Create drawings from models (Creo Elements/Direct Annotation) > Modify drawings > Add and modify BOM information > Create position flags
Create position flags
You can attach position flags to the views in the drawing associated with the parts included in the current BOM table. The flags and table entries can then be numbered to provide clear reference.
To attach position flags,
1. Scan an assembly for BOM information.
2. Generate reference numbers.
3. In Creo Elements/Direct Annotation, click Insert and then, in the BOM group, click the arrow next to Pos Flags. Alternatively, click Part Library and then, in the Position Flag group, click the arrow next to Create.
4. Click BOM Flag create. The Create Flag dialog box opens.
The view geometry to which it is possible to add flags is highlighted in green.
To attach position flags to all instances of a part or an assembly, click Part Library and then, in the Position Flag group, click the arrow next to Create. Click BOM Flag Instance create.
In shared parts, after scanning a frame for BOM information, you cannot create BOM flags on individual part views.
5. If necessary, specify a different active layout for the flags. See Flag layout.
6. Click Geometry and select a geometrical element in the viewport.
If you select a geometrical element which already has a flag, the geometrical element is highlighted in red until you specify the flag's position. Also, Creo Elements/Direct Annotation issues a warning if you select a geometrical element which is not represented in the BOM table.
7. Specify the position for the flag by clicking in the viewport or by typing coordinates in the user input line.
8. Select additional geometrical elements to create more flags, or click to complete the operation.
For information on how to automatically generate BOM flags, see Generate BOM flags.
Flag layout
Position flags are drawn according to the active flag layout. Creo Elements/Direct Annotation selects an active layout automatically, but you can change it in one of the following ways:
Type the layout name in the Act Layout box.
Click Act Layout and select the layout from the Flag Layout table.
The selected layout remains the active layout until it is changed again.
The flag layout table
The Flag Layout table displays all the flag layouts available for new position flags. Any sketch can be used as a layout, but it must be registered first to appear in the table. See Creo Elements/Direct Annotation customization for advanced users.
Layouts are listed in the table in the order they were registered. However, you can control what is displayed by applying a filter over the column data. Right-click the Flag Layout Name column header to open the Column Filter box, and set (or clear) filters.