Assemblies · Lesson 12
In-context external references
When a part is built in context — a sketch converted from another part, a feature extruded up to another part's face — it stores an external reference to that assembly. SOLIDWORKS marks it with an arrow in the tree and updates the part when the referenced geometry changes. That is powerful, but every reference is a dependency. Know how to read them, lock them when a design is settled, and break them when a part must stand alone.

Where to find it
Right-click a part or feature → List External Refs
Reference symbols
| Symbol | Status |
|---|---|
-> |
External reference, in context |
->* |
Locked — does not update |
->x |
Broken — no longer updates; new references allowed |
->? |
Out of context — the referenced assembly is not open |
{->} |
A sketch inside the feature has an external reference |
From the official FeatureManager tree conventions. Lock and Break are explained in Hawk Ridge's definitions of external references.
Lock vs Break
| Lock | Break | |
|---|---|---|
| Updates | Stop | Stop |
| New references | Not allowed | Allowed |
| Reversible | Yes — Unlock | No |
If referenced files go missing altogether, see missing references.
Step by step
-
1
See the reference
Open the assembly with the lid from the top-down lesson. In the tree, the lid and its feature show -> — an external reference.
-
2
Change the referenced part
Edit the plate and change its length from 100 to 120 mm. Rebuild the assembly (Ctrl + B). The lid grows with it.

The lid follows the plate while its references are active. -
3
List and lock the references
Right-click the lid → List External Refs. The dialog shows each reference and its status. Click Lock All — the symbol becomes ->* and the lid no longer updates.
-
4
Break them if the part must stand alone
Break All removes the references permanently; the lid keeps its current shape and can then be referenced to something new. Breaking cannot be undone.
Common mistakes
- Opening an in-context part on its own and wondering why it does not update — references update only when the assembly is open (out of context is shown as ->?).
- Long chains of parts referencing parts referencing parts. Changes ripple unpredictably and rebuilds slow down.
- Breaking references when locking would do. Locking can be undone; breaking cannot.
Lesson 12 of 16 in the assemblies course.
Practice
Change the plate from 100 to 120 mm long with the lid's references active, then lock them and change the plate back. Check: with references active the lid becomes 36,000 mm³ (120 × 60 × 5); after locking, it stays 36,000 mm³ even when the plate returns to 100 mm.
Sources
- SOLIDWORKS Help 2024 — FeatureManager design tree conventions
- Hawk Ridge — SOLIDWORKS external reference definitions
- CATI — No External References (2018)
- Javelin — Top-down design with a skeleton sketch (Jun 2025)
- Hawk Ridge — SOLIDWORKS external reference definitions
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
What does -> mean in the SOLIDWORKS tree?
+
The item has an external reference. ->* means locked, ->x broken, and ->? out of context — the referenced document is not open.
How do I remove external references?
+
Right-click the part or feature, choose List External Refs, and click Break All. This cannot be undone; Lock All is the reversible option.
How do I stop SOLIDWORKS creating external references?
+
Turn on the No External References option while editing in the assembly. Features then capture positions without linking to other parts.
Are in-context references bad?
+
Not in themselves — they are how top-down design works. But they are resource-heavy in large assemblies and make parts harder to reuse, so use them deliberately and lock them when the design is settled.
Related
- Top-down design in SOLIDWORKSTop-down design in SOLIDWORKS: create a new part inside an assembly, edit it in context, save virtual components, and use layout and skeleton sketches.
- SOLIDWORKS missing references — unable to locate fileSOLIDWORKS "unable to locate file" when opening an assembly or drawing? How the search order works, how to repair references, and how to rename files safely.
- SOLIDWORKS large assembliesHow to work with large assemblies in SOLIDWORKS: Resolved, Lightweight and Large Design Review, Large Assembly Mode and Assembly Visualization.
- SOLIDWORKS Convert EntitiesHow to use Convert Entities in SOLIDWORKS to project model edges and faces into a sketch, plus On Edge, inner loops, Intersection Curve and Silhouette.