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Assemblies · Lesson 16

SOLIDWORKS bill of materials (BOM)

A bill of materials lists every component of an assembly with its quantity, part number and description. SOLIDWORKS builds it automatically from the assembly and the parts' custom properties, and keeps it in step with the balloons on the drawing. Choose top-level only, parts only or indented depending on whether subassemblies should appear as units.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Assembly drawing with numbered balloons and a bill of materials table

Where to find it

Drawing: Insert → Tables → Bill of Materials

BOM types

Type Lists
Top-level only First-level parts and subassemblies as single rows
Parts only Every part, subassemblies dissolved
Indented Subassemblies with their parts indented below

Useful BOM settings

Setting Detail
Part number source Configuration properties: document name (default), configuration name or user specified
Custom property columns Column type Custom Property + property name
Combined values e.g. a Description built from several properties with $PRP:"..." references
Sort Right-click → Sort → Save current sort settings
Template Right-click → Save As → .sldbomtbt; use it in drawings and assemblies
Exclude Component, configuration or model (2022+)
Balloons Auto Balloon numbers follow the BOM; editing a balloon updates the BOM

This is the last lesson of the assemblies course; drawings come next — see BOM and balloons in drawings. Custom properties are easiest to manage in your part templates.

Step by step

  1. 1

    Give the parts properties

    In the plate and the pin, open File → Properties and add Description (for example "Base plate", "Pin Ø10 × 30"). These feed the BOM columns.

  2. 2

    Make a drawing of the assembly

    Create a drawing of the plate-and-pins assembly with an isometric view.

  3. 3

    Insert the BOM

    Insert → Tables → Bill of Materials, select the view, choose a template (star icon) and the type — Parts only for this example — and place the table.

    Parts-only BOM with the plate quantity 1 and the pin quantity 4
    A parts-only BOM — one row per unique part, with quantities.
  4. 4

    Add balloons

    Annotation → Auto Balloon on the view. The balloon numbers match the BOM item numbers; changing a balloon number updates the BOM.

Common mistakes

  • Typing part numbers into a PartNo property and expecting the Part Number column to use it. The PART NUMBER column follows the configuration setting (document name, configuration name or user specified); use a custom property column for your own field.
  • Missing descriptions because the parts' templates have no properties. Add them to your part templates.
  • Reference parts such as skeletons appearing in the BOM — exclude them, or insert them as envelopes.

Lesson 16 of 16 in the assemblies course.

Practice

Create a parts-only BOM of the plate with four pins from the previous lesson. Check: two rows — plate, quantity 1 and pin, quantity 4 — and four balloons on the pins sharing item number 2.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

How do I insert a BOM in SOLIDWORKS?

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In a drawing, Insert → Tables → Bill of Materials, select a view of the assembly, choose a template and type, and place it. A BOM can also be inserted directly in the assembly.

What is the difference between top-level, parts-only and indented BOMs?

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Top-level lists only the first level, with subassemblies as single rows. Parts only lists every part, without subassemblies. Indented shows subassemblies with their parts indented beneath them.

How do I add a custom column to a BOM?

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Insert a column, set its type to Custom Property and choose the property name, such as Description or Material.

How do I exclude a part from the BOM?

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Use Exclude from Bill of Materials in the component's properties; since 2022 this can be set for a component, a configuration or a model.