Exploded Views, Assembly Configurations, and Bill of Materials

Exploded Views, Assembly Configurations, and Bill of Materials

Why Exploded Views Matter in Marine and Manufacturing Documentation

When a machinist in a shipyard or a fabrication shop receives a set of assembly drawings, they need to understand how every part fits together before they touch a single tool. An exploded view separates the components of an assembly along logical axes so each part is visible, identified, and spatially related to its neighbors. Combined with a Bill of Materials (BOM), the exploded view becomes the primary reference document for ordering stock, staging parts, and verifying deliveries. In marine manufacturing, where a misidentified fastener can cause catastrophic failure at sea, accuracy in these documents is not optional.

Assembly Configurations in SolidWorks

SolidWorks stores multiple states of an assembly in a single file using Configurations. The two configurations you will use most often are the Resolved (fully assembled) configuration and the Exploded configuration. You create an exploded view inside a configuration rather than as a separate file, which means the geometry stays linked to the live model. If a part is renamed or a dimension changes, the exploded view and BOM update automatically when you rebuild.

To access configurations, open the ConfigurationManager tab (the stacked-pages icon at the top of the left panel). Right-click the active configuration and choose New Exploded View to launch the Explode PropertyManager.

Creating an Exploded View with the Explode Step Tool

The Explode Step tool moves one or more selected components along a chosen direction by a specified distance. Each move is recorded as a discrete step, so you can edit, reorder, or delete individual steps later without rebuilding the whole sequence.

Best practice for step distances: separate parts far enough that a leader line and balloon will fit without overlapping adjacent components. For small assemblies like a clevis-and-pin, 25–50 mm per step is usually sufficient on a standard drawing sheet. Larger weldments may require 150 mm or more. The goal is clarity, not photographic realism.

After all steps are defined, click Done in the PropertyManager. Use Collapse to return the assembly to its assembled state, then Explode again to confirm the steps replay correctly. This repeatability check is critical: if the model is shared electronically, a recipient must be able to collapse and re-explode without error.

Placing the Exploded View on a Drawing Sheet

With the drawing template open, insert a new view using Insert → Drawing View → Model. In the PropertyManager, select Current Model View and choose the saved exploded configuration from the Reference Configuration drop-down. SolidWorks will place the view in its exploded state on the sheet.

Scale the view so every part is legible. For a five-component clevis assembly, a 1:1 or 2:1 scale on a B-size (11 × 17 in) sheet is typical.

Balloons and the Automatic BOM

Balloons are annotation circles that point to each component and display the BOM item number. Insert them using Insert → Annotations → Auto Balloon after the BOM is placed, or add them individually. SolidWorks links balloon numbers directly to BOM rows, so renumbering the BOM updates all balloons automatically.

Insert the BOM table using Insert → Tables → Bill of Materials. SolidWorks reads part numbers and descriptions from each component's File Properties (File → Properties in the part or subassembly file). This is why keeping file properties current is essential — a blank Description field produces a blank BOM cell.

Adding a Custom Material Column

The default BOM includes Item No., Part Number, Description, and Quantity. For manufacturing and marine drawings, a Material column is required by most shop standards. To add it:

1. Click inside the BOM table to activate it.

2. Right-click any column header and choose Insert → Column Right (or Left).

3. In the Column Type drop-down, select Custom Property and type `Material`.

4. SolidWorks will populate each row from the `Material` custom property in each part file.

If a cell remains blank, open the corresponding part file, go to File → Properties → Custom, and add the `Material` property manually. Do not type material names directly into the BOM table cells — that breaks the parametric link and creates a static table that will not update if the model changes.

ASME Y14.34 and Documentation Standards

ASME Y14.34 governs the format and content of Associated Lists, which includes BOMs used with engineering drawings. Key requirements include consistent item numbering that matches balloons, clear part number and description fields, and quantity expressed as a whole number. While SolidWorks automates much of this, the drafter is responsible for verifying compliance before issuing documents. In marine applications, classification societies and shipyard quality systems may impose additional requirements on top of ASME standards.

Production Documentation Audit

In professional practice, a receiving inspector compares the physical parts or the 3D model against the issued BOM to catch errors before fabrication begins. Discrepancies are recorded on a punch list — a written log of items that must be corrected before the document is accepted. Common punch list items include wrong material listed, part number that does not match the file, quantity mismatch, and balloons pointing to the wrong component. Practicing this audit role in the classroom builds the habit of independent verification that employers in both manufacturing and marine sectors expect.

Safety Note

SolidWorks is a software environment, so the primary hazards are ergonomic: eye strain from extended screen time, and repetitive-stress injury from mouse and keyboard use. Follow your facility's workstation ergonomics guidelines. If you print drawings for the punch-list exercise, the printer area is shared equipment — keep the pathway clear and do not leave hot output unattended. No lockout/tagout or PPE beyond standard ergonomic awareness applies to this lesson.