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SOLID WORKS ClubSOLID WORKS Club

Assemblies · Lesson 6

Mate references and magnetic mates

A mate reference stores, inside a part, which faces or edges it should mate with and how. When you insert the part into an assembly next to a matching reference, it snaps into place with the mates already added. Use it for parts you place again and again — fasteners, standard components, motors. Magnetic mates, added in 2017, do something similar for layouts: parts snap together at published connection points.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Part snapping into position using mate references and conveyor sections snapping with magnetic mates

Where to find it

Part: Insert → Reference Geometry → Mate Reference; Tools → Asset Publisher

Mate references at a glance

Item Detail
Create Insert → Reference Geometry → Mate Reference
References Primary, secondary, tertiary — each with a mate type
Types Concentric, coincident, parallel, tangent, Default (Toolbox) — not Width
Matching Same name and order in both parts
Works when Inserting from the Design Library, File Explorer, another window or Insert Components
Stored MateReferences folder in the part; several sets per part

Magnetic mates (2017+)

Step Detail
Publish Tools → Asset Publisher in the part: ground plane and connection points
Connection point Linear edge = midpoint; circular edge = centre
In the assembly Turn magnetic mates on in the Tools menu; purple dots show connections; add a ground plane
Control [ and ] cycle connection points; right-click → Lock Magnetic Mate

Mate-referenced parts are ideal for the Design Library.

Step by step

  1. 1

    Open the pin part

    Open the pin part (Ø10 × 30 mm) on its own.

  2. 2

    Create the mate reference

    Insert → Reference Geometry → Mate Reference. Name it pin-hole. Primary reference: the cylindrical face, type Concentric. Secondary reference: the end face, type Coincident.

    Mate Reference PropertyManager with primary concentric and secondary coincident references on a pin
    Primary — concentric on the cylinder; secondary — coincident on the end face.
  3. 3

    Add the matching reference to the plate

    In the plate part create a mate reference with the same name and the same order: the hole face (concentric), then the bottom face (coincident).

  4. 4

    Insert and watch it snap

    In the assembly insert the pin and move it near a hole — it previews in position. Click to drop it; the mates are created automatically.

Common mistakes

  • Different names or a different order of references in the two parts — they will not match.
  • Using Width as a mate reference type — it is not allowed.
  • Expecting existing components to snap when dragged normally — use Alt-drag (SmartMates) for components already in the assembly.

Lesson 6 of 16 in the assemblies course.

Practice

Add matching pin-hole mate references to the pin and the plate. Check: inserting the pin near a hole adds concentric and coincident mates without opening the Mate dialog, and the pin sits 20 mm proud of the plate as before.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

What is a mate reference in SOLIDWORKS?

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A feature in a part that stores up to three reference entities and mate types. When the part is inserted near a matching reference, the mates are created automatically.

How do mate references match?

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By name and order: both parts need a mate reference with the same name, and their primary, secondary and tertiary references in the same order.

What are magnetic mates?

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A feature added in SOLIDWORKS 2017: parts published with Asset Publisher have connection points and a ground plane, and snap together when dragged near each other. Useful for layouts such as conveyors.

Do Toolbox parts have mate references?

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Yes, Toolbox parts use a Default mate reference so they snap onto holes when inserted.