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.

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
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1
Open the pin part
Open the pin part (Ø10 × 30 mm) on its own.
-
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.

Primary — concentric on the cylinder; secondary — coincident on the end face. -
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
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
- TriMech — No assembly required: mate references
- Javelin — SOLIDWORKS mate references (2018)
- SOLIDWORKS Tech Blog — Magnetic mates in 2017
- GoEngineer — Magnetic mates explained (Apr 2023)
- Javelin — The magnetic mate in assemblies (Nov 2022)
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?
+
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.
Related
- SOLIDWORKS SmartMates and Smart FastenersHow to use SmartMates in SOLIDWORKS: Alt-drag components to mate them instantly, which mates edges, faces and holes create, and Smart Fasteners.
- SOLIDWORKS standard matesHow to use SOLIDWORKS standard mates: coincident, parallel, perpendicular, tangent, concentric, lock, distance and angle, Quick Mates and lock rotation.
- SOLIDWORKS Design LibraryHow to use the SOLIDWORKS Design Library: default folders, adding your own folders, saving reusable library features (.sldlfp) and inserting them.
- Toolbox fasteners in assembliesHow to add bolts, nuts and washers to SOLIDWORKS assemblies with Toolbox: drag onto holes, change sizes, Smart Fasteners and configuration settings.