Last week, I spoke briefly about the benefits of using the Design library in Why Do I Need to Use the Design Library? . As promised, this week I will show you my favorite way of using the Design Library. Adding frequently used components, with Mate References, to the Design Library allows you to build assemblies faster then you ever imagined. The steps illustrated today may seem like a lot but a few extra minutes when setting up your library components can save you hours in the long run.

What is a Mate Reference?

Mate references are a huge time saver. Mate references allow you to designate different features of a component to automatically mate when inserting the component into an assembly. As you will see here today, when you drag a component that has mate references into an assembly it will automatically mate to other components with mate references of the same name and type. Something to note, if the component being inserted into an assembly finds the same mate reference name but the mate types do not match up, the mate will not be created.

Adding Mate References to Components

Adding a Mate Reference is extremely easy. In the Shortcut bar, select Mate Reference from the Reference Geometry flyout. You can also select Insert -> Reference Geometry -> Mate Reference.

In the Mate Reference PropertyManager, you must first name the reference. This is crucial since the Reference Name is first thing SolidWorks evaluates when inserting a component with mate references into an assembly. Mates are made based on the reference names in an assembly. For this example, the name of the Mate Reference will be Plate.

Every Mate Reference must have at least one Reference Entity designated. While still in the Mate Reference PropertyManager; select a face, edge, vertex or plane that makes up the Primary Reference Entity.

Next, select the Mate Type for the selected entity. For this particular part we want the selected face to use the Concentric mate when we insert the component into the assembly. Next the Mate References Alignment can be selected from the options of: Any, Aligned, Anti-Aligned or Closest.

For this particular component we wish to specify a Secondary and Tertiary Reference Entity, since we want the component mates to be fully defined on insertion into the assembly. Using the same methods as describe above, select the mating face for the flange of the linear bearing.

This face will Coincident when inserted in the assembly.

Lastly, we will designate one of the screw holes to be Concentric with a corresponding threaded hole in the assembly. This last mate will create a fully defined component that will not be able to move.

Make sure to select Concentric for this Tertiary Reference Entity.

Click the green check mark and you will see that the newly created Mate Reference is shown in the MateReferences folder in the FeatureManager.

Using the same methods, we can create more Mate References to be used with other components in an assembly. Each created Mate Reference will also be shown in the MateReferences folder in the FeatureManager.

Adding Components to the Design Library

Now that we have added Mate References to our component, we can add the component to the Design Library to be accessible for future uses. As I mentioned last week, the Design Library is nothing more then a folder structure on you hard drive or a shared drive on a network. You can add components to the Design Library by adding it to the appropriate folder with Save as or using Windows Explorer. Sometimes it is a pain in the ass to find the folder you need, especially if you do not know where the Design Library is located. To make things easier, SolidWorks has the ability to add a component to the Design Library from within the Design Library interface. With the component open, select the Add to Library button in the Design Library. You can also add to library by:

• Right-clicking the component or feature in FeatureManager and selecting Add to Library.
• Drag the item from the graphics area directly into the lower pane of the Design Library.
• Drag a feature or component from the FeatureManager directly into the lower pane of the Design Library.

In the Add to Library PropertyManager, select the Feature, Sketch, Block, Part or Assembly to be added to the Design Library. Note that you can select multiple features or sketches but you can only select one block, part or assembly at a time.

In the Save To section of the Add to Library PropertyManager, enter the File name of the component that will be displayed in the lower pane of the Design Library. Then select the folder location in the Design Library folder section.

In the Options section of the Add to Library PropertyManager you can select the File Type of the selected item. In this case, we will accept the default file type shown. In the Description field enter the item description that will be displayed in the tooltip in the Design Library. Here you can add more information that you would not normally include in the file name.

Once all the options have been selected properly in the Add to Library PropertyManager, click the green check mark to add the component. The added component is now available for use and is shown in the lower pane of the Design Library when the appropriate folder is selected.

To Be Continued…

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