Adding the Third Component

In order to assemble the third component, you need to hide the Flange.

1. In the FeatureManager Design Tree, click the right mouse button on the Flange and select Hide Components to hide the Flange. Now, it is easy to assemble the third component.

SOLIDWORKS allows you to hide a body placing the cursor on it and pressing the Tab key. You can unhide the body by placing the cursor at its position and pressing Shift+Tab.

Tip: You can also hide a part face so that the obscured face is visible. To do this, activate the Mate tool, place the pointer on a face, and then Alt key; the face is temporarirly hidden.

1. To insert the third component, click Assembly > Insert Component.
2. On the PropertyManager, click the Browse button.
3. Browse to the folder: C:\Users\Username\Documents\Oldham Coupling, and then double-click on the Key.
4. Click inside the graphics window to position the key.

1. Activate the Mate tool.
2. On the Mate PropertyManager, click Coincident.
3. Right-click on the side face of the key and select Select Other.

1. From the Select Other box, select the bottom face of the Key.

1. Select the bottom face of the slot.

1. Click Add/Finish Mate.
2. This aligns the bottom face of the key with the bottom face of the slot.

1. Select the front face of the Key and back face of the Shaft.

1. Click Flip Alignment.

1. Click Add/Finish Mate.
2. This applies the mate between the selected faces.

1. Click on the top face of the key.

1. Rotate the shaft and select the side face of the slot.

1. Click Add/Finish Mate.

1. Click OK on the PropertyManager.
2. Now, you have to turn-on the display of the Flange.
3. Click the right mouse button on the Flange in the FeatureManager tree, and then select Show Components to display the Flange.