SOLIDWORKS Mate References are a Huge Time Saver when building an assembly

Article by Mehdi Rezaei, CSWE updated January 18, 2018

Article

Imagine you are creating an assembly with many components in it. Each component you insert into the assembly requires three mates. It will be a tedious job making these kinds of assemblies over and over again. Repeating mating process many times in a row. Now, imagine you could drag and drop each component into your assembly, place it close to the right location, and then components snap to their correct spots; and all the mates are added automatically. This is possible using SOLIDWORKS Mate References. In this article, a sample model is used to demonstrate how to use Mate References. The same method could be used for any SOLIDWORKS part file.

How to Run Mate Reference Command

In the following, it is shown that Mate Reference are found under the Features CommandManager tab > Reference Geometry. The mate references have to be added to both the part models that are going to be mated in an assembly environment. The Mate References must share the same names and the same mating items must be selected for both part files.

SOLIDWORKS Mate References

Run Mate Reference Command

Add SOLIDWORKS Mate References to Parts

In this sample case, we have a crank handle and needs to mate a knob and a crank shaft to it. In the following images, adding mate references is shown. For the knob,

  • A round face is selected as the primary reference with Concentric as the mate type. Also, note that due to the location of the secondary mate entity, Anti-Aligned is selected for the primary reference.
  • The secondary mate is a Coincident mate at the bottom face of the knob and the tertiary reference is a parallel mate on the flat face on the pin. Note that the Reference Name is also added.

The same SOLIDWORKS Mate References are added to the crank handle using the same order. Note that the reference name matches the reference name on the knob part file.

With these settings, if the Knob is dragged into an assembly where the crank handle exists, it will snap into place automatically. In these cases, matching names of the reference mates plays an important role. Upon dragging the part into assembly, the mouse pointer does not even have to be very close to the snapping location. In the following images note where mouse pointer is.

Assign Reference Mates for Knob and Crank Handle

Drag the Knob Model into Assembly to Snap in Place

The same steps have been taken for the crank shaft model. In this case, the crank handle file will have two sets of mate references. Note that the mate references are added to the Feature Manager Design Tree in the “MateReferences” folder.

Assign Reference Mates for Crank Shaft and Crank Handle

More than one set of mate references can be added to a part file. Any mate references can be modified by right-clicking on them and selecting Edit Definition.

Drag the Crank Shaft Model into Assembly to Snap in Place

Note: This technique would be very helpful for creating 3D models of PCB’s. You can assign smart references to the 3D models of electronics which will be inserted over and over into various different PCB assembly models.

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Mehdi Rezaei, CSWE

Mehdi is a Certified SOLIDWORKS Expert (CSWE) and works near Vancouver, British Columbia, Canada