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.

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

A parts-only BOM — one row per unique part, with quantities. -
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
- CATI — BOM types
- Javelin — Sort a bill of materials and save settings (Jun 2025)
- Javelin — SOLIDWORKS BOM template
- CADimensions — Control part numbers in a BOM
- Javelin — Combine custom properties in a BOM
- Javelin — SOLIDWORKS 2022 assemblies
- Javelin — Balloons in drawings (Nov 2022)
- Solid Solutions — How to create part templates
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?
+
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?
+
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?
+
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?
+
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.
Related
- Component patterns and Mirror ComponentsHow to pattern components in SOLIDWORKS assemblies: linear, circular, pattern driven and chain patterns, plus Mirror Components and opposite hands.
- SOLIDWORKS subassembliesHow to create subassemblies in SOLIDWORKS from selected components, save virtual ones, make them flexible or dissolve them, and why they speed things up.
- SOLIDWORKS exploded viewHow to create an exploded view in SOLIDWORKS: regular and radial steps, auto-space, smart explode lines, animation, and showing the exploded state in drawings.
- How to create SOLIDWORKS templatesCreate SOLIDWORKS part, assembly and drawing templates (.prtdot, .asmdot, .drwdot), save them to your own folder and set them as the defaults.