Boolean Operations on Parts

In some situations, it may be advantageous to combine what were separate parts back into a single part, to subtract one part from another, to find the intersection part, or to get the difference from the selected parts.. The operations of combining parts and subtracting one part from another are known as Boolean operations. You control these operations with commands on the Boolean Operation Toolbar or from the Feature Fluent Ribbon Bar.

The Boolean Operation Toolbar provides the following capabilities:

Set Operation. This command allows the user to change a part’s operation type. This can be very useful when creating parts with complex inner cavities. The inner chambers can be created as positive material. This positive part can then have its operation type changed to remove material and then subtract material from a larger shape/part to achieve the desired result.
Boolean. This command allows multiple parts to be combined into a single part. The resulting part is always defined by the first one selected in the set. Following a Boolean operation, components of a part lose their IntelliShape identities.
Union. This command to union to selected parts into a single shape regardless of the set operation designation on the parts.
Subtract. This command to subtract the second selected part from the first selected part regardless of the set operation designation on the parts.
Intersection. This command creates an intersection part based on the two selected parts. The parts must intersect in order for the command to yield a result.

The Boolean Command on the Feature Fluent Ribbon Bar provides the following capabilities:

Union. This command to union to selected parts/bodies into a single shape.
Subtract. This command to subtract the second selected part/body from the first selected part/body.
Intersection. This command creates an intersection part/body based on the two selected parts/bodies. The parts must intersect in order for the command to yield a result.

The difference between the Boolean Operation Toolbar and the Boolean Command on the Feature Fluent Ribbon Bar is that the toolbar will support the Set Operation commands and the Boolean Command on the Feature Fluent Ribbon Bar will support Bodies under Structured Parts (review the Boolean Feature topic for more details).

To use a Boolean operation to create a single part from multiple parts:

Drag one independent part onto a surface of a second independent part in the scene.
Holding down the Shift key, select the two parts at the part editing level.
From the Feature Fluent Ribbon Bar or Boolean Operation Toolbar, select the desired Boolean Type on the toolbar or in the command browser.
Click in the scene background to deselect the new part and then select either of the original parts at the part editing level.

A cyan outline appears on both components of the new part.

To create a negative part using the Set Operation:

Display the Scene Browser.
Drag the desired shape to be used as a negative part from one of the catalogs and drop it in the scene as an independent shape.
Select the new shape at the part editing level. Note that, in the Scene Browser, the text box next to the new shape’s icon is highlighted in gray.
From the Feature Fluent Ribbon Bar or Boolean Operation Toolbar, choose Subtract on the toolbar or in the command browser.
Select OK to complete the command.

when you use the Set Operation and Remove Material, the shape becomes a negative part and is displayed in the scene as a semi-transparent object. Note that in the Scene Browser, its icon has changed to a semi-transparent icon.

The negative part can now be dragged into a catalog, to be retrieved and applied later to a solid part in a scene using the Boolean Command on the toolbar.

Note: Boolean Parts can still be edited using the original IntelliShapes. In the Scene Browser, you can select the original features under the boolean feature.

Note: Part to Part Boolean is not supported on Structured Parts. Only Body Boolean operations are supported.