CAD History, Versions, and Sharing
Separate feature order from edit history, preserve useful design states, and share the intended model with the right access.
The feature list describes how geometry is built
The feature list describes how geometry is built
The SOLIDWORKS FeatureManager design tree and the Onshape feature list help you find sketches and modeling features. Later features can depend on earlier geometry. Rename important features so another reader can tell what they do.
A tree also contains items such as planes, bodies, or components; not every row is a modeling operation. To understand how features build a part, continue with Feature-based Modeling.
A rollback bar lets you work at an earlier position in the feature sequence while later features are temporarily left out of regeneration. Move it forward again to evaluate the complete model and check dependent features. Rolling back does not retrieve an old saved revision, and it is not the same operation as separately suppressing one feature.
Rollback follows the regeneration sequence
SOLIDWORKS Rollback Bar help explains moving through the feature sequence. A file can be saved with its bar rolled back, so inspect the bar's position when reopening a model.
Onshape history records edits; versions preserve milestones; Interactive
Onshape history records edits; versions preserve milestones
Onshape records completed edits in document history. The feature list shows the modeling sequence; history records changes to the document over time. Editing an early sketch today changes the history today even though the sketch remains early in the feature list.
A version captures the design state of the workspace, including its tabs, at a named point. That captured design state is read-only. Use a meaningful milestone name and description so a reviewer knows which state you mean.
A branch starts from a version and provides a separate workspace for further edits. Use it to explore an alternative while preserving the starting version. Compare changes before merging; merging needs review, not just a button click.
Viewing history, restoring, and branching serve different purposes
Viewing an earlier state is inspection. Restoring changes a workspace back to an earlier state. Branching gives you a separate place to continue editing. Check the active workspace before any restore or merge. See Onshape Versions and History and Document Management.
Worked symbolic timeline: feature order stays put while edits accumulate
What: the feature list remains Mounting sketch → Base extrude → Edge fillet. Why: editing the first feature later should add a new history event, not move that feature to the end of the regeneration sequence.
- Start Main workspace: sketch width 60 mm, extrude depth 12 mm, fillet radius 2 mm.
- Edit the early Mounting sketch now: width 60 → 72 mm. It remains feature 1.
- Create the fixed Design review snapshot: 72 / 12 / 2 mm.
- Edit Main again: sketch width 72 → 84 mm. The snapshot still reads 72 / 12 / 2 mm.
- Create Lightweight branch from Design review, then edit only its extrude depth 12 → 8 mm.
- 1 · Mounting sketch — width starts at 60 mm.
- 2 · Base extrude — depth starts at 12 mm.
- 3 · Edge fillet — radius starts at 2 mm.
| State after the worked actions | Sketch width | Extrude depth | Fillet radius |
|---|---|---|---|
| Main workspace · editable | 84 mm | 12 mm | 2 mm |
| Design review · fixed snapshot | 72 mm | 12 mm | 2 mm |
| Lightweight branch · editable | 72 mm | 8 mm | 2 mm |
This is a symbolic in-memory model, not Onshape or SOLIDWORKS. It performs no rollback, restore, merge, save, file operation, or permission change.
A SOLIDWORKS save or file copy needs its own revision plan
A SOLIDWORKS save or file copy needs its own revision plan
In a local file workflow, Save writes the current document to disk. A deliberate copy can preserve an earlier state, but a filename alone does not establish a managed revision or capture all referenced files. Keep descriptive names and know which copy is the active design.
Before copying an assembly or drawing for an alternative, check what its references will point to. Two assembly copies can still use the same part file; editing that shared part can affect both. Use the transfer checks in CAD Files and Documents.
SOLIDWORKS installations may use PDM or connected data management for version and revision control. Follow that system's workflow when present; local Save and Save As are not a universal replacement for it.
Share the intended state and check the recipient's access; Checklist; Practice
Share the intended state and check the recipient's access
In Onshape, decide whether the recipient needs to inspect a fixed version or collaborate in an editable workspace. A link to a changing workspace can show later edits; a version identifies a fixed design state. Grant access using the document's sharing controls.
- Confirm the document, workspace or version, and tab you intend to share.
- Review document visibility and the intended recipient.
- Choose view or edit access and inspect additional permissions such as export, copy, and resharing.
- Check that the recipient can open the intended state with the intended access.
Do not assume that sending a URL grants access, or that view access prevents copying or exporting. Available sharing options depend on the account and organization. Review Onshape Share Documents for those permissions.
Choose version or branch Distinguish rollback from history Check sharing