Sink Marks in Injection Molding: Causes, Prevention, and Fixes

Sink marks in injection molding are not a mystery. They are a predictable result of specific design, process, or material decisions. In our experience managing hundreds of offshore tool programs, fixing sink marks after tool steel is cut adds an average of $3,500 to $8,000 in rework costs and delays part approval by three to five weeks. Front-load the solution and you pay nothing extra.

What Causes Sink Marks in Injection Molding

A sink mark forms when the outer skin of a molded part solidifies before the core does. The core continues to shrink, pulling material inward. The result is a shallow depression on the visible surface, typically directly opposite a thick section, rib, or boss.

Sink mark causes fall into three categories: part design, process settings, and material selection. Most sinks you will see in production trace back to design first, process second, and material a distant third. Blaming the press operator before reviewing the wall section drawing is a waste of everyone’s time.

The most common design driver is a rib that is too thick relative to the nominal wall. SPI guidelines recommend rib thickness at 50 to 60 percent of the adjoining wall. A 3.0 mm nominal wall should carry ribs no wider than 1.5 to 1.8 mm at the base. Violate that ratio and you have created a local thick section that will sink on the show surface every time.

Bosses carry the same risk. A boss wall thickness exceeding 60 percent of the nominal wall will almost always produce a visible sink on the opposite face. Core out the boss. If structural loading prevents full coring, offset the boss from the show surface and hide it behind a rib.

Sink Marks and Ribs: The Design Math

Sink marks in ribs are the single most common cosmetic defect we see on first-shot samples from offshore suppliers. The geometry is straightforward, but the fix requires discipline during DFM review, not after T1.

Use this reference table to set rib dimensions before you cut steel.

Nominal Wall (mm)	Max Rib Base Width (mm)	Recommended Draft per Side (deg)	Max Rib Height (mm)
2.0	1.0 to 1.2	0.5 to 1.0	6.0
2.5	1.25 to 1.5	0.5 to 1.0	7.5
3.0	1.5 to 1.8	0.5 to 1.0	9.0
3.5	1.75 to 2.1	1.0	10.5
4.0	2.0 to 2.4	1.0 to 1.5	12.0

Rib height should not exceed three times the nominal wall. Beyond that, you trade a sink risk for a warp risk, and the ejector pin marks get worse too. Keep the geometry inside these numbers and you eliminate the most common structural driver of sink.

If your part design requires a thick rib for load-bearing reasons, consider a cross-rib lattice pattern. Two thinner intersecting ribs carry more load per unit of material than one thick rib, and neither produces a sink when sized correctly.

Process Causes: Pack Pressure and Hold Time

Even a well-designed part will sink if the process is wrong. The two most common process-driven sink mark causes are insufficient pack pressure and short hold time.

Pack pressure compensates for volumetric shrinkage as the part cools. Most semicrystalline resins, such as nylon 6/6 or polypropylene, shrink between 1.5 and 2.2 percent. Amorphous resins like ABS or PC shrink between 0.4 and 0.8 percent. You need enough pack pressure delivered through the gate before it freezes to replace that lost volume.

A gate that freezes too early cuts off pack pressure prematurely. This is why gate sizing matters. For a 3.0 mm wall section in ABS, a submarine gate of 0.8 mm diameter will freeze in roughly 1.5 to 2.0 seconds. If your hold time is set at 1.0 second, you are not finishing the job. Extend hold time in 0.5-second increments while watching the part weight on a calibrated scale. When part weight stops increasing, your gate has frozen and additional hold time buys you nothing.

Pack pressure itself should typically run at 50 to 80 percent of peak injection pressure. If your injection pressure is 18,000 psi, your pack pressure floor is 9,000 psi. Running pack at 4,000 psi on a thick-walled part and wondering why you have sinks is a process setup problem, not a tool problem.

Melt temperature also contributes. An overly hot melt increases the thermal gradient between skin and core, giving the core more time to shrink before it solidifies. Run the resin at the low end of the manufacturer’s recommended melt temperature range when sinks are present, provided you are not creating short shots or weld line failures elsewhere in the part.

Material Causes and Resin Selection

Material is the third lever. High-shrinkage resins produce deeper sinks for the same geometry. Glass or mineral fill reduces shrinkage and reduces sink severity. According to CAMPUS material database data, unfilled polypropylene shrinks at 1.5 to 2.0 percent. A 20 percent glass-filled PP shrinks at 0.4 to 0.8 percent. That difference alone can move a marginal sink below the visible threshold without changing the tool or the process.

If your program allows a material change, adding 10 to 30 percent mineral fill is often the lowest-cost fix for chronic sinking in thick sections. Talc-filled PP is a common choice for structural interior parts where surface gloss is not critical. The trade-off is reduced impact strength and a slight increase in specific gravity.

Foamed or microcellular injection molding (MuCell) eliminates sinks on thick sections by creating internal pressure from the foaming agent. This is not a general-purpose fix. It requires specialized press equipment and produces a surface texture that is not acceptable for Class A finishes. For structural non-cosmetic components, it is a genuine option.

How to Fix Sink Marks: Process and Tool Corrections

When you receive a T1 sample with sinks, work through this sequence before requesting any steel work. Most sinks on a properly designed part resolve at the press.

• Increase pack pressure in 500 psi increments up to 80 percent of peak injection pressure.
• Increase hold time in 0.5-second increments until part weight plateaus.
• Lower melt temperature by 10 degrees F and re-shoot.
• Increase cooling time by 3 to 5 seconds to allow the skin to solidify before ejection.
• Verify gate size. A gate smaller than 50 percent of wall thickness will freeze before pack completes.

If process adjustments do not eliminate the sink, the fix moves to the tool. The most common tool corrections are gate enlargement, cooling line relocation, and wall section reduction through steel addition (not removal). You can always add steel; removing it means welding, which costs time and weakens the tool at the weld location.

When sink marks on ribs persist after process optimization, the root cause is almost always a rib base that is too thick. The tool fix is to add steel to the rib forming insert, narrowing the rib. This is a straightforward EDM or milling operation on a P20 or H13 insert, typically running $400 to $900 at an offshore shop. Do not attempt this correction on hardened S7 or 420SS inserts without confirming the heat treatment protocol with your toolmaker. You risk cracking the insert.

Texture can mask minor sinks on non-cosmetic surfaces. A VDI 30 or EDM texture at Ra 3.2 micrometers breaks up the reflection that makes shallow sinks visible. This is a cosmetic mask, not a structural fix. Do not rely on texture to hide a sink that will grow deeper over 100,000 shots as the tool wears.

In our shops, we flag any rib-to-wall ratio above 0.65 in the DFM report before the customer approves tool design. That single checkpoint has eliminated first-shot sink issues on more than 80 percent of the programs where we applied it systematically.

Prevent Sink Marks in Plastic Parts: A Pre-Tool Checklist

The lowest-cost way to prevent sink marks in plastic parts is to build a DFM gate before steel release. These are the non-negotiable checks our project managers run on every cavity layout.

• Rib base width is 50 to 60 percent of adjoining nominal wall. No exceptions without a written process deviation.
• Boss outer wall is 60 percent or less of nominal wall. Boss is cored where possible.
• No abrupt wall transitions. Taper between wall sections at a 3-to-1 length-to-thickness ratio.
• Gate is sized at 50 to 80 percent of wall thickness at the gate land.
• Cooling lines are within 2.0 to 2.5 diameters of the cavity surface at all thick sections.
• Mold flow simulation run at final gate location before tool design is frozen.

Mold flow simulation catches approximately 70 percent of sink risk locations before T1, according to internal benchmark data from Autodesk Moldflow validation studies. It does not replace good design practice. It catches what slips through.

Frequently Asked Questions

What is the main cause of sink marks in injection molding?

The most common cause is a local thick section in the part, typically at a rib base or boss wall, where the core continues to shrink after the outer skin has solidified. Insufficient pack pressure and short hold time are the second most frequent drivers. Solve the design geometry first, then tune the process.

Can sink marks be fixed without modifying the tool?

Yes, if the part design is within accepted rib-to-wall ratios. Increasing pack pressure, extending hold time, reducing melt temperature, and adding cooling time resolve the majority of process-driven sinks without touching steel. If the rib base is oversized by design, the tool will need steel added to correct the section thickness.

How do sink marks on ribs differ from other sinks?

Sink marks on ribs appear on the visible face directly opposite the rib. They are caused by the rib base creating a localized thick section. The fix is to reduce the rib base width to 50 to 60 percent of the nominal wall, which requires adding steel to the rib-forming surface of the tool.

Does resin choice affect sink mark severity?

Yes. High-shrinkage resins like unfilled polypropylene at 1.5 to 2.0 percent volumetric shrinkage produce deeper sinks than low-shrinkage resins. Adding 20 to 30 percent glass or mineral fill can cut shrinkage by half or more, which often reduces sinks below the visible threshold on marginal geometry.

When should I use mold flow analysis to prevent sinks?

Run mold flow analysis before the tool design is released for machining, specifically at the final gate location with the final nominal wall sections. Running it earlier on preliminary geometry produces results that do not match the built tool. According to Autodesk Moldflow documentation, sink index outputs are most accurate when wall thickness variation is within 10 percent of the production intent model.

If you want a structured review of your part geometry before tool release, use our injection molding consulting service to run a DFM audit. If you need a fast check on clamp requirements for your wall sections and shot size, our clamp force calculator is available at no cost.