Applying Mates

After adding the components to the assembly window, you have to apply mates between them. By applying mates, you establish real contact and motion between components.

You can apply mates between parts using the Mate tool.

The following sections explain some of the assembly mates that you can apply using the Mate tool.

Coincident: Using this mate, you can align two faces such that they will point in the same direction.

On the context toolbar that appears in the graphics window, click Flip Mate Alignment to flip the alignment direction.

Parallel: Using this mate, you can make an axis, face, or edge of one part parallel to that of another part.

Perpendicular: Using this mate, you can make an axis, face or edge of one part perpendicular to that of another part.

Concentric: Using this mate, you can align the centerlines of the cylindrical faces.

Click Flip Mate Alignment to flip the alignment direction. Check the Lock Rotation option to lock the rotation between components.

Lock: Makes parts to form a rigid set. As you move a single part in a rigid set, all the other parts will also be moved.

Distance: Applies the distance mate between two components.

Angle: Applies the angle mate between two components.

Click Flip Dimension to reverse the angle direction.

Tangent: This mate makes two faces tangent to each other.

1. On the CommandManager, click Assembly > Mate.
2. On the Mate PropertyManager, click Concentric.

1. Click on the cylindrical face of the Shaft.

1. Click on the inner cylindrical face of the Flange

In SOLIDWORKS, the first selection is made transparent while applying mates. You can turn OFF the transparency by unchecking the Make first selection transparent option in the Options section of the Mate PropertyManager.

1. Click Add/Finish Mate.

This aligns the Shaft and the Flange axially.

1. On the Mate PropertyManager, click Coincident.
2. Click on the front face of the shaft.

1. Rotate the model.
2. Click on the slot face of the flange, as shown in figure.

1. On the Mate PropertyManager, under the Standard Mates section, click the Aligned button.

1. Click OK on the SOLIDWORKS message.

1. Click Add/Finish Mate.

This aligns front face of the Shaft and the slot face of the Flange.

1. On the Mate PropertyManager, click Coincident.
2. In the FeatureManager tree, expand Flange and select Top Plane.
3. Expand Shaft and select Right Plane.

1. Click Add/Finish Mate.
2. Click OK on the PropertyManager.

This assembles the two components and fully constrains the Shaft.