Assemblies · Lesson 9
Toolbox fasteners in assemblies
Toolbox is the SOLIDWORKS library of standard parts — bolts, screws, nuts, washers, pins, bearings — in ISO, DIN, ANSI and other standards. It comes with SOLIDWORKS Professional and Premium. Drag a fastener onto a hole and Toolbox picks a matching size and adds the mates; Smart Fasteners fills many holes at once.

Where to find it
Task Pane → Design Library → Toolbox (Professional and Premium)
Toolbox settings that matter
| Setting | Effect |
|---|---|
| Create Configurations (default) | Sizes are configurations of one master file per type |
| Create Parts | One part file per size |
| Permissions — Set the same for all users | Everyone uses the same rules |
| Hole Wizard/Toolbox folder (System Options) | Points SOLIDWORKS to the shared Toolbox database |
| Lock rotation for Toolbox concentric mates (2019+) | Stops bolts spinning and over-solving |
If the database cannot be found or is the wrong version, see Toolbox errors. Fasteners appear in the BOM with their size.
Practise it: compare Toolbox parts with models you build yourself — the spur gear, M10 bolt and nut and 6201 bearing.
Not in Toolbox? Download the supplier's model — see free SOLIDWORKS models.
Step by step
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1
Turn on Toolbox
Tools → Add-Ins, tick SOLIDWORKS Toolbox Library (and Utilities). Toolbox now appears in the Design Library tab.
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2
Prepare holes
Give the plate two M10 clearance holes made with the Hole Wizard (Hole type, ISO, screw clearance, Normal fit) instead of plain Ø10 holes.
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3
Drag a bolt onto a hole
Design Library → Toolbox → ISO → Bolts and Screws → Hex Head, drag a hex bolt and drop it on the edge of a hole. Toolbox suggests the size and length; confirm, and the bolt is mated.

Drop the fastener on the hole edge; Toolbox suggests the size. -
4
Change a size later
Right-click the bolt → Configure Component to change its size or length.
Common mistakes
- Each user with a different Toolbox folder — bolts change size or go missing on other PCs. Share one Toolbox; see Toolbox errors.
- Ctrl-dragging fasteners with Create Parts on Ctrl+Drag set — resellers do not recommend it.
- Modelling every thread. Toolbox fasteners use cosmetic threads to stay light.
Lesson 9 of 16 in the assemblies course.
Practice
Add one M10 hex bolt to each clearance hole by dragging from Toolbox. Check: the FeatureManager shows two instances of the same bolt part (one file, configured size), and each bolt is concentric with its hole.
Sources
- Hawk Ridge — Toolbox: manage and automate fasteners (Aug 2023)
- Hawk Ridge — Toolbox Smart Fasteners (Aug 2023)
- Javelin — SOLIDWORKS Toolbox setup (Nov 2023)
- GoEngineer — Fix Hole Wizard and Toolbox database errors (Sep 2024)
- Javelin — Toolbox lock rotation (2018)
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
Is Toolbox included in SOLIDWORKS Standard?
+
No. Toolbox is included in SOLIDWORKS Professional and Premium. It must be turned on as an add-in.
How do I add a bolt to a hole?
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Drag the fastener from Design Library → Toolbox onto the hole edge. Toolbox matches the size where it can and adds the mates.
What are Smart Fasteners?
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A command on the Assembly tab that adds fasteners to Hole Wizard holes automatically, sized to the holes, with optional washers and nuts.
Does Toolbox create a new file for every size?
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By default it creates configurations in one master file per fastener type, which grows over time. It can be set to create separate part files instead.
Related
- SOLIDWORKS SmartMates and Smart FastenersHow to use SmartMates in SOLIDWORKS: Alt-drag components to mate them instantly, which mates edges, faces and holes create, and Smart Fasteners.
- SOLIDWORKS Hole WizardHow to use the SOLIDWORKS Hole Wizard: hole types, standards, sizes and fit, the Type and Positions tabs, cosmetic threads, slots, favourites and Advanced Hole.
- SOLIDWORKS Toolbox and Hole Wizard errors — fixesFix SOLIDWORKS Toolbox errors: swbrowser.sldedb wrong version or missing, Hole Wizard database errors, fasteners changing size, read-only parts and PDM.
- SOLIDWORKS bill of materials (BOM)How to create a bill of materials in SOLIDWORKS: top-level, parts-only and indented BOMs, part numbers, custom columns, sorting, templates and balloons.