Using the Center-Plane command

To place a new part into the assembly, drag a placement part from the Parts Library into the assembly workspace. The system automatically opens the Assemble command and the associated Assemble command bar, and highlights the placement part (for more information, see Assemble parts (workflow)). Most often it takes more than a single relationship to fully assert a Center-Plane relationship with the Center-Plane relationship being the last relationship to be applied (similar to a Mate relationship).

On the Assemble command bar, select the Center-Plane option from the Relationship Types drop-down list .

For more information, see Using the Center-Plane features on the command bar.

Use the Selection Type option to determine if the placement part is to be identified by a single element or a double element (for more information, see About the Center-Plane relationship).

On the highlighted part being placed, select one or more elements (depending on the Placement Type being either a single or a double) on the placement part. The valid elements include the planar faces, edges, keypoints, axes, or reference planes.

Select the first of two elements in the assembly between which the placement part is to be centered. These elements can be on the same part or two different parts. The selection sequence is to select the assembly part first then the specific element followed by the second instance of assembly part and element. The command can be used to center objects between faces and planes that are not parallel.

To complete the action, press OK. The Assemble command bar remains open to apply the next relationship. To apply another relationship, continue with Create additional relationships. To close the Assemble command and the Assemble command bar, press the Esc key.

To create a Center-Plane relationship between two parts already in the assembly, you can do either of the following:

• To create a relationship using the Assemble command bar, the Assemble command bar must be open. If not open, select the Assemble command (Home tab→Assemble group→Assemble). On the Assemble command bar, select the Center-Plane icon from the Relationship Types drop-down list.

• To create a relationship using the Center-Plane command bar, the Center-Plane command bar must be open. If not open, select the Center-Plane command that resides under the Center-Plane relationship (Home tab→Assemble group→Center-Plane) .

The actions that can be performed are the same for each option. However, after the Center-Plane command bar is opened, only an Center-Plane relationship can be applied. The relationship type cannot be changed (see Using the Center-Plane features on the command bar).

Select the relationship parts and features as described previously.

To complete the action, press OK.

To close the command and the command bar, press the Esc key.