Assemblies · Lesson 7
SOLIDWORKS exploded view
An exploded view pulls the components of an assembly apart in steps so you can see how it goes together — for assembly instructions, manuals and drawings. Each step moves or rotates components; a radial step pushes a ring of parts out from an axis at once. Explode lines show the paths, and the explode can be animated or shown in a drawing view.

Where to find it
Assembly tab → Exploded View
Exploded view features by version
| Version | Added |
|---|---|
| 2015 | Radial explode steps |
| 2018 | Smart Explode Lines — all lines in one click |
| 2019 | Rollback bar, reordering, naming and suppressing steps |
| 2020 | Auto-space options: bounding box centre, front or rear |
Auto-space spreads several selected components evenly along the drag direction; select the part that should move furthest first. Exploded views are stored per configuration. In a drawing they are usually combined with a BOM and balloons — see BOM and balloons in drawings.
Step by step
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1
Start the exploded view
Open the plate-and-pins assembly. Assembly tab → Exploded View.
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2
Create the first step
Click one pin. A triad appears; drag its vertical arrow upward about 50 mm (or type the distance). Click Add Step (or Done).

Drag the triad arrow to move a component, then add the step. -
3
Explode the second pin
Select the second pin and drag it up 50 mm as another step. Explode in the order you would take the assembly apart — explode lines follow that order.
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4
Add explode lines and animate
Finish, then right-click the exploded view in the ConfigurationManager → Smart Explode Lines → OK. Right-click again → Animate collapse/explode to play it.
Common mistakes
- Clicking the red X in the Exploded View PropertyManager — it cancels the whole explode. Use the undo arrow in the PropertyManager instead.
- Exploding in a random order. Follow the real disassembly order so lines and animations make sense.
- Trying to pick single parts of a subassembly without ticking Select sub-assembly parts.
Lesson 7 of 16 in the assemblies course.
Practice
Explode both pins 50 mm up in two steps and add smart explode lines. Check: the exploded view shows 2 steps in its list, and double-clicking it in the ConfigurationManager collapses and explodes the assembly.
Sources
- Solid Solutions — How to create an exploded view (Jan 2025)
- GoEngineer — Create a radial explode (Jun 2022)
- CATI — Regular and radial explode steps (Apr 2022)
- CATI — Radial explode in SOLIDWORKS 2015
- CATI — Exploded view spacing options (2020)
- Javelin — SOLIDWORKS 2019 exploded view
- Javelin — Smart Explode Lines (2018)
- GoEngineer — Smart Explode Lines explained (Jan 2022)
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
How do I create an exploded view in SOLIDWORKS?
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Assembly tab → Exploded View. Select components, drag the triad arrows to move or rotate them, and add each movement as a step.
What is a radial explode?
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A step type, added in SOLIDWORKS 2015, that moves several components out radially from an axis at once — for example a ring of screws.
How do I add explode lines?
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Right-click the exploded view and choose Smart Explode Lines (since 2018), or draw them manually with an Explode Line Sketch.
How do I show an exploded view in a drawing?
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Insert an isometric view of the assembly and tick Show in exploded or model break state in the drawing view's PropertyManager.
Related
- SOLIDWORKS Interference DetectionHow to use Interference Detection in SOLIDWORKS: overlaps and their volume, ignoring and isolating results, Clearance Verification and Hole Alignment.
- 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.
- SOLIDWORKS assembly basicsSOLIDWORKS assembly basics: start an assembly, insert components, fixed and floating parts, degrees of freedom, moving and rotating components, and Pack and Go.
- SOLIDWORKS configurationsHow to use configurations in SOLIDWORKS: add them, change dimensions and suppress features per configuration, configuration tables and display states.