4.2.2 Boolean Operations (None, Unite, Subtract, Intersect)

This exercise deals with boolean operations:

 

Create independent bodies

The Boolean Operation None  creates two independent bodies.

 

Unite

The Boolean Operation Unite connects multiple bodies by uniting them to a single body.

 

Subtract

The Boolean Operation Subtract  subtracts one body from another body.

 

Intersect

The Boolean operation Intersect creates a body from the intersecting parts of two (or more) bodies.

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Create a new model with the name bool according to the naming convention.

Dimension	Value [mm]
Diameter	50
Height	500

Select the Z-Axis as orientation.

The cylinder should be positioned at the point of origin of the WCS-coordinate- system. To do so confirm the default values.

 

None (creating independently)

Next, create a sketch on the XY-Plane: (refer figure "Sketch").

Extrude this sketch with the values Start 100 mm and End 400 mm. Make sure, that you selected the positive Z-Axis for Specify Vector.

The cylinder should now be created independently from the first shaft. Cylinder and shaft should not be united to form a single body. To do so, choose for Boolean. Close this menu by clicking OK . (refer figure "Boolean Operation: None")

 

Unite

To open the window Unite, click Unite .

As soon as this menu pops up, first select the narrow shaft, then the wide one.

Confirm this selection by clicking OK.

Now both shafts are not independent anymore. They now form a single body and changes affect both. (refer figure "Boolean Operation: Unite")

Now access Part Navigator. Unite now appears as part of your model history.

To undo Unite, you can eiter click Undo or delete the feature from Part Navigator..

 

Subtract

Click Subtract to open the window Subtract.

First select the wide shaft, then the narrow. By doing this, the narrow one will be subtracted from the other one.

Confirm with OK. (refer figure "Boolean Operation: Subtract) Undo this action or delete the feature Subtract within Part Navigator.

 

Since both shafts are intersecting, you can create a body with the boolean operation Intersect.

Click Intersect to open the window Intersect .

Again, select both shafts and confirm by clicking OK.

NX creates a body from the intersection of both. (refer figure "Boolean Operation: Intersect")

 

Attention!

For the boolean operations Subtract and Intersect bodies have to intersect. (refer figure "error Boolean Operation") For the operation Unite at least one joint surface has to exist.

Hint:

If any of those requirements are violated by editing geometry, an error pops up. In this case just use the Undo-Button !

 

Summary

Boolean Operation	Function	Icon
None	create independently
Unite	unite
Subtract	subtract
Intersect	body from intersecting parts

Hint:

These examples are used to illustrate how boolean operations work. For effective modeling, typically form features as explained in chapter 4.2.3 "Form Features" are preferred. Boolean operations should only be used if using them can save additional steps in construction or if no adequate form feature exists.