Mate references within SolidWorks are used to quickly align and add Mates to define a component automatically during the drag and drop process.
Creating a Mate Reference
The mate reference command in SolidWorks is found under Reference Geometry on either the Features toolbar or under the Insert menu dropdown.
Mate Reference Features
When creating the mate reference the first field is Reference Name. Define a name that will be common for this type of attachment. For example, the files shown for this tip are a terminal block and DIN rail that will be mated and used inside of a control panel so the mate reference is named DINRail. While this is not required it becomes beneficial when using multiple mate references later on.
Starting with the terminal block the reference name is set to DINRail. Next we choose the model geometry to use for the mating surfaces. Selecting the faces of the block’s feet that will lock to the DIN rail the primary reference entity and the secondary reference entity are chosen. The tertiary is not required for this component but can be used as a third mate when required.
Now that the mate entities have been defined there are options under each that can be used to define the Mate Reference Type and Mate Reference Alignment for each selection. These are both smart dropdowns that will filter based on the type of surface selected. Notice in the menu shown below only selections that can be used with a planar face are available.
For the primary reference that will mate the top face of the clip notch to the top face of the DIN rail the mate type is set to Coincident.
Next the alignment of the mate is set to one of the four options shown below. While the Any option works for many parts it can be set to align the parts the same way each time which can save frustration in the future. For this component it is set to Anti-Aligned so that the terminal block will lock to the rail correctly.
The same menus are available for the secondary reference
and are set as shown below.
When these are set and confirmed the new mate reference feature is created and can be found in the Mate References folder in the SolidWorks feature tree.
Now the matching feature can be created for the model of the rail.
The matching faces to be used for the terminal block’s mate are selected and set to the options shown below in the same method as the terminal block. Since the alignment is set using the selections in the block the Mate Reference Alignment is left on the Any selection. This will allow other block models used for the control panel to be aligned as needed using the same reference without changing settings in the rail part file that could cause issues with previously created blocks.
Now that both components have been setup they can be tested in a sub-assembly file. The rail is inserted first as the main component in this sub-assembly since it will be the component mated inside the control panel itself. Then the terminal block is dragged over from the library to the rail. The terminal block snaps into position as shown and there is another information dialog shown in the view that allows the component to be rotated if needed using tab. For our component it drops in perfectly to the rail without rotation.
With the part in place now we can expand the Mates folder and see that two new coincident mates have been added automatically to the assembly.
While using mate references in SolidWorks is relatively straight forward in can get more complicated when using multiple mate reference definitions in the same part. Especially for entities that are close together. These types of components will be covered in a future posting along with mating sub-assemblies using mate references.