AutoDrop

Use AutoDrop to automatically size and place standard content.

Access:

In an open assembly file: In the Place from Content Center dialog box: Select an AutoDrop enabled Family, and click OK. Double-click an AutoDrop enabled family. Note: Hold down ALT and double-click an AutoDrop enabled family to place a member from the Family dialog box. The Family dialog box allows selection of specific sizes and material. From the Browser Bar Favorites drop-down menu, use drag and drop or double-click the selected AutoDrop-enabled family.

Overview of individual cursors:

	Select a conical hollow face - used for a countersunk bolt. The target cone angle and the bolt head cone angle must be the same.
	Select a shaft cylinder - used for bearings, washers, retaining rings, and so on.
	Select an edge on a shaft - used for bearings, washers, retaining rings, and so on.
	Select an edge in a housing - used for bearings.
	Select a hollow cylindrical face -used for bolts, pins, bearings, and so on.
	Select a hole edge -used for bolts, nuts, washers, pins, and so on.
	Select a tapped cylindrical face - used for nuts.
	Select a normal planar face - used for nuts, bolts, washers, bearings, pins, and so on. Used as a secondary target after a cylindrical face was selected.
	Select a groove edge
	Select an inner groove edge - used for external and internal retaining rings.

Toolbar commands

	Change size inserts the part and opens the Part Family dialog box where you can edit the component.
	Bolted Connection opens the Bolted Connection Generator. Available for some bolts only.
	Apply inserts the component to the assembly. This command finishes the current insertion and AutoDrop continues with the given family. You can insert several sizes during one command call. The subsequent default member is always the last one dropped.
	Done inserts the component to the assembly and stops AutoDrop.
	Follow pattern is for circular patterns. If the target geometry is in a pattern, the inserted component can follow the pattern. By default, this option is switched on. Note: The pattern must be on a part, not an assembly.
	Follow pattern for rectangular patterns. If the target geometry is in a pattern, the inserted component can follow the pattern. By default, this option is switched on. Note: The pattern must be on a part, not an assembly.
	Insert multiple inserts multiple components. This switch is available if AutoDrop identifies several available targets like the selected target. For example, if you select a circular edge of a hole and in the target component there are several coplanar circular edges with the same diameter, use this switch to populate components for all holes. If the Insert multiple switch is on, AutoDrop highlights the targets. Use the tooltip of the Insert multiple command to check how many components are offered for the insertion. Insert multiple function does not offer targets for insertion that are already occupied. If there is a component already inserted to some geometry, Insert multiple function disregards such target. For example, if a screw is inserted to some of the holes, such holes are not populated. This behavior happens even if the screw is invisible or suppressed.
	Flip flips the bearing. It changes the bearing side used for mating (for example for tapered roller bearings). The bearing is always inserted to mate the adjacent planar face, regardless of the flip. With some bearings, which look the same from both sides, the flip has no visible affect. If the particular bearing family template does not have iMates defined from both sides of the bearing, the Flip command is not available.