3 Ways to Mate in SOLIDWORKS Assemblies

3 Ways to Mate in SOLIDWORKS Assemblies

Table of Contents

So, you’ve successfully learned how to build your part and now you’re ready to create your first assembly. Congratulations!

Once you’ve inserted your components (via “Insert Components”, dragging and dropping, etc), let’s move on to mating. One of the great benefits of SOLIDWORKS is that there are multiple ways to accomplish the same result, and that also goes for mating!

We’ll discuss how we can use the Mates menu, Quick Mates, and SmartMates to get you up and running.

1. Mates Menu

The first way we learn to mate is with the Mate icon (it resembles a paper clip) in the Assembly menu, on the CommandManager.

The Mate icon is next to the Insert Components icon.

Once you’ve selected the Mate feature, you can select the first entity to mate. It also may turn transparent, if ‘Make first selection transparent’ is turned on the very bottom.

Select the Make first selection transparent option after selecting the Mate feature.

Next, select the second entity you want to mate to. Based on the selections, SOLIDWORKS will guess which mate you’re trying to create. If it’s the correct one, press the green check to accept it; if it isn’t, select the mate you’re looking for and accept it.

TIP: Use the Alt key to temporarily hide a face when you need to select through it.

This is the Mate toolbar in SOLIDWORKS.

In some instances, certain mates will require you to select the mate first, before selecting the entities to mate, such as the Width mate under the Advanced Mates.

2. Quick Mates

Another way is to pre-select the faces you’re creating a mate for, without having to be in the Mate menu. Simply hold down Ctrl and select the two entities you wish to mate.

Pre-select the faces to Quick Mate by holding down Ctrl and selecting entities.

The supported mate types are all standard mates (Concentric, Coincident, Equal, etc), as well as some advanced mates (Profile Center, Symmetric, and Width) and some mechanical mates (Cam and Slot).

3. SmartMates

If you prefer to drag your components together and have them magically snap into place, SmartMates is probably more up your alley.

In this scenario, we’ll create a ‘peg-in-hole’ SmartMate, which will result in a concentric and coincident mate.

To create it, hold down the Alt key, and left-click and drag the circular edge to the edge you want to mate it to. If successful, you’ll see this icon:

This is the mate SOLIDWORKS icon when SmartMates is activated.

TIP: It’s easier when you can see what you’re dragging and what you’re dragging it to, in the same view.

A red knob is selected to demonstrate how much easier it is to see where you are mating the objects.

2 Options If Your Part Flips

If the part flips on you, there are two options to fix it:

1. If you have let go of your left mouse button (release the part), click the Tab key to flip the orientation.
2. If you haven’t released your left mouse button, right-click on one of the mates that’s created and select Flip Mate Alignment.

A red knob is upside-down and needs to be flipped.

A red knob was upside down and is not right side up.

This is the mouse right-click menu option where Flip Mate Alignment is located.

Here’s a breakdown of different types of mates that can be created when using SmartMates:

Pointer Mating Entities Type of Mate
2 linear edges, or 2 temporary axes Coincident
2 planar faces Coincident
2 vertices Coincident
2 conical faces, or 1 conical face and 1 temporary axis Concentric
2 circular edges (peg-in-hole SmartMates). The edge do not have to be complete circles. Concentric (conical faces)and Coincident (adjacent planar faces)
2 circular patterns on flanges (flange SmartMates) Concentric and coincident
Origins and coordinate systems Coincident

Lastly, if you want to control the speed that SOLIDWORKS applies the SmartMate, that can be done in the System Options > Performance > SmartMate Sensitivity. Dragging the slider from left to right will decrease the speed of the SmartMate.

This is the System Options menu in SOLIDWORKS to control the speed to apply SmartMate.

For more information on SOLIDWORKS or if you have any questions, don’t hesitate to contact us at Hawk Ridge Systems today. Thanks for reading!

Picture of Ricky Huynh

Ricky Huynh

Ricky Huynh is a SOLIDWORKS senior applications engineer with Hawk Ridge Systems based in Mountain View, California. He specializes in SOLIDWORKS, Composer, and Electrical. He graduated from UC Davis in 2010 with a B.S. in mechanical engineering.
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