Assemblies · Lesson 11
Top-down design in SOLIDWORKS
In bottom-up design you model parts first and assemble them. In top-down design you create parts inside the assembly, referencing the parts around them — a lid that fits a box, a gasket that matches a flange. The new part follows when the neighbouring part changes. Layout and skeleton sketches take the idea further: one sketch in the assembly drives the sizes of many parts.

Where to find it
Assembly tab → Insert Components flyout → New Part
Top-down tools
| Tool | Use |
|---|---|
| Insert Components → New Part | A new virtual part placed on a face or plane |
| Edit Part / Edit Component | Edit an existing part in the context of the assembly |
| Save Part (in External File) | Turn a virtual part into a normal part file |
| Make Virtual | Turn a part into a virtual one, cutting the link to its file |
| Layout (Insert → Layout) | A layout sketch in the assembly, often with blocks |
| Skeleton / master part | A part of sketches that drives the others; insert as an envelope to keep it out of the BOM |
Top-down design creates in-context references — the next lesson explains how to read, lock and break them.
Step by step
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1
Insert a new part
In an assembly that contains the 100 × 60 × 10 mm plate, choose Insert Components → New Part and click the plate's top face. A new part is created, shown in brackets (virtual), and a sketch opens on that face.
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2
Sketch in context
Select the top face and click Convert Entities — the plate outline is copied into the new part's sketch, linked to the plate.

Convert Entities copies the plate outline into the new part, linked to it. -
3
Build the lid
Extrude the sketch 5 mm upward and exit editing (click the Edit Component button or the confirmation corner). The lid matches the plate.
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4
Save it externally
Right-click the new part → Save Part (in External File). Until you do, the part lives only inside the assembly file.
Common mistakes
- Leaving parts virtual and then copying the assembly file — the parts go with it, but they cannot be reused elsewhere until saved externally.
- Referencing many parts in context. Every reference is a dependency; large in-context assemblies get slow and fragile.
- Forgetting you are editing a part in context — exit the edit before doing assembly work.
Lesson 11 of 16 in the assemblies course.
Practice
Create the 5 mm lid in context on the 100 × 60 mm plate. Check: the lid's volume is 30,000 mm³. In the next lesson you change the plate and watch the lid follow.
Sources
- Javelin — Create a new part in an assembly (Jan 2023)
- TriMech — What engineers should know about virtual components
- Javelin — How to create a virtual subassembly (Nov 2025)
- SOLIDWORKS Tech Blog — Using assembly layout sketches (2015)
- GoEngineer — Ultimate guide to SOLIDWORKS blocks (Feb 2024)
- Javelin — Top-down design with a skeleton sketch (Jun 2025)
- GoEngineer — Convert Entities quick tips
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
What is top-down design in SOLIDWORKS?
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Creating or editing parts inside the assembly so they reference other components. The parts update when the components they reference change.
What is a virtual component?
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A part or subassembly saved inside the assembly file rather than as its own file. Its name is shown in brackets. Save it externally to reuse it.
What is a layout sketch?
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A sketch in the assembly, usually made of blocks, that defines the positions and sizes of components. Parts built from it update when the layout changes.
What is a skeleton part?
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A part containing only sketches and reference geometry that drives the other parts. Inserted as an envelope, it stays out of the BOM.
Related
- In-context external referencesHow SOLIDWORKS in-context references work: the -> symbols, List External Refs, locking and breaking references, and when they slow assemblies down.
- SOLIDWORKS subassembliesHow to create subassemblies in SOLIDWORKS from selected components, save virtual ones, make them flexible or dissolve them, and why they speed things up.
- 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.
- SOLIDWORKS multibody partsWhat multibody parts are in SOLIDWORKS, how Merge result and Feature Scope work, Save Bodies to make an assembly, and when an assembly is better.