Hide Table of Contents

Mate PropertyManager - Analysis Tab

You can assign mate properties for use in SolidWorks Motion and SolidWorks Simulation analysis. (You can add the properties without having SolidWorks Motion or SolidWorks Simulation added in.)

To add analysis properties to mates:

  1. Pre-select a mate:

    • Existing mates: Right-click the mate in the FeatureManager design tree and select Edit Feature .

    • New Mates: Define in the Mate PropertyManager.

  2. In the PropertyManager, on the Mates tab, select a mate in Mates.

  3. On the Analysis tab, select the properties to add, and then set options as described below.

  4. Click .


Mate Location . Overrides the default mate location with the point you select. The mate location point determines how parts move in relation to each other. The mate location is always a point. If you select another type of entity such as a face for the mate location, the mate location is at the center of the selected entity.

Treat interference as a shrink/press fit. Treats mates that force interference as a shrink fit in SolidWorks Simulation.

Load Bearing Faces

You can associate additional faces with a mate to define which faces share in bearing the load. (Not available for Symmetric, Width, Path, or Cam mates.) Example

Load-bearing Faces/Edges . In the graphics area, select faces from any component referenced by the mate.

Isolate components. Click to display only the components referenced by the mate. Click Exit Isolate (Isolate pop-up toolbar) to return the display to its original state.


You can associate friction properties with some types of mates. (See mate types under Joint dimensions below.)

Parameters. Select how to define the friction properties of the mate:

  • Specify materials. Select the materials of the components from lists and .

  • Specify coefficient. Specify Dynamic Friction Coefficient by typing a number or moving the slider between Slippery and Sticky.

Joint dimensions. Available dimensions vary depending on geometry and mate type.



Mate Types


  • Coincident mate between any two vertices, sketch points, or reference points

  • Concentric mate between two spherical faces


  • Concentric mate between two cylindrical faces

  • Coincident mate between two linear entities (edges, axes, temporary axes, sketch lines)


Coincident mate between two planar faces


Coincident mate between two planar faces

Universal Joint

Universal Joint mate


You can associate bushing properties with a mate. Bushing properties make a mate somewhat flexible by giving it spring and damper characteristics. Mates with bushing properties can produce a more realistic distribution of forces in SolidWorks Motion analyses. In SolidWorks Help, see Motion Studies, Motion Analysis, Bushing.


Isotropic. Select to apply uniform translational properties. Clear to specify different properties in each direction. For example, a bushing mount for a suspension arm has different properties in Z-axis than in the X-axis or Y-axis.

Stiffness. Enter the translational stiffness coefficient.

Damping. Enter the translational damping coefficient.

Force. Enter the preload applied.


Isotropic. Select to apply uniform torsional properties. Clear to specify different properties in each direction. For example, a bushing mount for a suspension arm has different properties in Z-axis than in the X-axis or Y-axis.

Stiffness. Enter the torsional stiffness coefficient.

Damping. Enter the torsional damping coefficient.

Torque. Enter the preload applied.


Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Mate PropertyManager - Analysis Tab
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: SOLIDWORKS 2011 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.