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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.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Lid part being created inside an assembly on top of a base part, with in-context reference arrows

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

  1. 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.

  2. 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.

    New part sketch on the plate's top face with the outline converted from the plate
    Convert Entities copies the plate outline into the new part, linked to it.
  3. 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.

  4. 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

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.