thick zones at the outside corner. Minimum internal radii should follow resin-specific guidance, but as a sink-prevention principle, avoid placing cosmetic A-surfaces directly opposite un-cored internal corners or heavy fillet intersections.

Plan cosmetic surfaces away from known thick features. If the industrial design requires a flawless show face opposite a structural rib network, either thin the ribs to the pass range, add coring, or accept that process tuning alone will not deliver consistent results. Draft angles of 0.5–1° on ribs and bosses support ejection and reduce polishing variation that can make shallow sinks more visible.

Mold Design Factors Engineers Should Specify

While part design drives most sink risk, mold engineering determines how effectively the cavity compensates for shrinkage during packing and cooling. Engineers issuing RFQs should specify expectations—not just part geometry—so mold builders can plan gate, vent, and cooling strategy before cutting steel.

Gate location and flow path

Gate placement controls whether melt reaches thick sections under pressure before freeze-off. Ideally, flow paths direct material into heavy regions early in fill so pack pressure can feed them during hold. Gates placed far from thick bosses or rib networks may allow those regions to freeze before adequate packing, worsening sinks regardless of nominal wall compliance.

Discuss gate type and location during DFM dialogue. Tab, edge, or submarine gates each affect pack behavior differently depending on part geometry and material.

Venting and cavity fill

Inadequate venting traps air in rib tips, boss cores, and deep pockets. Trapped air prevents full cavity pack-out, which mimics underpack shrinkage and can intensify sink marks. Specify venting expectations for deep features and confirm vent depth and location during mold design review.

Cooling layout around thick features

Cooling channels should extract heat evenly around thick sections. Isolated hot spots—regions far from cooling lines or without adequate baffle or bubbler coverage—extend cooling time and increase differential shrinkage. Conformal cooling can help in challenging thick-boss geometries, but part-side coring often delivers more predictable results at lower tooling complexity.

Process Parameters That Influence Sink Marks

When geometry is borderline, process tuning can reduce sink severity. When geometry is in the fail range of the DFM table above, processing cannot reliably eliminate sinks across a production window.

Pack and hold pressure/time

Pack and hold compensate for volumetric shrinkage as the part cools. Increasing hold pressure and hold time feeds material into thick regions until the gate freezes. This is most effective when the thick section is connected to the gate through a flow path that remains open during hold. Once the gate freezes, no further packing reaches the cavity.

Melt temperature, mold temperature, and cooling time

Higher melt temperatures increase shrinkage magnitude. Excessive mold temperature prolongs cooling and can worsen sinks on thick sections. Conversely, too-low mold temperatures can cause premature freeze-off before pack completes. Cooling time must allow thick sections to solidify enough for ejection without continuing to shrink on the show surface after demolding.

Early ejection—pulling the part while the core is still contracting—often deepens sink marks and invites warpage. Validate cooling time against the thickest feature, not just nominal wall.

When processing can help—and when it cannot

Processing is worth trying when ribs and bosses are in the warn range, gate location is defensible, and sinks are shallow and inconsistent—signals of pack or cooling imbalance. Escalate to design when sinks are deep, repeatable, and mapped directly to features exceeding fail thresholds, or when hold pressure increases cause flash without improving cosmetics.

Troubleshooting Workflow for Engineers

Use this sequence when reviewing first shots or evaluating a CAD revision flagged for sink risk.

Step 1: Confirm location and geometry

Photograph sinks under raking light and map each depression to the opposite-side feature in CAD. Mark rib bases, boss locations, wall transitions, and uncored thick pads. If the sink pattern does not correlate to geometry, investigate venting, fill imbalance, or material degradation before redesigning.

Step 2: Run DFM checks

Screen for wall uniformity, rib and boss ratios against the pass/warn/fail table, coring opportunities on bosses and thick pads, and transition ratios between sections. Document cosmetic surface class so reviewers know which thresholds apply.

Step 3: Evaluate mold/process levers

If geometry is borderline, review gate location relative to thick features, venting at rib tips and bosses, cooling access to hot spots, and current pack/hold pressure and time. Change one variable at a time and correlate with sink depth on the mapped features.

Step 4: Redesign vs accept

If geometry exceeds fail thresholds and cosmetics matter, redesign is the durable fix: thin ribs, core bosses, relocate thick features, or add coring. If the surface is non-cosmetic and sinks are shallow, acceptance may be justified—document the deviation against cosmetic class. Weigh tool modification cost and production volume: high-volume programs justify redesign; low-volume programs may accept sinks on hidden faces if mechanical requirements are met.

Get DFM Feedback Before Tooling Release

Sink marks are predictable when thick geometry sits behind cosmetic surfaces—and expensive when discovered after mold completion. Uploading CAD early for manufacturability review catches rib, boss, and wall-thickness risks while changes remain low-cost model updates rather than cavity welding.

NetProto's quoting flow pairs instant pricing feedback with DFM dialogue so engineers can resolve sink-prone geometry before tooling release. Upload your CAD for instant DFM feedback and pricing, and use the troubleshooting workflow above to prioritize design fixes over endless process tuning.