Mechanical Assembly Drawings and Bill of Materials

Mechanical Assembly Drawings and Bill of Materials

What an Assembly Drawing Does

An assembly drawing shows how individual parts fit together to form a complete product. Unlike a detail drawing, which documents one part in full, an assembly drawing communicates the relationship between parts — their positions, orientations, and the order in which they go together. In manufacturing and marine drafting, assembly drawings are the primary document a technician reads on the shop floor or in the shipyard.

A complete mechanical assembly drawing package contains at minimum:

• One or more assembled views showing the parts in their working positions.
• An exploded view showing the parts separated along their assembly axes so each component is identifiable.
• Balloon callouts linking each part in the views to a numbered row in the parts list.
• A bill of materials (BOM), also called a parts list, that catalogs every component.

The Exploded View

An exploded view pulls components apart along the axes they travel during assembly. In SolidWorks, you create an exploded view inside the assembly file using the Exploded View tool (Insert → Exploded View). You drag each component along its assembly direction and set an offset distance that gives visual clarity without wasting sheet space. Good practice: keep exploded steps in assembly order so a reader can mentally reverse the steps to disassemble the product.

Once the exploded view is saved in the assembly file, you insert it onto the drawing sheet as a named configuration. SolidWorks labels the exploded configuration automatically; you reference it when placing the view on the sheet.

Balloon Callouts

Balloons are circular leaders that point to a component in a view and display a number. That number corresponds to a row in the BOM. ASME Y14.35 and common industry practice require that every component shown in the assembly appear in at least one balloon, and every balloon number must have a matching BOM row — no orphaned balloons, no unbalanced rows.

In SolidWorks Drawing, use Insert → Annotations → Auto Balloon on the exploded view to place all balloons in one step. Review each balloon afterward: confirm it points to the correct component and that the number sequence is logical (typically starting at 1 in the upper-left and proceeding clockwise or top-to-bottom). Reorder item numbers in the BOM table properties if needed to match a logical sequence.

The Bill of Materials

The BOM is a structured table, usually placed above the title block or in the upper-right area of the sheet. At minimum, each row contains:

| Column | Content |

|---|---|

| Item No. | Matches balloon number |

| Part Number | Drawing or catalog number |

| Description | Brief, plain-language name |

| Material | Alloy, grade, or trade name (e.g., 1018 CR Steel, 6061-T6 Aluminum) |

| Quantity (QTY) | How many of that part per assembly |

In SolidWorks, the BOM is generated automatically from the assembly file's component list using Insert → Tables → Bill of Materials. The table is linked to the model: if you change a part property in the assembly, the BOM updates. Always verify the auto-generated BOM against the actual components — phantom or envelope parts can appear unexpectedly and must be suppressed or excluded.

The Change-Order and Revision Process

Engineered drawings are living documents. When a design change is approved, the drafter performs a formal revision that:

1. Updates the affected view or dimension.

2. Adds a revision cloud (a cloud-shaped outline, per ASME Y14.35) around the changed area on the drawing sheet to highlight what changed.

3. Records the revision in the revision block in the title block area, adding the revision letter (A, B, C…), a brief description of the change, the date, and the approver's initials.

4. Updates the BOM or detail as needed — in this case, editing the Material cell for the changed part.

The revision cloud and revision block entry together form a permanent, auditable record of the change. Never erase or overwrite a previous revision; increment the letter.

SolidWorks Workflow Summary

1. Open the provided assembly file; confirm all mates are fully defined.

2. Create the exploded view in the assembly; save the file.

3. Open a new drawing using the mechanical title block template.

4. Place the assembled view (isometric or front/top/right orthographic as required).

5. Place the exploded view using the saved exploded configuration.

6. Auto-balloon the exploded view; verify and clean up balloon positions.

7. Insert the BOM table; populate or verify Part Number, Description, Material, and QTY columns.

8. For the change-order exercise: revise the Material property in the part file, rebuild the assembly, return to the drawing, confirm the BOM updates, add a revision cloud with the Sketch tool or annotation cloud tool, and fill in the revision block.

Safety Note

SolidWorks is used to design parts that will be manufactured on CNC machinery, presses, and welding equipment. Drawings you produce may be used on a real shop floor. Errors in the BOM — wrong material, wrong quantity — can result in parts being machined from incorrect stock, leading to equipment failure or injury. Treat every BOM entry as safety-critical. Before releasing any drawing, check:

• Every balloon has a matching BOM row.
• Material specifications are exact and match the engineering requirement.
• Quantities are correct; under-ordering fasteners or over-ordering heavy components both create hazards on a marine or manufacturing job site.

When working in a lab environment that includes physical hardware or sample assemblies, follow all posted shop rules. If a physical vise or tooling is used for reference, keep fingers clear of moving jaws and wear safety glasses whenever handling metal components.