Inventor

Using Joints in Autodesk Inventor 2014

30 Sep, 2013 By: R. Eric France

IMAGINiT Tricks Tutorial: Don't get bent out of joint about the new tool on the Assemble tab — learn how to use it to your advantage.


Editor's note: This tutorial courtesy of IMAGINiT Technologies.
 

If you started using Inventor 2014 recently, you may have noticed a change to the tools and terminology used to constrain components together in an assembly. With the 2014 release, a new Joint tool has been added to the Assemble tab, and a new term — relationships — is used to describe the process of locating components relative to each other. Let's look more closely at both and see how to take advantage of these enhancements to Inventor.

Where Are the Constraint Tools?

You may have already noticed that the Assemble tool, which appeared several releases ago to streamline constraining components, has disappeared. Don't worry: It is still there, and it behaves just like it did in the past. However, it has been moved to the expansion portion of the relationships panel.



Additionally, it is still available on the Assembly Marking menu along with the other relationship tools.



While we are on the topic of relationships, let's talk about the term and what it means to Inventor users. Basically, creating relationships is the process of adding intelligence to two components to identify how they behave with each other. In the past, this was done by applying constraints, but now it has been expanded to include applying joints. In addition to joints, there are some new visibility tools to graphically understand the relationships that have been established and their health in the assembly.

How Joints Work

We are all familiar with the fact that when we bring components into an assembly, they come in with six degrees of freedom (DOF). When we apply constraints, we reduce those DOF based on the type of constraint we apply and what geometry we select. For example, if we apply a mate-flush constraint, we reduce the DOF of the component by two rotational and one translational.

With joints, it is a little different. When applying a joint, we are identifying how many degrees of freedom will remain after we apply it. So, if a part starts with six DOF and we apply a rotational joint, we will only be left with one rotational DOF — the ability to rotate around the axis specified.



These images depict the joints available in Inventor (left) and the DOF remaining for each (right). We can see that the use of joints produces a more fully constrained set of components more quickly than if we just applied constraints to the components.

 

Applying Joints

We now know what joints are and what they do, but how do we apply them? Joints are applied a little differently than we would apply constraints. Using the Connect selection buttons on the Joints dialog (below, left) or the Joints mini-toolbar (below, right), we are able to select points along faces or edges to establish the relationship between the components.



When you select a face, you can choose from any of the corners, the midpoints of any of the edges, and even the center of the face to position the component. When you select a linear edge you can pick from its endpoints and midpoint. When you select a circular edge or spherical geometry, you can pick the center of the edge or geometry.

Spherical geometry can also be selected where other geometry intersects the sphere. As you would expect, you can also Flip the direction of the selection and you can use the Align tools to adjust the orientation of the components you are applying the joint to.



Some additional options for controlling joints are gaps and limits. Similar to Offset for constraints, Gap allows us to keep components a specified distance away from each other. Also like constraints, we can apply limits to the angular and/or linear elements of a joint to specify a range of motion for that joint.

Completing the Joint

After applying the joints we need to control the position or motion of our components, there are several other options available on the right-click cursor menu of a joint. If we want to maintain the current position of a component, but not restrict the DOF, we can lock the joint. We can use Protect to monitor a joint and prompt us when additional joints being applied violate the DOF of the monitored joint.



Additionally, while joints go a long way toward establishing the relationships between our components in the assembly, constraints are always available to finish the job. Feel free to use them as you have in the past.

Looking at Relationships

Once you have established the relationships, it is sometimes necessary to see and understand how they apply to other components. By using Show Relationships and selecting the components we want a better understanding of, we get the glyphs shown here.



Selecting a glyph provides specific information regarding that relationship and the components involved. The Show Sick command is used to identify relationships that have been broken or are over-constraining components.

To review, we defined two new enhancements in Autodesk Inventor 2014. First, we looked at where the relationship tools are located. Then, we focused on what joints do and how to apply them. Next, we looked at the other options used with joints. Finally, we discussed how we can view, understand, and monitor the joints in our assembly. Now you know how useful joints can be, and you can leverage them in your daily use of Inventor. Time to leave this joint!


About the Author: R. Eric France

R. Eric France

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