Assemblies · Lesson 3
SOLIDWORKS advanced mates
Advanced mates handle positions the standard mates cannot express simply: centring a tab in a slot (Width), keeping two parts mirror images (Symmetric), centring one profile on another (Profile Center), moving along a curve (Path), coupling two motions (Linear/Linear Coupler) and allowing movement only within a range (limit mates).

Where to find it
Mate PropertyManager → Advanced tab
Advanced mates
| Mate | What it does |
|---|---|
| Profile Center (2015+) | Centres circular or rectangular profiles on each other |
| Symmetric | Keeps two entities mirrored about a plane — doors, jaws |
| Width | Centres a tab in a slot; Centered, Free, Dimension or Percent |
| Path | A point follows a curve; pitch/yaw and roll control |
| Linear/Linear Coupler | Couples translation of two parts by a ratio |
| Distance / Angle limit | Allows motion between a minimum and a maximum |
Limit values can be used in equations and design tables. Since 2020 Slot, Profile Center, Width and limit mates are also on the Quick Mates toolbar. Next: motion-driven mechanical mates.
Practise it: limit distance in the bench vise and limit angle in the robot arm.
Step by step
-
1
Build a slot and a tab
Make a base part — a 60 × 40 × 20 mm block with a 30 mm wide slot cut across its top, 10 mm deep — and a tab part, a 10 × 40 × 20 mm block. Insert both into an assembly, base fixed.
-
2
Add a Width mate
Mate → Advanced → Width. Select the mate type first. Width selections: the two side faces of the slot. Tab selections: the two side faces of the tab. Keep Centered.

Width mate — two slot faces, two tab faces, centred. -
3
Finish positioning
Add a coincident mate between the bottom of the tab and the slot floor. The tab can now only slide along the slot.
-
4
Limit the travel
Add a Distance limit mate between the tab's end face and the base's end face with a minimum of 0 and a maximum of 20 mm, then drag the tab to see the range.
Common mistakes
- Selecting faces before choosing Width — for Width, pick the mate type first, then the four faces.
- Expecting a Symmetric mate to stop motion. It keeps two parts mirrored about a plane but does not lock them.
- Too many limit mates fighting each other; use one limit per motion.
Lesson 3 of 16 in the assemblies course.
Practice
Centre the 10 mm tab in the 30 mm slot with a Width mate. Check: measure from each tab face to the nearest slot wall — both gaps are 10 mm.
Sources
- SolidProfessor — Advanced assembly mates (2019)
- GoEngineer — Introduction to SOLIDWORKS mates (Feb 2022)
- Hawk Ridge — 3 ways to mate in assemblies
- SolidProfessor — SOLIDWORKS 2015 assemblies
- CATI — Quick Mates enhancements (2020)
- SOLIDWORKS blog — New assembly productivity tools in 2021
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
What is a Width mate?
+
A mate that centres a tab between two faces of a groove or slot. It needs four selections: two width faces and two tab faces, with options Centered, Free, Dimension or Percent.
What is a Profile Center mate?
+
A mate, added in SOLIDWORKS 2015, that centres rectangular or circular profiles on each other in one step, with offset, flip and lock rotation options.
How do I limit how far a part can move?
+
Use a Distance or Angle limit mate with minimum and maximum values. The component can move only within that range.
What does a Path mate do?
+
It makes a point on a component follow a curve, edge or sketch path, with options to control pitch, yaw and roll.
Related
- SOLIDWORKS standard matesHow to use SOLIDWORKS standard mates: coincident, parallel, perpendicular, tangent, concentric, lock, distance and angle, Quick Mates and lock rotation.
- SOLIDWORKS mechanical matesHow to use SOLIDWORKS mechanical mates: Cam, Slot, Hinge, Gear, Rack and Pinion, Screw and Universal Joint, with ratios and how they simulate mechanisms.
- 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 mate errors — over defined and failed matesFix SOLIDWORKS mate errors: over defined components, mates not satisfied, conflicting mates and fixed parts, using MateXpert and the Mates folder.