Capstone Model Package: Marine Winch Component Assembly and Drawing Set

Capstone Model Package: Marine Winch Component Assembly and Drawing Set

This lab is the culmination of your SolidWorks course. You will independently build a complete engineering deliverable — a marine winch drum assembly — from blank parts to a finished, ASME-compliant drawing set. The skills you demonstrate here directly mirror what employers and the CSWA credential expect: accurate solid modeling, correct assembly constraints, and professional documentation.

What a Marine Winch Assembly Involves

A drum winch hauls rope or wire rope aboard vessels by winding it around a rotating barrel. The assembly you are building contains four parts: a shaft, a drum barrel, two flanges (one on each end of the barrel), and a keyway feature on the shaft that locks the drum from spinning independently. Each part must be modeled separately as its own SolidWorks part file before any assembly work begins. Getting dimensions, tolerances, and feature relationships right at the part level prevents cascading errors in the assembly.

Step 1: Plan Before You Model

Before opening SolidWorks, read the project brief completely and write a design tree outline in your lab log. List every part, the base sketch plane, the key features (extrude, revolve, keyway cut, fillet), and the order you will build them. Your instructor must approve this plan in writing before you proceed. This gate exists because rework is expensive — both in industry and in your grade. Planning is a professional habit, not a formality.

Step 2: Build the Parts

Shaft: Start with a centerline revolve on the Front Plane. Dimension the diameter zones for the bearing seats and drum seat. Add the keyway as a rectangular extruded cut, fully defining the sketch with relations and dimensions so no sketch turns blue or under-defined yellow. Verify mass properties (Evaluate → Mass Properties) against the brief before moving on.

Drum Barrel: Use a Boss-Extrude with a shell, or a revolve profile that already includes wall thickness. Keep the bore concentric with the shaft seat.

Flanges: Build one flange, verify it, then derive or separately model the second. Use Smart Dimension and geometric relations so every sketch is fully defined (all lines black).

Keyway Details: The keyway must match the shaft slot in width and depth. In industry, keyway dimensions follow standard tables (refer to your project brief for the specified key size). The keyway cut on the shaft and the matching slot in the drum bore must align in the assembly — check this with a section view.

Step 3: Assemble with Mates

Insert parts into an assembly file. Fix the shaft, then apply mates:

• Concentric mate between shaft OD and drum bore.
• Coincident mates between flange faces and drum barrel ends.
• Coincident mate aligning the keyway features.

Run Interference Detection (Evaluate → Interference Detection) before declaring the assembly finished. Zero interference is required. An underdefined mate shows as a component that can still move — drag-test every part before closing the assembly. Resolve any warnings in the FeatureManager before proceeding to drawings.

Step 4: Exploded View

Create an exploded view (Insert → Exploded View) with clear separation along the shaft axis so each part is identifiable. The exploded view will appear on your assembly drawing sheet.

Step 5: Drawing Set — Three Sheets

Sheet 1 — Assembly Drawing: Use the approved drawing template. Place the assembly view and the exploded view. Insert a Bill of Materials (BOM) linked to the assembly. Every part must appear in the BOM with part number, description, material, and quantity. Add balloon callouts that match BOM item numbers. Title block must be complete: part name, drawn-by, date, scale, revision.

Sheet 2 — Shaft Detail Drawing: Include front view, section view through the keyway, and an end view. Apply dimensions per ASME Y14.5-2018: use proper tolerance formats, datum references where required, and surface finish symbols if called out in the brief. Dimension the keyway width and depth with limits.

Sheet 3 — Sheet Metal End Cap Flat Pattern: If the end cap is modeled as a SolidWorks Sheet Metal part, insert the flat pattern view using Insert → Drawing View → Flat Pattern. Note the bend lines and any weld symbols per AWS A2.4 if the brief specifies a weld joint on the cap flange.

ASME Y14.5-2018 Compliance Checklist

Before printing or submitting drawings, verify: all dimensions have tolerances, no dimension is duplicated, views are in first-angle or third-angle projection consistently (third-angle is standard in the US), section arrows point in the correct direction, and the title block is complete. Missing or incorrect GD&T is one of the most common reasons a drawing is rejected in industry.

Desk Review

The 10-minute desk review is a professional simulation. You will explain your modeling decisions, show how you resolved any interference or underdefined sketch, and make a live change the instructor requests (such as changing the shaft diameter or flange bolt-circle count) and rebuild without error. Practice explaining out loud before the review day — clear verbal communication is part of every engineering team's daily work.

Safety in the CAD Lab

The lab is a low-physical-hazard environment, but digital hygiene matters: save your SolidWorks files to the designated network folder at the end of every work session — data loss is the most common lab emergency. Follow the lab's lockout/tagout awareness: do not touch physical shop equipment in adjacent bays during CAD lab hours without proper authorization and PPE. Eye strain is real — follow the 20-20-20 rule (every 20 minutes, look 20 feet away for 20 seconds). Report any ergonomic discomfort (wrist, neck) to the instructor early.