This year’s assembly enhancements include innovative new ways to add, edit and control mates, as well as a fantastic new file management time-saver.
Copying Multiple Components
You can now copy several components at once, while preserving all mates between them. Simply select several components while holding Shift or Ctrl, and Ctrl+drag the group to a new location. New instances of the components are created, along with any mates that existed between them. Previously, the only way to do this was by using Copy with Mates, or forming a subassembly, both of which required several steps.
Component Preview Window
With the new Component Preview Window, you can zoom, pan, and orient an individual part – and select faces, edges, or other entities – without changing the orientation of the overall assembly. This is especially useful when mating components in tight spaces, when your view can be obscured, or when selecting very small faces for mating.
To activate the Component Preview Window, click on the part you’ll be mating, and select the Component Preview Window icon from the context toolbar.
The component is then displayed in a separate pane on the right side of the graphics area. Any entities that are selected in the Preview Window are also selected in the main graphics area, meaning that one mate reference can be selected in the main assembly, while the other can be selected from the Component Preview Window. When selecting multiple features between the preview window and the main graphics area, the Quick Mates context toolbar still appears.
Globally Replace Failed Mate References
“If a mate reference is missing from a component that is used in many places in an assembly, you can replace the missing reference for all instances at the same time.”
Before SolidWorks 2016, if a change was made to a component which affected a mate entity, every instance of that component would have to be re-mated. That’s a huge drag when you have a lot of those parts in your designs. Now, however, the first time you edit a broken mate using Replace Mate Entities to re-select an appropriate reference, SolidWorks asks you if you’d like to apply that change to every instance of that broken mate. That can save a huge amount of time and effort.
Make Components Transparent for Mating
In addition to the Component Preview Window above, there’s another enhancement in SolidWorks 2016 which should make mating easier. Under the Options box in the mate PropertyManger, look for the checkbox for “Make first selection transparent” (it’s checked by default). This this option activated, the first part you select for a mate will become temporarily transparent, allowing you to select parts behind it. This one also satisfies an enhancement request on the SolidWorks World Top Ten List from 2014.
Angle and Limit Angle
Distance and Limit Distance
Distance or Percentage along Slot
Distance or Percentage along Width
After activating the Mate Controller from the Insert menu, you can instantly Collect All Supported Mates in your assembly, or choose specific mates manually. You can numerically change the values of any of the supported mates, and watch the assembly update instantly in the graphics area. You can also unlock specific mates to manually drag them in the graphics area.
The mate controller then becomes a feature in the assembly tree below the mates folder, which can be configured and edited. Clicking this feature displays a drop-down menu above the context toolbar (similar to the configuration dropdown) which allows you to choose between your saved positions.
Quick Mates Improvements
The Quick Mates context toolbar – which appears when Ctrl+selecting multiple parts in an assembly – now supports even more mate types, including:
- Profile Center
Mirror Assembly Features
You can now mirror an assembly feature, just as you would a regular part feature in a part. This mirror command is found under the Assembly Features drop-down menu on the Assembly tab. This enhancement satisfies a request on the SolidWorks World Top Ten List from all the way back in 2007!
AssemblyXpert has been renamed to Performance Evaluation, and has been expanded to support drawings. Read more about the new functionality when we discuss drawing improvements in Chapter 10.
Open Component Drop-Down Menu
In SolidWorks 2016, when you click on a part in the graphics area which is contained within a subassembly, the “Open Part” button on the context toolbar will include a flyout menu. Clicking this button will allow you to open any subassembly which contains the selected part. To quickly open the part itself, simply click the folder icon.
Renaming Components in the FeatureManager Design Tree
My favorite assembly enhancement this year is the ability to rename components directly from within the SolidWorks FeatureManager tree. In my experience, nearly every part I create in a production environment gets renamed at least once (such as adding a part number, changing a descriptive name, etc.)
In the past, this generally involved going through Windows Explorer, and either changing the name manually (and dealing with the broken references that popped up later) or using the SolidWorks Rename tool (which may people are unaware of).
In 2016, you can avoid Windows Explorer entirely, and update component names directly from the FeatureManager design tree, while also updating any references in other documents. Renaming components in an assembly works exactly the same way as renaming features in a part. You can do any of the following:
- Click-pause-click the component.
- Right-click the component and select Rename Assembly or Rename Part.
- Select the component and press F2.
Then simply type a new name and press Enter. The file name of the component changes in memory, and all currently open documents that reference the component are updated to reference the new name.
The next time you save the assembly, SolidWorks will ask you if you’d also like to update references to any documents, which were not open when the component was renamed. When the Rename Documents dialog box appears, select Update where used references, and click OK.
This feature was first requested in the SolidWorks World 2007 Top Ten List.
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