Using the Planar Align features on the command bar

The Planar Align command bar features are used to define a Planar Align relationship between two face elements in an assembly (for more information, see About the Planar Align relationship).

The following image shows the Planar Align relationships using the horizontal toolbar form of the Command User Interface. The features displayed for the vertical docking window interface form are similar. The version that is displayed is user-selected using the Command User Interface options on the Helpers tab in the QY CAD Options dialog box. For more information, see Helpers tab (QY CAD Options dialog box).

The Planar Align command bar:

has the same features as the Assemble command bar:

when a Planar Align relationship type is selected. For more information, see Assemble command bar.

Access the Planar Align command bar (Home tab→Assemble group→Planar Align) to apply a Planar Align relationship between two parts already in the assembly workspace. The Assemble command bar for a Planar Align relationship is displayed when a new part is dragged into the assembly workspace from the Parts Library and the Planar Align relationship type is selected (for more information, see Using the Planar Align command).

The command bars have the following features:

Command Bar Icon

The icon displayed is determined by how the command was accessed. The Planar Align icon is displayed if the Planar Align command is selected from the ribbon (Home tab→Assemble group→Planar Align) when defining or modifying a relationship for parts that are already in the assembly workspace. The Assemble icon is displayed after dragging a new part into the assembly workspace and a Planar Align relationship type is selected.

Occurrence Properties

Select this option to open the Occurrence Properties dialog (for more information about the selected part, see Occurrence Properties command). This option is only available after you select a part.

Construction Display

This feature is only displayed when a part is selected. When visible, this option opens the Construction Display dialog box that is used to show or hide the selected reference elements for the part. The visible reference elements (the ones that have been turned on) can then be selected to form the Planar Align relationship. The reference items include:

• show/hide coordinate systems

• show/hide reference planes

• show/hide sketches

• show/hide references axes

• show/hide construction surfaces

• show/hide construction curves

• use designed or simplified part

Relationship List

On the Planar Align command bar, the identifier for the next relationship to be formed is displayed. This value is for reference only and cannot be changed. On the Assemble command bar the identifier for the next relationship to be formed is also displayed but any previously defined relationships are displayed in the drop-down list and can be selected. This allows previously defined relationships to be modified directly from the Assemble command bar.

Relationship Type

On the Planar Align command bar, this option is locked and cannot be changed. On the Assemble command bar the type of relation to be formed can be selected from the list. Changing the relationship type from Planar Align to some other relationship type also changes the options that appear on the command bar.

Command Bar Options

Select this feature to open the Options dialog box for the command bar (see Assemble command bar Options dialog for more information about using the options in this dialog box).

Placement Part

Specifies which part is to be positioned in the assembly. This button is active when adding a relationship to a part that already exists in the assembly, or when placing a subassembly. This button is inactive when placing a new part in an assembly as the new part that is dragged into the assembly workspace is automatically selected as the placement part.

Placement Part Element

Use this feature to specify which face element is to be used on the part being positioned in the assembly.

Target Part

Use this feature to specify the target part to be used to form the relationship.

Target Part Element

Use this feature to specify the target face element to be used to form the relationship.

OK

Orients the part in the assembly using the relationship that has just been defined.

Offset Type

Use this option to open a drop-down list of Offset Types. Select one of the following types of offset:

• Fixed—When a fixed offset is defined, the value for the offset distance (the fixed distance between the selected faces) is specified. If the offset value is set to zero, the faces are coplanar. When this option is selected, enter the offset value or zero into the adjacent Offset Value box. A negative value can be entered. For more information, see Modify the offset value for a relationship.

• Float—When a floating offset is defined, another applied relationship will control the offset distance. This option is selected when a fixed value is not known or is variable and the offset is to be determined by a subsequent relationship. When this option is selected, the Offset Value box is disabled.

• Range—When a range option is selected, two offset values are defined to limit the upper and lower limit of the offset values. Movement is limited by the defined range. When this option is selected, two offset value boxes are displayed. The first box is for the minimum range value and the other is for the maximum range value.

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