SOLIDWORKS assembly delighters for everyday use!

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Since assembly modelling in SOLIDWORKS is one of the daily tasks of an engineer, I want to share some handy tricks to simplify the workflow of this task. The main focus in this tech blog will be the creation of mates.

1. Adding mates from the Quick Mates Context Toolbar

Tired of opening the Mate PropertyManager for every mate definition? The Quick mates context toolbar is here to help! First of all, be sure that the Quick Mates functionality is active in SOLIDWORKS. Go to Tools > Customize. On the Toolbars tab, under Context toolbar settings, select Show quick mates.

The Quick Mates context toolbar appears when you Ctrl + select mate entities.

  • For model geometry (such as faces, edges, and vertices), you select in the graphics area.
  • For reference geometry (such as planes, axes, and points), you can select in the graphics area or in the FeatureManager design tree.

Supported mate types include all standard mates, plus some advanced mates (Profile Center, Symmetric and Width) and some mechanical mates (Cam and Slot). Only mates that are appropriate for your selections are available on the Quick Mates context toolbar.

When you select a mate in the Quick Mates context toolbar, the mate is directly applied and the toolbar closes. For some mates, such as Distance, Angle, and Profile Center, the toolbar expands. Enter the mate specification (such as distance) and click.

2. Previewing a Mate Component in the Component Preview Window

Probably the following scenario is also recognizable for a lot of users. You mate a component in an assembly and after clicking OK, you see the component move into the assembly, making it invisible. The Component Preview Window can provide an easy solution for this behaviour. When you view a component in the Component Preview Window, you can zoom and rotate the view of the component independently from the rest of the assembly. This solves the issue of losing a component out of sight.

To preview a mate component:

  1. Select the component you want to view in the Component Preview Window.
  2. The context toolbar appears next to your cursor. Here you can select Component Preview Window .
  3. The screen splits, the Component Preview Window opens on the right side and displays the selected component.|
  4. The component becomes transparent in the main window. Now you can select a face of the component in the Component Preview Window and use Mate to position it. (Use Ctrl selection of the first tip in this tech blog!)
  5. Click Exit Preview to close the Component Preview Window.


3. Quickly find a Mate with the Selection Breadcrumbs

When an assembly grows, the number of mates will also grow. At a certain point it will be challenging to find that particular mate you want to change. To help you with this, you can use the Selection Breadcrumbs, so you can review the mates of a selected component directly in the graphics area.

First of all, be sure that the Breadcrumbs functionality is active in SOLIDWORKS. Go to Tools > Options > System Options > Display. Select Show breadcrumbs on selection.

By default, the Breadcrumbs appear in the upper left corner of the graphics area when you select:

  • An entity in the graphics area.
  • A node in the FeatureManager design tree.

To move Breadcrumbs to the cursor location, press D. D is the default keyboard shortcut to move the selection breadcrumbs to the cursor. To assign a different key to move the controls: Go to Tools > Customize. On the Keyboard tab, search for Move Selection Breadcrumbs and type an unused key to assign it.

When you hover over the items in the Breadcrumbs, it displays the mate information of the part, the body or the feature selected. This is useful, because a part can still contain a lot of mates, but when you select the feature, it will only show the mates connected to this feature.

Conclusion

Hopefully these tips will help you to gain some time and speed up your workflow during daily tasks, like assembly modelling.

Written by Martijn Visser, Elite Application Engineer, CAD2M

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