Thick-Section Design: Coring Out, Ribbing, and When You Actually Need Gas Assist

Thick plastic is rarely just a material-cost issue. It creates a thermal bottleneck that can govern the entire molding cycle and produce sink marks, internal voids, warpage, long gate-seal time, and inconsistent dimensions. Increasing packing pressure may move the symptom, but it does not remove the volume that must cool and shrink.

The right question in thick section plastic part design is therefore not “Can this thickness be molded?” It is “What is the least complex way to carry the load without leaving a concentrated hot mass?” The answer usually follows a ladder: recover stiffness with geometry, core out the mass, improve local cooling if the mass must remain, and use gas assist only when a designed hollow path creates enough value to justify a specialized process.

 

Why Thick Sections Produce Both Sink Marks and Voids

The surface of a molding freezes before its center. As the hot core cools and contracts, one of two related outcomes may occur:

• If the frozen skin can still move, the surface pulls inward and forms a sink mark.
• If the skin remains comparatively rigid while the center cannot be adequately fed through the gate, a shrinkage void may form inside the thick region.

BASF’s engineering-thermoplastics troubleshooting guide places voids in the molten center and associates them with thick sections; it also connects rib bases and local material accumulation to sink-mark risk.[1] A peer-reviewed study of thick polycarbonate lenses similarly found large temperature differences between thick central and thin edge regions and warned that common simulation outputs may not characterize large-volume sink behavior in the same way they detect sink under a rib.[2]

Thickness also has a nonlinear effect on cooling. A simplified one-dimensional heat-conduction model contains the square of part thickness, along with polymer thermal diffusivity and the melt, mold, and ejection temperatures.[3] This is a useful first-order explanation—not a universal cycle-time calculator. Actual cooling also depends on geometry, crystallization behavior, tool steel, coolant layout and flow, contact at the cavity surface, and the chosen safe-ejection criterion. Autodesk’s Moldflow documentation, for example, lists local thickness, material transition temperatures, distance from the injection location, ejection temperature, and surrounding tool-steel temperature among the inputs to its time-to-ejection result.[4]

The practical conclusion is robust: a single thick island can set the cycle for the whole part, and a process-only correction cannot make its thermal mass disappear.

 

Level 1: Use Ribs and Gussets Instead of Solid Thickness

Stiffness is strongly affected by section geometry. A deeper section, supported by ribs, gussets, flanges, or a closed profile, can resist bending more efficiently than a flat solid wall made thicker everywhere.

This first level belongs in CAD because it is usually the lowest-cost intervention:

1. Establish the load path and the direction in which bending or twisting must be resisted.
2. Keep the nominal wall as uniform as the material and flow length allow.
3. Place ribs along the load path rather than forming a decorative grid.
4. Taper and radius ribs for ejection and stress control.
5. Keep the rib base thin enough to avoid recreating a thick junction on the opposite cosmetic surface.
6. Connect bosses to walls with ribs or gussets while coring the boss center.

There is no single rib ratio for every resin, texture, surface class, and gate arrangement. BASF gives a rib thickness of about half the basic wall as an advantageous starting point in its troubleshooting guidance, but that value belongs to the material and geometry context of the guide.[1] A design team should use the exact resin supplier’s recommendations, then verify sink, filling, weld lines, ejection, and structural performance in analysis and trials.

Ribs are especially effective when the requirement is bending stiffness or local support. They are less able to replace solid bearing material around an insert, a sealing land, an impact point, or a handgrip whose external form must remain bulky.

 

Level 2: Core Out the Section, Then Restore the Load Path

Coring converts a solid mass into a shell around a mold core. In many parts, this is the decisive change: it makes the thermal path more uniform, reduces material, and leaves stiffness to ribs and section depth rather than to a block of resin.

A good coring study asks more than whether a void can be drawn in CAD:

• Can the core be manufactured and cooled? A deep or slender core can become the new hot spot and may deflect under asymmetric cavity pressure.
• What core and rib depth is actually manufacturable? Put maximum unsupported depth, minimum steel section, machining/EDM access, cooling route, stiffness, and inspection method into the tool review; do not rely on an unverified universal height-to-width ratio.
• Can the part eject? Internal walls need draft, and texture or a deep draw may increase the requirement.
• Where is the parting line? Coring can create shutoffs, slides, lifters, or inserts that add tool cost and maintenance.
• How will the melt fill around the core? Flow may split and recombine, creating weld lines whose location must be checked against load paths and appearance requirements.
• Can pressure reach the thickest remaining junction before gate seal? A cored feature can still sink if ribs, bosses, and fillets create a concentrated base.
• Can the core be supported? Long cores and insert features need a filling pattern that avoids excessive unbalanced pressure.

The useful default is conditional: if conventional coring preserves function and produces a manufacturable, adequately cooled and supported core, it should be evaluated before a specialized molding process. “Core first” is not an absolute command; it is a cost-and-risk gate.

Level 3: Use Local Cooling When Geometry Cannot Remove the Heat

Sometimes the thick section is functional: a bearing region, optical geometry, a grip, an energy-absorbing feature, or a sealed volume may not be freely hollowed. In that case, the next task is to reduce the temperature imbalance rather than pretend it is absent.

Conventional drilled channels should be optimized first. Check their distance from the cavity, circuit balance, flow, pressure drop, coolant temperature rise, and access for cleaning. Baffles, bubblers, high-conductivity inserts, and separate circuits can often reach a localized hot spot without additive manufacturing.

Conformal cooling becomes attractive when straight drilling cannot follow the cavity surface or reach a deep core. Additive manufacturing can create curved internal channels closer to complex geometry, but the insert is not automatically better. Channel size, structural steel around the channel, surface finish, leak integrity, corrosion, pressure loss, water quality, and cleanability still need engineering control.

Evidence is application-specific. In one Oak Ridge National Laboratory demonstration, the modeled conformal design doubled heat-transfer rate at the mold interface, with the report describing cycle-time reduction as a potential production benefit rather than a universal percentage.[5] A separate peer-reviewed case with a pronounced thick region reported large simulated cooling-time reductions for several conformal and high-conductivity layouts.[3] Neither result should be copied into a quotation for another part. The business case must use the new part’s thermal analysis, predicted cycle saving, insert cost, expected volume, maintenance plan, and trial data.

Conformal cooling helps remove heat; it does not remove polymer shrinkage or correct a structurally poor thick-to-thin transition by itself.

 

Level 4: Use Gas Assist When a Controlled Hollow Channel Is the Design

Gas-assisted injection molding introduces pressurized nitrogen into molten polymer so gas penetrates selected thick regions or channels and pushes material toward the cavity surface. The gas can continue to apply internal pressure while the skin cools. Equipment suppliers and technical literature report potential reductions in sink, part weight, cavity pressure, and clamp demand for suitable geometries.[6][7]

The phrase “suitable geometry” carries most of the engineering work. Gas follows the lower-resistance molten path, not the intent shown on a drawing. The part and tool must therefore be designed around a controlled channel rather than treating gas as a late process setting.

Gas-Channel Design Questions to Resolve Before Cutting Steel

• Is there one continuous, predictable path from the gas entry toward the intended end of penetration?
• Does the channel act as a flow leader during polymer fill, and if so, does it create unwanted race tracking or air traps?
• Is the channel large and continuous enough to keep gas from fingering into adjacent nominal walls?
• Are closed loops or competing branches creating ambiguous flow paths?
• Is the gas entry positioned so the gas does not break through the melt front or enter a thin cosmetic area?
• Can displaced resin move into the remaining cavity volume or an overflow without overpacking another region?
• Where will the gas stop, and how will incomplete or excessive penetration be detected?
• Can the gas pin be accessed, sealed, cooled, and maintained?
• Which section of the hollow channel carries the service load, and what minimum residual wall is acceptable?

The Society of Plastics Engineers’ Injection Molding Division identifies a too-small channel as a cause of gas fingering into adjacent material and emphasizes designing the channel network to guide gas through the intended path.[8] That guidance is more useful than a universal dimension: final sizing depends on resin viscosity, nominal wall, fill pattern, temperature history, timing, pressure, and channel length.

Gas-Assist Failure Modes Are Diagnostic

Symptom	Design or process hypothesis	Evidence to collect
Gas fingering into a nominal wall	Intended channel is not the lowest-resistance molten path	Section parts along the path; compare fill and gas-penetration simulation with short-shot trials
Blow-through or a surface blister	Melt skin is too thin at gas arrival, dose is low, or pressure/timing is too aggressive	Record resin shot size, gas delay and pressure profile; section the failure location
Incomplete hollowing	Channel is discontinuous, freezes early, or competes with another branch	Map residual wall and hollow length over consecutive shots
Sink remains above the channel	Gas does not reach the hot mass soon enough or channel position is ineffective	Compare gas penetration with local temperature and gate-seal behavior
Variable dimensions	Gas penetration, resin dosage, melt temperature, or cooling is not stable	Trend part weight, gas pressure, channel wall, dimensions, and cycle conditions

 

Because these modes depend on interaction among part, mold, material, and gas delivery, production-intent trials and sectioning are part of process development—not merely final inspection.

When Gas Assist Is Worth the Complexity

Gas assist deserves serious evaluation when several of these conditions align:

• the part contains a long, thick, connected feature such as a handle or structural rail;
• surface sink over that feature is unacceptable;
• conventional coring would break the required outer form or load path;
• resin mass, clamp demand, or cooling time has a meaningful unit-cost impact at the expected volume;
• the geometry permits a controlled channel and accessible gas-pin location; and
• the project can support simulation, specialized tooling, gas controls, sampling, sectioning, and process validation.

It is often a weak fit for small or thin parts, isolated thick islands with no connected path, highly branched networks, low volume that cannot amortize development, or designs that can be fixed cleanly with coring and ribs.

Gas assist is also not the only advanced option. Microcellular molding dissolves a controlled supercritical fluid—commonly nitrogen or carbon dioxide—into the melt and creates distributed cells after the pressure drop. It can reduce density, sink, and clamp demand, but the cellular structure, surface, dimensions, and mechanical properties require application-specific qualification.[9] A two-piece assembly may be preferable when it creates two uniformly walled moldings and a robust joint. Each alternative changes the validation problem rather than removing it.

 

A Decision Ladder for DFM Review

Use the following sequence before the design is frozen:

1. Map the thick zones. Create a wall-thickness analysis and identify the local thermal mass, not only the nominal wall.
2. Map function and appearance. Mark load paths, bearing regions, sealing faces, cosmetic surfaces, datums, inserts, and allowable internal hollows.
3. Try geometry first. Replace bulk with section depth, ribs, gussets, flanges, or a closed profile.
4. Core the remaining mass. Check draft, core stiffness, cooling access, fill balance, weld lines, and tool action.
5. Model the thermal bottleneck. Use grade-specific thermal data and a realistic mold/coolant model; do not judge only by fill.
6. Price local cooling. Compare conventional circuits, inserts, and conformal cooling against predicted cycle and quality gains.
7. Evaluate gas assist as a designed process. Define the channel, entry, fill strategy, displaced-resin path, inspection method, and validation window before tooling release.
8. Prototype the risk. Sample with production-intent resin and section the thick regions. Record sink, voids, residual wall, dimensions, part weight, cycle, and functional results.

This ladder keeps the least expensive corrections available longest. Once the cavity is cut, geometry changes, cooling inserts, and gas-pin relocation become progressively more expensive.

For early supplier discussions, HordRT’s injection molding DFM guide, gas-assisted molding guide, and plastic injection molding service can be used as public scoping references. These links do not establish that a particular site or project includes gas-assisted equipment, simulation, sectioning, or validation; request those capabilities and deliverables explicitly.

 

Frequently Asked Questions

Can higher packing pressure fix a thick-section sink mark?

It may reduce sink when pressure can reach the region before gate seal, but it does not remove the thermal mass. It may also shift shrinkage, residual stress, flash, or void behavior. Treat it as a controlled diagnostic or optimization variable, not a substitute for evaluating the geometry.[1][2]

Should every thick plastic part be cored out?

No. Coring is the preferred early study when it preserves function and creates a manufacturable, supported, cooled core. Bearing loads, sealing geometry, impact requirements, optical paths, or tool-access limits may justify retained thickness.

Does conformal cooling eliminate sink marks?

No. It can improve local heat extraction and temperature uniformity, which may reduce cycle and differential shrinkage, but polymer shrinkage, gate seal, packing, material behavior, and junction geometry still matter.[3][5]

Does gas assist always reduce clamp tonnage?

Suitable gas-assist designs may operate at lower cavity pressure than conventional solid packing, but the reduction is part- and process-specific. Press selection still requires projected area, cavity-pressure evidence, safety margin, mold construction, and trial confirmation.[6][7]

 

Conclusion

The best thick-section solution is usually the first one that removes concentrated mass without compromising the load path. Start with ribs and section geometry, then core out the volume. Improve local cooling when functional geometry must stay thick. Choose gas assist when a controlled hollow channel is itself the right structural and manufacturing solution—not because a conventional design was allowed to remain bulky until tooling release.

For thick section plastic part design, the decisive review happens before steel is cut: map thickness, load, appearance, cooling, and gas paths together, then validate the real risk by molding and sectioning representative parts.

 

Sources

[1] BASF: Injection-Molding Problems in Engineering Thermoplastics—Causes and Solutions. https://download.basf.com/p1/8a8082587fd4b608017fd6631d5a24b1/en/Injection-Molding_Problems_in_Engineering_Thermoplastics_-_Causes_and_Solutions_Brochure_English.pdf

[2] Polymers: Thick-Walled Polycarbonate Optical Lenses—Cooling and Sink-Mark Study. https://pmc.ncbi.nlm.nih.gov/articles/PMC11360770/

[3] Polymers: Application of New Conformal Cooling Layouts to Complex Injection-Molded Parts. https://pmc.ncbi.nlm.nih.gov/articles/PMC9921164/

[4] Autodesk: Inputs to Moldflow Time-to-Reach-Ejection-Temperature Results. https://www.autodesk.com/support/technical/article/caas/sfdcarticles/sfdcarticles/Considerations-regarding-the-Time-To-Reach-Ejection-Temperature-result-with-Autodesk-Simulation-Moldflow.html

[5] Oak Ridge National Laboratory: Direct Metal Deposition Mold Plates With Conformal Cooling. https://www.ornl.gov/sites/default/files/2019-06/web_Radio%20Systems_%20MDF-TC-2013-026_Final%20Report.pdf

[6] Materials: Advanced Injection Molding Methods—Review of Gas-Assisted and Microcellular Processes. https://pmc.ncbi.nlm.nih.gov/articles/PMC10489002/

[7] BAUER Compressors: Gas-Assist Injection Molding Process. https://www.bauercomp.com/applications/plastics

[8] Society of Plastics Engineers, Injection Molding Division: Ten Part-Design Rules for Gas-Assisted Injection Molding. https://www.injectionmoldingdivision.org/2021/06/29/ten-part-design-rules-for-gas-assisted-injection-molding-process

[9] Trexel: MuCell Microcellular Injection Molding Technology. https://trexel.com/mucell