Injection Molded Sunglasses

Y2K-inspired injection-molded sunglasses designed and manufactured 

Design Iterations

The sunglasses went through multiple CAD revisions before being committed to tooling. Early designs had overly complex geometry with thin features that the 1/8" ball end mill could not faithfully reproduce. Key iteration decisions included: 

• Simplifying the outer rim profile to avoid radii smaller than the smallest available end mill 

• Increasing nominal wall thickness on the frame rim after flow simulation showed incomplete fill in thin regions 

• Adjusting the arm geometry to reduce volume below 2 oz while maintaining structural rigidity 

• Relocating gate positions based on flow simulation feedback to reduce weld-line formation in cosmetically critical areas 

Design Results & DFM Analysis

Gate Type and Location 

Both parts used a single edge gate located at a non-cosmetic surface; at the center of the arms on the arms mold, and on the inner nose-bridge area of the frame mold. Edge gates were selected because they are easy to manually trim post-ejection and provide directional fill control. The gate was sized to allow adequate flow given the 1/8" default end mill constraint while minimizing gate vestige on visible surfaces. 

Parting Line Location 

For the frame mold, the parting line was placed along the widest horizontal cross-section of the part; essentially along the mid-plane of the glasses frame. This allowed both A and B sides to be machined with straightforward 3-axis toolpaths and avoided undercuts. Similarly, for the arms mold, the parting line was placed along the vertical midline of the arms. 

Draft Angle Analysis 

All mold-release faces were designed with 5° draft as required by course guidelines, applied using the 5° draft tool available in the library. Draft analysis was performed in CAD on both parts prior to committing to tooling. The frame presented the greatest challenge because the curved lens opening required compound draft that was carefully verified to ensure the part could be ejected without drag marks or tearing. 

Possible Design Optimizations 

In retrospect, several design changes would improve manufacturability and part quality: 

• Increase minimum wall thickness to ≥0.125" throughout the frame to prevent warping and ensure complete fill without requiring elevated injection pressures 

• Use a 1/16" ball end mill for the lens-rim geometry, or redesign the rim profile to a radius ≥1/8" achievable with the standard tool set 

• Add a small ejector-pin boss on the inside of the frame to allow mechanical ejection rather than manual prying, which contributed to part distortion 

• Reduce the frame's projected area to allow lower clamping force (6.5 ton was at the high end of machine capacity) 

• Consider a two-cavity arm mold to halve cycle count for the 5-assembly run 

Flow Analysis

Manufacturing

CAM & Machining 

CAM toolpaths were generated in Fusion 360 for both mold halves. A 3/4" shear hog was used for all roughing, as well as a 3/8" ball endmill and a 1/4" ball endmill. Finishing passes and fine details were accomplished with 1/8" and 1/16" ball endmills.

Machining was performed on a Tormach CNC mill. Both frame mold halves required approximately 11 hours of total machining time, as did both arm mold halves. A 1/8" end mill was broken during arm mold machining, adding $16.43 to tooling cost. All mold faces were machined to the best surface finish achievable with available tooling before injection molding. 

CAD Models

CAM Paths

Machining

Finished Molds

Injection Molding Parameters

Challenges

Surface Finish of Mold Halves 

Achieving a satisfactory surface finish on the aluminum mold halves proved difficult, particularly on the concave lens-rim geometry of the frame. The ball end mill leaves characteristic scalloped cusps whose height is a function of step-over distance and tool radius. With the 1/8" ball end mill, achieving a visually acceptable finish required a very fine step-over, significantly increasing machining time. 

DFM Resolution: Step-over was reduced to the minimum practical value for cosmetically important surfaces, accepting the associated machining time cost. Future iterations would benefit from specifying surface finish requirements in CAM and using a dedicated finishing pass strategy (e.g., scallop toolpath) to meet them systematically. 

Runner Diameter: Inadequate Fill Due to Under-Milled Channels 

The runner and gate channels in the mold CAD were designed at a nominal diameter, but the as-machined channels were undersized relative to the CAD model. This restricted polymer flow and contributed to short shots and incomplete fill in initial molding attempts. 

DFM Resolution: The runner channels were manually enlarged using manual bridgeport mill after the initial machining run. Flow was verified by test shots before committing to production parts. Going forward, runner diameter should be specified with a positive machining tolerance (e.g., program slightly oversized) to account for real-world cutting behavior, and a brief test shot at low pressure should be performed before optimizing for production parameters. This experience directly informed the importance of verifying toolpath simulation against post-processor output before committing to metal. 

Inconsistent Shots: Temperature & Pressure Balancing 

Early injection molding attempts produced incomplete fills and short shots, particularly in the thin rim sections of the frame. The root cause was a combination of insufficient injection pressure, mold temperature variation between shots, and material cooling too quickly in thin sections before the cavity was fully packed. 

DFM Resolution: Injection force was progressively increased to 7,000 PSI for the frames and clamping force raised to 6.5 tons to prevent flash while ensuring full fill. A consistent block pre-heating procedure (2 minutes for frames, 3 minutes for arms) was established and strictly followed between shots to minimize thermal variation. Cooling time was extended to 1 minute for frames to allow sufficient solidification before mold opening, reducing part ejection distortion. These process parameter optimizations stabilized shot quality and enabled production of five acceptable assemblies. 

Dimensional Analysis

Arm Dimensions

Arm dimensions were considerably closer to nominal. The slight width undersize is attributed to corner rounding from end mill radius at tight-radius intersections. The thinnest section was actually thicker than designed because the end mill could not fully reach the deepest pocket geometry — a conservative outcome that preserved structural integrity. 

Bill of Materials & Cost Analysis

Detailed Manufacturing BOM

Costs at Scale

At the class's target production volume of 1,000–10,000 units/month, injection molding is economically compelling. The high up-front tooling cost (~$3,300 combined for both parts in our case) is rapidly amortized and per-unit cost approaches material cost at volume. A polished mold finish (not achieved in this project) would add cost but dramatically improve cosmetic quality for a retail product. 

Cycle Time Summary