SOLIDWORKS Mate Reference - Peg and Hole

By David Brown

SOLIDWORKS has a host of powerful automation tools that can boost your productivity, save time, and improve efficiency. One of these is the Mate Reference tool located on the Features Command Manager under the drop down menu below the Reference Geometry button.

For this example, (see the image below), I am going to add a mate reference to a part that I have created and placed in a folder that is linked in my Design Library named Cap. This Mate Reference will allow me to select the part from my design Library and when I drag and drop it on to the end of the legs of the frame in my assembly, the appropriate coincident and concentric mates will be added automatically.

With the part open in its own window, I select the inner circular edge then select the Mate Reference command from the Command Manager. This places the Edge in the Primary Reference Entity box on the property manager of the Mate Reference tool. As you can see, you are able to add a Secondary and a Tertiary reference as well as select a mate type and alignment condition for each. This enables you to build a complex arrangement of mating conditions that will be automatically placed when the part is dragged and dropped from the Design Library. A Peg and Hole mate condition is based on the edge that borders a cylindrical face and a planar face. In this example we will use the circular edge on the inside of the Cap. The inner diameter cylindrical face shares this edge with the bottom planar face on the inside of the cap. Once the edge is selected I finish the command by clicking the Green Checkmark. The default settings are okay and no other settings or Reference Entities need to be used. As you can see in the image below, a folder has been added to the top of the Feature Manager Design Tree which contains the Mate Reference Feature. You can make changes to this feature by right clicking on it and selecting Edit Definition.

Once the Mate Reference is added to the part, I save the changes and close it. Now, when I select the Cap part from the Design Library folder and drag and drop it onto the end one of the legs, the Cap snaps into position and the coincident and concentric mates are added automatically. I can continue placing them on the ends of the other legs simply by moving the mouse over the ends of the tubes and clicking to place. When all the ends are covered I select the Red X on the Insert Components property manager or the Green Check with the Right Mouse Button to stop placing caps in the assembly.

Having parts in your Design Library with Mate References in them will greatly improve your assembly time by automating the sometimes laborious task of mating components.

A video that demonstrates the techniques in this blog can be found here.