A variety of methods are available to apply alignment constraints to parts and assemblies using the Positioning Constraint tool.  Use Positioning Constraint tool to maintain spatial relationships between parts , IntelliShapes, and/or assemblies.

This tool allows the user to determine the desired constraint prior to selecting any geometry and it will narrow the available types based on entity type selected. This Tool can be activated in both the normal solving mode or within the Mechanism Mode. In addition, this tool incorporates the following types:

• Mate. Creates a constraint between two faces where the faces are anti-aligned (Use the alignment option in the command bar to change alignment direction).
• Align. Creates a constraint between two faces where the faces are aligned (Use the alignment option in the command bar to change alignment direction).
• Parallel. Create a constraint between two faces/edges where the edges/faces are parallel.
• Perpendicular. Create a constraint between two faces/edges where the edges/faces are perpendicular
• Coincident. Creates a constraint between a point and point/face/edge where the point is coincident with the second selection.
• Concentric. Creates a constraint between an edge (or circular face) and a circular face to where the selections are concentric.
• Tangent. Creates a tangent constraint between a two surfaces or point and surface. This constraint is to a single surface and an infinite surface definition (Spline Surface are to the bounded surface).
• Distance/Angle. Creates a locked distance or angle SmartDimension at the current location of the selected entities.
• Follower/Cam. Creates a Tangent Constraint from a point or surface to the swept side surface of an extruded profile.

In addition to these constraints, a Fixed in Parent Constraint can be added by right-clicking on a selected shape. This will lock all degrees of freedom for the shape which will disallow all movements. The shape is fixed in the parent space which means that the parent shape can move and the fixed shape will stay in its current position with respect to its parent.

Note: Positioning Constraints cannot be  applied on IntelliShape features of Structured Parts. Positioning of features on Structured Parts are defined by the 2D Sketch Positioning. Review the 2D Sketch Positioning for details.

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To Apply A Positioning Constraint:

1. Select the Positioning Constraint Tool from the Standard Toolbar, from the Tools Fluent Ribbon Bar, or from the Tools menu.
2. Select the desired type of constraint from the drop-down list within the command bar or you can selected the faces first and select the constraint type from the "S" popup menu. The S menu allows you to more easily select constraint type and apply them.
3. Select Faces/Edges of Assemblies/Parts /IntelliShapes to create the constraint
4. (Alternatively, select the entities first and then select the constraint type in the drop-down list that is available based on the selections made).  If needed, toggle the alignment to the desired alignment direction.
5. Left-click to accept the created constraint or right-click to cancel the constraint creation (or select the options in the command bar).
6. When all constraints have been added, select the "OK" button to accept the change.

Note: Often during the design, constraints previously added on object may need to change and/or copies of object are created where constraints information needs to be reused and adjusted. New behaviors have been added to the constraint and dimension annotations to allow the ability to reconnect these annotations to new reference information. For example: A fastener may be co-axial aligned to a particular hole. Due to the design change, a new hole is created where a copy of the fastener is needed. After creating the copy, users can now simply drag the endpoint of the previous co-axial constraint and refer it to the newly created hole to create the new alignment for the copied fastener.

Constraint Status Display In Scene Browser:

Parts and Assemblies will now display the over, under, or fully defined constraint status in the scene browser. This option can be disabled if not needed.

Automatic Part/Assembly Constraint On Drop Option:

This functionality gives you the ability to automatically create constraints when dropping parts onto one another. The constraints will be applied speeding up your design time. The option can be turned on and off in the Tools/Options/Assembly menu.