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SOLIDWORKS External References: What the Symbols Mean and How to List, Lock and Break Them Before You Share an Assembly | SolidWorks | Register and Certify IP of CAD design

2026-03-15 07:47 Guides
TL;DR: SOLIDWORKS external references in one paragraph

A SOLIDWORKS external reference is a link that makes one file depend on another: an in-context feature on a part follows the geometry of another component in the assembly. You see it as -> after the feature name. To list them, right-click the part, feature or top-level assembly and click External References; there you can lock them (they stop updating, and you can unlock them later) or break them (they stop updating for good and cannot be restored). Before an assembly leaves your company, lock or break what the recipient should not drive, leave proprietary components out of the Pack and Go package, and keep a dated record of the version you sent.

🔗 For the wider security set-up, read SolidWorks Security Best Practices for Enterprises.

What are external references in SOLIDWORKS?

In SOLIDWORKS you create an external reference when one document depends on another document for its solution: if the referenced document changes, the dependent one changes too. The most common case is top-down design. You edit a part inside an assembly and sketch on, convert or offset the edges of another component; the resulting in-context feature keeps an external reference to that component and updates when it changes. Derived and mirrored parts reference their parent part in the same way.
That is useful while you design, and a source of trouble afterwards. When you save a part with external references, SOLIDWORKS stores the path and an internal ID of the referenced document. Move or rename the original and the reference can no longer be resolved; open the part without its assembly and the reference is out of context. The official External References page in SOLIDWORKS Design Help also lists three rules: a component cannot reference itself, you cannot reference one instance of a part to build a feature on another instance of the same part, and you cannot replace a part with a part derived from it.
“Think of CAD data as the heart of your design business. A single compromised assembly or misplaced file reference exposes your confidential blueprints to risks ranging from collaboration clashes to outright IP theft.” , Dirk-Jan Bonenkamp, Chief Legal Officer, CADChain
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SOLIDWORKS external reference symbols: what ->, ->*, ->x and ->? mean

The state of each external reference is shown by a symbol after the part or feature name in the FeatureManager design tree. Most questions on forums start with one of them, so here they are side by side:
SymbolStateWhat it meansWhat to do
->External referenceThe feature depends on geometry in another file and updates when it changes.Nothing while you design in context.
-> *LockedExisting references do not update and you cannot add new ones to that feature.Unlock to edit again; lock at release or before sharing.
-> xBrokenExisting references do not update and cannot be restored. You can add new references.Only for files that must stand alone for good.
-> ?Out of contextThe referenced document is not open (or not found), so the reference cannot update.Open the assembly that holds the update path, or locate the moved file.
{->}Sketch with referencesThe feature contains a sketch that has external references.Expand the feature to find and manage that sketch.
->{->}BothThe feature has an external reference and contains a sketch with one.Check both the feature and the sketch.
If the x on broken references clutters the tree, SOLIDWORKS can hide it: Tools > Options > System Options > External References, clear Show "x" in feature tree for broken external references. The reference stays broken; only the symbol is hidden.

How to list external references in SOLIDWORKS

  1. For one item, right-click the feature, component, body or part in the FeatureManager design tree. For everything under a subassembly, right-click the subassembly; for the whole model, right-click the assembly name at the top of the tree.
  2. Click External References. The command only appears for items that have external references.
  3. Read the External References dialog box: it lists the components or features that contain external references, and you can sort them by status and isolate selected components.
Listing from the top-level assembly shows every component in its hierarchy that has external references, but not the individual references; list a single item to see each one. For a wider view of how parts, subassemblies and drawings depend on each other, see file management tips for SOLIDWORKS engineers.

How to lock or break external references in SOLIDWORKS

In the same External References dialog box, select the references and click Lock Selected, Unlock Selected or Break Selected, then OK. The difference matters, as the SOLIDWORKS help page on locking and breaking external references explains:
  • Lock freezes the references: they no longer update and you cannot add new ones, but you can unlock them later and carry on. SOLIDWORKS does not update locked references during a rebuild, so the model is not marked out of date.
  • Break is permanent: the references stop updating and cannot be restored. You can add new references, and replace broken sketch relations with ones that do not reference the assembly.
  • Unlock lets you add references or edit existing ones again.
A practical rule: lock in-context features when a design is released, so a later change to a neighbouring part does not silently change it; break only when a part must live on without its assembly, for example as a standard part reused in other products. Frozen features with out-of-date references make SOLIDWORKS prompt you to lock them as well.

How to stop SOLIDWORKS creating external references

If your team or your PDM set-up does not want in-context references at all, switch them off: click No External References on the Assembly toolbar, or go to Tools > Options > System Options > External References and clear Allow creation of references external to the model. Then no in-place mate is created for new components, and Convert Entities, Offset Entities or Up to Vertex on another component do not create references. You can switch it on and off as you work, so only some components get references. This also helps in multi-user projects where other people own the components you design against; see SOLIDWORKS PDM security and vault permissions for the access side.

Why external references matter when you share a SOLIDWORKS assembly

References are not only a rebuild problem. An assembly with live in-context features tells a recipient how its parts were designed against each other, and a package sent with every referenced file can include more than the supplier needs. Three things are worth checking before anything leaves the company:
  • What still updates. Lock or break in-context features in the copy you send, so the supplier's edits to one part cannot drive yours, and so you know exactly which geometry was shared.
  • What goes into the package. Pack and Go gathers parts, assemblies, drawings, references, design tables, decals, appearances and simulation results into a folder or zip file. A zip is a container, not protection: it does not limit who opens the files.
  • What the files reveal. Native parts carry their feature history and design intent. When the supplier only needs the shape, a simplified copy is safer.

Checklist: share a SOLIDWORKS assembly without giving away more than you mean to

  1. List the external references of the top-level assembly and note which in-context features are still live.
  2. Lock or break them in the copy you send: lock when you may need to continue in context later, break when the copy must stand alone.
  3. Suppress proprietary components the supplier should not receive (an internal mechanism, a patented sub-assembly, tooling).
  4. Pack and Go from the File menu and clear Include suppressed components: their files are left out of the package. The Pack and Go dialog box notes that suppressed components still appear in the FeatureManager of the packaged assembly, so rename anything whose name says too much. Review the file list and the drawings, decals and simulation results it includes before you save.
  5. Simplify when the supplier only needs geometry: use the SOLIDWORKS Defeature tool or a STEP copy, and read about neutral CAD format risks first.
  6. Prove what you sent: register a fingerprint and timestamp of the released version, under an NDA. See best practices for sharing CAD files with suppliers.
“European SMEs sharing CAD files are especially vulnerable to IP leaks during collaboration. Implementing locked references ensures tamper-proof design handoffs.” , Violetta Bonenkamp, CEO, CADChain

Common mistakes with SOLIDWORKS external references

MistakeWhat happensBetter
Renaming or moving parts in Windows ExplorerReferences cannot find the original; SOLIDWORKS asks you to locate it, and a wrong file gives rebuild errorsRename and move with Pack and Go or inside SOLIDWORKS PDM
Breaking references "to be safe"They cannot be restored; the part no longer follows design changesLock instead, break only parts that must stand alone
Leaving in-context features live at releaseA later change to a neighbouring part silently changes the released partLock references when the design is released
Sending the whole Pack and Go zipSuppliers get every referenced file, drawing and decalSuppress and exclude proprietary components, review the list
Treating a zip or password as protectionAnyone who opens the package can copy the filesUse PDM permissions, encrypted transfer or DRM, plus a dated ownership record
For the version side of the same problem, see SOLIDWORKS file versioning and tracking, and for teams spread across sites, secure CAD collaboration for distributed engineering teams.

Proof of ownership for multi-file assemblies

Locking references controls what changes; it does not show who designed what, or when. If a shared assembly turns up later in someone else's product, you need dated evidence of each version you had. The BORIS add-in registers a fingerprint (hash) and a timestamp of a file version from inside SOLIDWORKS: tamper-evident proof of authorship. It does not lock, encrypt or hide anything, so it works next to the steps above. See blockchain CAD protection for multi-file assemblies and our guide to CAD file protection for SOLIDWORKS parts, assemblies and drawings. If a supplier needs the live native model, rights management is the layer that travels with the file: compare DRM access control levels for CAD files on CADChain and DRM vs IRM for CAD.
Teams on Autodesk Inventor face the same questions with derived parts and adaptive features: see CAD file dependencies in Autodesk Inventor assemblies.

FAQ on SOLIDWORKS external references

What is an external reference in SOLIDWORKS?

A link that makes one document depend on another for its solution. Most come from in-context features: you build a feature on one part using the geometry of another component in the assembly, and it updates when that component changes. The feature name then shows ->.

How do I find external references in SOLIDWORKS?

Right-click the feature or part, or the assembly name at the top of the FeatureManager design tree, and click External References. The dialog box lists everything with external references and lets you sort by status.

How do I break external references in SOLIDWORKS?

In the External References dialog box, select the references and click Break Selected, then OK. Broken references do not update and cannot be restored, so lock them instead if you might need them again.

What is the difference between locking and breaking external references?

Locked references stop updating and you cannot add new ones, but you can unlock them later. Broken references stop updating for good and cannot be restored, although you can add new references.

What does ->? mean in SOLIDWORKS?

An out-of-context external reference: the document the feature refers to is not open, so the reference cannot update. Open the assembly that holds the update path, or locate the file if it was moved or renamed.

How do I stop SOLIDWORKS from creating external references?

Click No External References on the Assembly toolbar, or clear Allow creation of references external to the model under Tools > Options > System Options > External References.

Does Pack and Go keep external references working?

Pack and Go copies a model with its referenced files into a folder or zip file, so the copy opens with its references in place. It does not lock or protect anything; lock or break references and leave out suppressed components first if the package goes to a third party.

Does locking external references protect my design from copying?

No. Locking only stops geometry from updating. To control who can open or copy files, use PDM permissions, encrypted transfer or DRM; to prove the design is yours, keep a dated fingerprint of each version.