Unite

Unite

Use the Unite Boolean command to combine the volume of two or more solid tool bodies into a single target body. This command creates a Unite feature.

You can:

• Use a group of bodies as the tool.
• Create a united body using only the tool bodies.
• Select body regions to keep or remove.
• Retain unmodified copies of the target and tool bodies.

Target solid body (1) united with a group of tool bodies (2) into a single solid body

To quickly convert a discrete Boolean unite feature to a subtract feature, right-click the feature and select Convert to Subtract.

Where do I find it?

Application	Modeling
Command	Unite

Unite with region selection

When uniting solid bodies that have overlapping, or excess material, you can use region selection to identify a collection of faces that should be kept or removed when the solid bodies are united.

Region selection saves you from having to trim the bodies before uniting them. This simplifies the part navigator feature tree, as there are no separate trim body features listed.

Before unite

After unite with selected regions removed

Combine tool body volumes using Unite

1. Choose Home tab→Base group→Unite .

Note: In the Unite dialog box, by default, Select Body is active first in the Target group, and after you select a target, it is active in the Tool group. 2. Select a target solid body.

** Selected target body (cyan)

** 3. Select one or more tool solid bodies.

** Selected tool solid bodies (red)

** 4. (Optional) You can do one or more of the following:

In the Preview group, use Show Result / Undo Result to check how the target and tool solid bodies will be modified.

** Modified solid body

** 5. To save an unmodified copy of the target body, select Keep Target. 6. To save unmodified copies of the tool bodies, select Keep Tool. 7. Click OK or Apply.

The target body is modified by combining it with the volumes of the four tool bodies.

Unite solids and remove regions

In this procedure you will unite solid bodies and define regions to remove.

1. Choose Home tab→Base group→Unite .
2. Select the target body.
3. Select the tool body.
4. Next you will define the regions to remove. In the Region group, select the Define Regions check box.
5. Click Body Region and then select Remove.
6. Select the two sheet bodies shown.
7. Click Apply.

The solids have been united and the selected regions have been removed.

Combine groups of adjoining bodies

For each group of adjoining tool bodies, NX creates a separate united body. If a part contains multiple groups of adjoining bodies, you can create multiple solid bodies by combining each group of bodies.

1. Choose Home tab→Base group→Unite .
2. In the graphics window, select a target body.

For this example, we select body (1) as the target body. 3. Select all the remaining bodies as tool bodies.

Note: You can select multiple tool bodies, but, you can select only one body as the target body. 4. Click OK or Apply.

Unite dialog box

Target
Select Body
Tool
Select Body
Region
Define Regions
Separate Target and Tool Regions
Select Region
Select Target Region
Select Tool Region
Settings
Keep Target
Keep Tool
Convert to Sew Feature
Tolerance