As SOLIDWORKS users, we inevitably spend a lot of time creating mates to hold our assembly components together and dictate how the motion in an assembly will work. Many of the components may be unique to the project you are working on at that time; however most designs do contain some number of standard components, as well. A “standard component” would be a part or sub-assembly that is commonly used in many different projects.
The SOLIDWORKS Toolbox (available in SOLIDWORKS Professional and Premium) contains an entire library of standard components like fasteners, retaining rings and bearings. One benefit to using SOLIDWORKS Toolbox components is that they come with built-in mate references that make mating a toolbox item in an assembly quick, easy, and automatic. For example, all you need to do with a fastener is drag and drop it onto a hole and SOLIDWORKS will automatically create the coincident and concentric mates necessary to hold that fastener in place. Ever wonder what magic is bestowed upon the toolbox components in order to make this possible? The answer lies in the power of Mate References.
Create Mate References
A mate reference tells SOLIDWORKS which geometry in a component will be used to hold that component in place and how. This is often accomplished with a coincident or concentric mate (although parallel and tangent mates are also available). Mate references are intended to be simple, given that they are utilized with a drag-and-drop action, so the more advanced mates, such as the Width mate, cannot be defined in this way.
There are two levels of sophistication with a mate reference. The simpler type of mate reference exists on only one component and (in most cases) only creates one mate. The component can then be mated to any matching geometry on another part within the assembly. Here are the steps to creating and utilizing this type of mate reference
- With the component open in SOLIDWORKS, access the Mate Reference manager in the Reference Geometry dropdown or by going to Insert > Reference Geometry > Mate Reference.
- While the Mate Reference dialog is active, select some geometry on the component that you want automatically mated when it is dropped onto the corresponding geometry in the assembly. This will work best with a planar or cylindrical face. This geometry should populate the blue selection field in the Primary Reference Entity Then you can choose which type of mate you desire (concentric, for example) and how you would like the alignment to turn out.And that’s it!
Also the alignment can be adjusted while the component is being inserted, so don’t stress out about this too much.
Check Your Mate
Now to test your mate reference, insert the component into the assembly. As stated before, this can be done by dragging and dropping the component from the Design Library (in the task pane), a separate Windows Explorer window, or even another SOLIDWORKS window. You can even use the Insert component dialog.
Either way, when you hold the component over any geometry that would be appropriate to match your mate reference (ie: a cylindrical face for a concentric mate), VOILA! Your component will automatically reposition itself to satisfy this mate!
As you move your mouse around the screen to hover over different “matching” types of geometries, the component will continue to realign itself. To flip the alignment of the component, tap the Tab key. When you like the position of the component, simply release your mouse button to place it (or click if using the Insert Component command). Check your mates list to find your new automatically created mate!
Pro Tip #1: To create a coincident AND concentric mate at the same time using this method, instead of selecting a flat or cylindrical face for the mate reference, select the round edge where a flat and cylindrical face meet and then select “Default” as the mate reference type – this is the type of mate reference used for toolbox fasteners.
Set Advanced Mate References
The more sophisticated type of mate reference takes a little more set up, but can create up to 3 mates at a time very easily when used. This type of mate reference is best for occasions when you find yourself mating the same two components together with the same exact mates, time and again. Instead of repeating this mundane activity for the rest of eternity, you can set up this mate reference so that when you simply drop one component onto the other in an assembly, they snap together in the correct orientation with the correct mates immediately.
The same basic steps are applied to setting up mate references, but there are two main differences:
- A mate reference needs to be created in both components that are to be mated together. The names of these mate references also need to match exactly. This is imperative for the mate reference to work. You can easily assign a name in the Reference Name field within the Mate Reference dialog.
- Multiple reference entities can now be chosen to create multiple mates, so you can designate that a coincident, concentric and parallel mate all be added at the same time as the primary, secondary and tertiary entities. These reference entities must be assigned in the same order for both definitions of the mate reference in corresponding parts. This is also imperative for the mate reference to work.
And just like that, once the matching mate references have been created for both components, all you need to do is insert one into an assembly where the other component already exists. Before dropping it into the assembly, hover the new component over the other component and they will quickly snap together. You can then place the component down with the mates automatically built for you!
Pro Tip #2: Did you forget about your mate references and already place both components in the assembly? No worries, just hold your Alt key and drag one component on top of the other and the mate references will be activated!
You are now ready to build a library of commonly used components that snap in place with a simple drag-and-drop – no assembly required!
For more information on how to get the most out of Toolbox components, watch our On-Demand Webinar “SOLIDWORKS Toolbox Do’s and Don’ts”