Inventor Design Intent And Imates

Jeff Wymer

Design Intent and iMates

The Knowledge Vault is a set of intelligent technologies that allows you to capture, store, and reuse the embedded design knowledge contained within your Autodesk Inventor models. iFeatures, iMates, iParts, and the Engineer's Notebook make up the basis of this Knowledge Vault. This month I'll highlight iMates and show how to use them to virtually automate the assembly of standard components within an Autodesk Inventor assembly.

iMates

While some products are unique, designed totally from scratch, many new designs are developed reusing existing components. This is especially true of industrial machinery; up to 60 percent of components within new designs may be reused, possibly more. As you work with Autodesk Inventor, you'll naturally build a database of standard parts, whether you've gotten them from the Web, found them in the content library that installs with Autodesk Inventor, or created them yourself. iMates, as shown in Figure 1, allow you to select the parts or subassemblies you need from a library and insert them into a new design and have them automatically assemble, providing a tremendous time savings when creating a new design.

Figure 1. iMates provide a tremendous time savings by automatically assembling your components together. Since the Create iMate dialog box looks exactly like the familiar Place Constraint dialog, iMates are very easy to learn and use.

Authoring iMates

While iMates provide a tremendous time savings downstream when adding standard components to an assembly, they do require up-front work and planning. First of all, you need to determine the most common way a component is going to be assembled.

To begin, instead of placing constraints on the component, simply select Create iMate from the Part Features or Assembly Panel tool palette. This will open a dialog box, similar to the Place Constraint dialog box. An iMate can be considered half of an assembly constraint, hence the similarities between the two dialogs. Next, select the appropriate constraint type and geometry that satisfies the assembly requirements determined earlier.

Upon selecting the Apply or OK buttons, you will notice that Autodesk Inventor places an iMate glyph on the part or assembly model. You will also find that an iMate folder has been created at the top of the active part or assembly node within the browser. This folder lists all of the iMates that currently exist on the active component.

To effectively use iMates, you may need to modify their properties after creation. By simply selecting and right-clicking over the iMate within the browser, you will find a number of different options relating to the iMate. Selecting Properties will open a dialog box, providing access to some important options.

One of the most important properties worth modifying is the iMate's name. Autodesk Inventor can automatically connect components upon placement based on matching iMates with the same name. When renaming, provide meaningful names that follow a common naming standard for replacement components. For example, to identify an iMate on a hole feature, rename the iMate to reflect the thread series and pitch. Fasteners containing the same iMate name, based on the thread callout, can then be assembled automatically.

Other options contained within the iMate Properties dialog are offset and index. The offset field allows you to modify the offset value of the assembly constraint formed by matching iMates. When a component is added to an assembly, its iMates solve in a sequential order, and the index drop-down list provides a means to control this.

In many cases, one iMate alone isn't enough to fully assemble a component. To provide iMate functionality for these components, Autodesk Inventor offers Composite iMates. Composite iMates essentially group a number of a component's iMates together into one unified iMate. To create a composite out of existing iMates, simply select the iMates that are to be grouped together from the browser, right-mouse click and select Create Composite. The Composite iMate behaves very similarly to a normal iMate, so be sure to rename it with a recognizable name.

Inferring iMates Autodesk Inventor 6 expanded upon the iMate functionality by providing a method of extracting the iMate intelligence from existing assembly relationships. This makes it easy to capture the design intent of the assembly constraints at the component level. To extract this information, select the component that you would like to add the iMates to, right-mouse click and select Infer iMates. Within the Infer iMates dialog you will find two options: Selected Occurrence Only and Create Composite iMates. The Selected Occurrence Only option allows you to control whether iMates are extracted only from the component instance selected or all instances of the same part. Keep in mind, one part can be instanced a number of times within an assembly and may have a variety of assembly constraints applied. The second option, Create Composite iMates, will collect all of the assembly constraints applied to an instance and group them within a composite. Assembling with iMates iMates provide an easy interface for assembling components and there are a number of ways to use them, as shown in Figure 2. The first method is to use iMates in conjunction with the Place Constraint dialog box. After starting the Place Constraint command, simply select an iMate glyph found on a component. Once you've picked an iMate glyph from one part, select part geometry or an iMate glyph from another component to constrain to. Two rules to remember with this method are that the iMate glyphs must be visible on the part and that the constraint type selected in the Place Constraint dialog box must match the iMate glyph. To turn on the visibility of an iMate glyph, simply select the part, right-mouse click, and select iMate Glyph Visibility. Figure 2. If you need to assemble multiple instances of a component, use the Infer iMates functionality to quickly extract iMates from existing assembly constraints. Then you can quickly use the iMates to assemble the other instances

Another method you can use is Autodesk Inventor's drag-mate technology. While holding down the Alt key, you can pick and drag a component to another part and create an assembly constraint. iMates extend the drag-mate functionality by filtering the constraint type available during drag. While dragging, all un-matching iMate glyphs disappear automatically, making it easier to find possible iMate solutions. For more information on drag-mates, perform a search in the help system on Alt-drag constraint placement. Placing Components The last method for using iMates involves initial part placement. Let's assume that an existing part in your assembly already has an iMate, or Composite iMate, placed on it. After selecting the Place Component command, browse to the component you want to place. It should also have iMates, or Composite iMates, with an identical name as the component in the assembly. Once you find the component to insert, select the Use iMate checkbox, as shown in Figure 3. As soon as you press OK, Autodesk Inventor will match the names of the iMates or Composites together and create assembly constraints between the components. Your components will automatically snap into place. Figure 3. If you've added iMates to your library of parts, be sure to use the Use iMate checkbox when placing a component. The iMates on the component will automatically assemble to any matching iMates in the assembly, essentially snapping you components into place upon insertion.

Conclusion Autodesk Inventor allows you to capture your design intent and leverage the intellectual capital in your models to create better designs. Leveraging this intellectual capital ensures that the design and process knowledge that resides in one designer's mind can be accessed and used by multiple designers.