On Freedom and Constraints
Autodesk Inventor allows you to assemble parts to create assemblies that can be tested for fit and function. The way to assemble parts in Inventor is to use assembly constraints. These constraints allow you to maintain the positions of components or their relations to one another in an assembly (such as two faces touching each other or a bolt in a hole).
Defining Degrees of Freedom
Let's first discuss the degrees of freedom (DOF) and how they impact assembly constraints. All parts initially have six DOF without any assembly constraint. The six DOF include three translational ones (linear along the x-, y-, or z-axis) and three rotational ones (angular along the x-, y-, or z-axis, as shown in Figure 1). A part or assembly is considered grounded (fixed in space) when it has no DOF. The first part inserted or created in the assembly is set as grounded by default in Autodesk Inventor. More than one component can be grounded and you can toggle between the components that are grounded. Select the components either in the graphics or the browser, right-click, and choose Grounded. You can visually identify the grounded components by their thumbtack icons displayed in the browser.
Figure 1. This symbol illustrates the three translational and rotational degrees of freedom available.
As you apply assembly constraints, DOF are removed based on the movements impacted by the constraints. Let's say we have two basic cubes, as shown in Figure 2. One currently has six DOF available and the other is grounded. If you apply a mate constraint between any two faces, it cancels three DOF (one translational movement and two rotational movements) from the body that remains movable. You can turn on a visual DOF symbol on the model by accessing the model properties. Right-click on the part file and select Properties. Then select the Occurrence tab and select the Degrees of Freedom box, also shown in Figure 2 (on the left is the assembly without the mate constraint, and, on the right, with the mate constraint).
Figure 2. The two cubes on the left show the way the assembly is before applying the constraint, and the arrangement on the right after applying the mate constraint
You can apply assembly constraints to edges, faces, and work geometry. You can select cylindrical faces/edges as well as planar faces/edges. If you're in the mate constraint and select a cylindrical face, the program will automatically pick the centerline axis of that face as the point to assemble to. Inventor supports simple constraints (such as mates and flushes), motion-specific constraints (for gears), and transitional constraints (to maintain contact between predefined faces).
- Mate/Flush assembles components face-to-face (mate) or adjacent to one another with their faces flush. It removes one degree of linear translation and two degrees of angular rotation between planar surfaces. You can select edges as well as faces to assemble.
- Angle assembles edges or planar faces at a specified angle to define a pivot point. It removes one degree of angular rotation.
- Tangent assembles faces, planes, cylinders, spheres, and cones to contact at the point of tangency. Tangency may be inside or outside a curve, depending on the direction of the selected surface normal. Tangent constraint removes one degree of linear translation.
- Insert combines a face-to-face mate constraint between faces and a mate constraint between the axes of the two components. The Insert constraint is used to position a bolt in a hole. Only one rotational degree of freedom remains after applying this constraint.
- Rotation specifies that a part rotates in relation to another part using a specified ratio, typically used for gears and pulleys.
- Rotation-Translation specifies that a part rotates in relation to the translation of another part using a specified distance. It shows the planar motions of rack and pinion devices, for instances.
- Transition creates a relationship between a cylindrical face and a contiguous set of faces on another part, such as a pin in a slot. It maintains contact between the faces as you slide the component along the open degrees of freedom.
To access assembly constraints, you need to be in an assembly file with at least one component referenced into it. You can select the Place Constraint icon from the tool palette or use the predefined shortcut key (C). When the dialog box opens, it defaults to the mate assembly constraint. By default Autodesk Inventor has the Show Preview option turned on. After the assembly selections are made, under-constrained components automatically move into a constrained position. To apply the assembly constraint, you must select Apply. Uncheck Show Preview to if you don't want to graphically view the constraint being applied