The injection molding boss design determines how well a plastic part accepts screws, threaded inserts, press-fit pins, and snap-fit connectors. A boss that is too thick creates sink marks and voids; one that is too thin cracks under assembly load.
Getting injection molding boss design right — wall ratios, fillet geometry, gusset placement, and draft — is one of the most direct ways to prevent costly first-article failures and assembly line rejections.
For a complete overview of rib design, wall thickness, draft angles, and DFM principles, see our Injection Molding Design & Engineering Guide.
What Is a Boss in Injection Molding
A boss is a cylindrical protrusion — a hollow post — molded integrally into a plastic part to serve as a mounting or fastening point. Bosses receive self-tapping screws, heat-set threaded inserts, ultrasonic inserts, press-fit pins, or act as alignment pegs in assemblies. They are among the most frequently used features in injection-molded enclosures, housings, brackets, and consumer product shells.
Unlike a solid post, a correctly designed boss is cored out — the center bore is formed by a core pin in the mold, leaving a hollow cylinder that provides adequate wall thickness for fastener engagement without the mass penalty of a solid feature. This core geometry is what makes injection molding boss design both structurally critical and dimensionally precise.
Core Boss Design Parameters
Every dimension of a boss in injection molding is governed by the relationship between the boss wall thickness, the nominal wall of the part, and the fastener’s requirements. The primary risk is identical to rib design: a boss wall that is too thick relative to the nominal wall creates a localized mass concentration that cools more slowly, producing sink marks on the visible surface directly opposite and internal voids within the boss wall itself.
The foundational rule of injection molding boss design is that the outer wall thickness of the boss should not exceed 60% of the nominal wall thickness. This single ratio, applied consistently, eliminates the majority of sink mark problems associated with boss features.
The outer diameter of the boss is typically set at 2× the inner bore diameter — a ratio that provides sufficient hoop strength for screw engagement while keeping wall mass within acceptable limits.
| Boss Design Parameter | Recommended Value | Consequence if Violated |
|---|---|---|
| Boss outer wall thickness | 50% – 60% of the nominal wall | Sink marks on the opposite cosmetic surface, internal voids |
| Outer diameter to bore ratio | 2× inner bore diameter | Insufficient hoop strength; boss splits under screw load |
| Base fillet radius (exterior) | 0.25× – 0.5× nominal wall | Stress concentration at base; cracking under lateral load |
| Base fillet radius (bore entry) | 0.25× – 0.5× bore diameter | Flow restriction into the bore; incomplete fill at the core pin tip |
| Maximum boss height | ≤ 3× outer boss diameter | Lateral instability; deflection under assembly load |
| Draft angle — outer wall | 0.5° – 1° per side | Drag marks on the boss exterior; tool wear on the cavity |
| Draft angle — inner bore | 0.25° – 0.5° per side | Core pin galling; inconsistent bore diameter along depth |
| Boss-to-wall standoff | ≥ 2× nominal wall from adjacent wall | Thick section between boss and wall; sink marks and voids |
Boss Wall Thickness and Sink Mark Risk
The most persistent quality problem in injection molding boss design is the sink mark produced on the part surface directly opposite a boss that is attached to or near the nominal wall. The mechanism is the same as for ribs: the boss wall and its connection to the nominal wall create a combined mass that retains heat longer than the surrounding geometry. As the interior contracts during cooling, it draws the solidified outer skin inward.
When a boss is positioned directly against the nominal wall — a common design shortcut — it creates a compound thick section where the boss outer wall, the boss base, and the nominal wall all intersect. This is one of the highest-risk configurations in plastic part design.
The preferred approach in injection molding boss design is to isolate the boss from the nominal wall, connecting it only through a narrow rib or gusset that carries structural load without adding significant mass. This keeps the connection geometry thin and dramatically reduces sink mark risk at the part’s exterior surface.
Design Warning
Never attach a boss directly to a side wall with a full-height connection. The resulting corner section — boss outer wall + nominal wall + corner fillet — creates a thick mass that is almost guaranteed to produce a visible sink mark on the opposite cosmetic surface. Connect the boss to the wall through a thin rib (≤ 60% of the nominal wall) instead.
Boss Height, Gussets, and Structural Support
A freestanding boss taller than approximately 3× its outer diameter will deflect laterally under assembly forces — whether from screw driving torque, press-fit insertion load, or in-service vibration. For tall bosses, gussets (triangular support ribs connecting the boss to the nominal wall or floor) are the standard DFM solution.
Gussets add lateral stiffness without significantly increasing the boss wall mass, provided they follow the same 50%–60% thickness rule applied to all rib features.
Gusset height should not exceed the boss height, and gussets should be evenly distributed around the boss circumference — typically two to four gussets at equal angular spacing. For bosses receiving high-torque self-tapping screws, four evenly spaced gussets are recommended to resist the torsional splitting force generated during screw drive-down.
| Fastener / Insert Type | Typical Bore Diameter | Boss Outer Diameter | Key Design Consideration |
|---|---|---|---|
| Self-tapping screw (M3) | 2.3 – 2.5 mm | 4.6 – 5.0 mm | Bore sized 85%–90% of screw OD; use 4 gussets for high torque |
| Self-tapping screw (M4) | 3.1 – 3.3 mm | 6.2 – 6.6 mm | Confirm the boss wall hoop strength for the resin chosen |
| Heat-set threaded insert (M3) | 4.2 – 4.5 mm | 8.4 – 9.0 mm | Larger bore requires increased boss OD; recheck wall ratio |
| Ultrasonic insert (M4) | 5.0 – 5.4 mm | 10.0 – 10.8 mm | The boss must withstand ultrasonic energy without cracking |
| Press-fit pin (3 mm) | 2.85 – 2.95 mm | 5.7 – 6.0 mm | Interference fit generates hoop stress; use PC or ABS for ductility |
| Alignment peg (no fastener) | Per mating part | 2× bore min. | Structural load is low; focus on dimensional accuracy and draft |
Draft Angle on Bosses
Both the outer wall and the inner bore of every boss require a draft angle. The outer wall drafts in the same direction as the part’s exterior walls — toward the parting line — at a minimum of 0.5° per side. The inner bore is formed by a core pin that the shrinking plastic grips tightly during cooling, making adequate bore draft critical for reliable ejection and consistent bore diameter along the depth of the boss.
For shallow bosses (depth-to-diameter ratio below 1.5:1), 0.25° of draft on the bore is generally sufficient. For deep bores (ratio above 2:1), increase to 0.5° or consider a collapsible core if zero-draft bore diameter is a functional requirement for the fastener engagement.
The cumulative effect of bore draft on the bore diameter at depth must be calculated and confirmed against the fastener’s minimum engagement diameter before tooling is finalized.
Design Tip
Specify the critical bore diameter at the top of the boss (at the parting line end), not at the bottom. Draft causes the bore to tighten with depth — the top is the widest point and sets the fastener entry condition. The tighter bore at depth actually improves thread engagement for self-tapping screws, provided the minimum engagement diameter is maintained throughout the full engagement length.
Boss Design for Screws and Threaded Inserts
The most common application for bosses in injection molding boss design is receiving self-tapping screws, where the screw cuts its own thread into the plastic bore wall during assembly.
Bore diameter for self-tapping applications is typically set at 85% – 90% of the screw’s nominal outer diameter — tight enough to generate sufficient thread engagement and pull-out resistance, but not so tight that the hoop stress from screw insertion cracks the boss wall.
For applications requiring repeated assembly and disassembly, or where high axial load is expected, heat-set brass inserts or ultrasonic inserts are specified instead of self-tapping engagement. These inserts are pressed into an oversized bore — either thermally or by ultrasonic energy — and their knurled outer profile bonds mechanically with the surrounding plastic.
Boss design for inserts requires a larger bore diameter (set by the insert supplier’s installation specification) and consequently a larger boss outer diameter to maintain the wall thickness ratio. Always confirm the boss outer diameter against the 2× bore rule after the insert bore size is determined.
Common Boss Design Mistakes
- The boss wall is too thick — the most common source of sink marks opposite boss features; always verify the 50%–60% nominal wall ratio.
- Boss attached directly to the side wall — creates a compound thick section; connect through a thin rib or gusset only.
- No exterior base fillet — sharp boss-to-floor transitions concentrate stress and restrict melt flow; minimum radius of 0.25× wall.
- Insufficient bore draft — core pin galling and inconsistent bore diameter result from zero or near-zero bore draft on deep bosses.
- Boss bore sized for nominal screw diameter — self-tapping bores sized at 100% of screw OD have no interference; target 85%–90% for proper thread engagement.
- No gussets on tall bosses — freestanding bosses taller than 3× outer diameter deflect under load; add gussets as standard practice.
- Ignoring insert supplier bore specification — heat-set and ultrasonic insert bores are precisely specified by the insert manufacturer; deviating from these values compromises pull-out strength.
Frequently Asked Questions
What is the standard boss wall thickness in injection molding?
The standard guideline is 50%–60% of the nominal wall thickness for the boss outer wall. This ratio prevents sink marks on the opposite surface while maintaining sufficient hoop strength for fastener engagement. For high-gloss cosmetic surfaces, reduce to 40%–50%.
How do you prevent sink marks on bosses in injection molding?
Keep boss wall thickness at or below 60% of the nominal wall, isolate the boss from side walls by connecting only through a thin rib, add generous base fillets, and ensure adequate packing pressure reaches the boss area through optimized gate placement. If sink marks persist, reduce wall thickness further or reposition the gate.
When should you use a threaded insert instead of a self-tapping screw boss?
Use threaded inserts when the assembly requires repeated disassembly (more than 3–5 times), when high axial load or torque is expected, or when the base resin is too brittle or too soft for reliable self-tapping engagement. Common applications include electronics enclosures, automotive brackets, and medical device housings.
Conclusion
Sound injection molding boss design comes down to controlling a small number of geometric ratios — outer wall at 50%–60% of nominal wall, outer diameter at 2× bore diameter, base fillets on both exterior and bore entry, and draft on both outer wall and inner bore.
These parameters, combined with disciplined isolation of bosses from adjacent walls through thin gussets rather than full-height connections, eliminate the sink marks, voids, and structural failures that make poorly designed bosses a persistent source of first-article problems.
At LZ Tooling, boss geometry is reviewed as part of every standard DFM analysis — verifying wall ratios, draft compliance, and fastener bore specifications before tooling is released, so assembly performance is built into the part from the first shot.