Exploded views in SOLIDWORKS, Fusion, Inventor and Onshape

All four work the same way underneath: you record one or more explode steps (which parts move, which way and how far), save them with the assembly, and then pick that exploded state when you place a view on a drawing sheet. Menu names change between versions; these are from each maker's current help, read on 1 November 2026.

SOLIDWORKS

1. 01

   Start the exploded view

   Click Exploded View, or Insert > Exploded View, or right-click a configuration in the ConfigurationManager and choose New Exploded View.

2. 02

   Pick the parts for the first step

   Select one or more components, then drag a translation or rotation handle. You can type an explode distance or angle instead.

3. 03

   Add more steps

   Click Done for each step, add the next, and click the green tick when the explosion is complete. It is saved under the configuration, and a configuration can hold several.

4. 04

   Put it on a drawing

   Insert a Model View of the assembly, then right-click the view and choose Show in Exploded State (or tick Show in exploded or model break state in its properties).

To send the assembly to someone else: File > Save As, choose STEP under Save as type, and set the version under Options.

Autodesk Fusion

1. 01

   Switch to Animation

   Change to the Animation workspace and start a new storyboard (Storyboard > New Storyboard, type Clean).

2. 02

   Explode

   Select the top of the assembly and use Transform > Auto Explode: All Levels, setting the distance with the slider; or use Transform > Manual Explode and drag the parts yourself.

3. 03

   Put it on a drawing

   From the workspace menu choose Drawing > From Animation, pick the storyboard as the reference, choose the template and standard, and place the base view.

4. 04

   Parts list and balloons

   Add Tables > Parts List: Fusion adds balloons to the view it labels.

To export a STEP file: File > Export, choose "STEP files (*.stp, *.step)" as the type, and click Export. Fusion's help lists STEP export for Personal Use licences too.

Autodesk Inventor

1. 01

   Make a presentation file

   Create a presentation (File > New, the .ipn template), or right-click the assembly in the browser and choose Create Presentation, and insert the model.

2. 02

   Tweak the parts

   Start a storyboard, then use Tweak Components on the Presentation tab: select parts, choose move or rotate, and drag the triad or type a distance.

3. 03

   Take a snapshot

   Capture the exploded state with New Snapshot View and save the .ipn.

4. 04

   Put it on a drawing

   Right-click the snapshot and choose Create Drawing View, or run Base View in an existing drawing and pick the .ipn and the snapshot.

To export a STEP file: File > Export > CAD Format, and choose STEP.

Onshape

1. 01

   Open the Exploded views panel

   In an Assembly tab, click the exploded view icon and Add exploded view.

2. 02

   Add steps

   Select parts (a box selection works), drag the manipulator or type a distance, choose translation or rotation, and tick each step. Explode lines are on by default.

3. 03

   Finish

   Click Done. Exploded views are made in the browser; Onshape's phone and tablet apps show them but don't make them.

4. 04

   Put it on a drawing

   Use Insert view and pick the named exploded view from the Explode/Position list.

To export a STEP file: right-click the Assembly tab, choose Export, and set the format to STEP.

When you only have the STEP file

Suppliers and customers usually send a STEP file rather than the native model, and not everyone who needs the drawing has the CAD program. See how to make an exploded view from a STEP file.