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Inventor

Add Reference Components to Your Assemblies

15 Aug, 2004 By: Kevin Schneider

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Inventor eliminates the worry that they'll show up in drawings down the line

How many times have you wanted to add a part to a design to help you size and position other elements, but hesitated because you didn't want that part to show up later in the drawing or the bill of materials or the parts list? The part might be a construction part, a layout, or truly "for reference only," and not a component of the final product. Fortunately, Autodesk Inventor offers an automatic way to add reference elements without the risk of passing them on to the manufacturing team.

Reference Components in Assemblies
Decide which components in your assembly you want as reference parts. The example assembly in figure 1 has two tubes to which an adjustable bracket mounts. We'll designate these tubes as reference parts.

Select the desired components in the browser and right-mouse click to display the context menu. Select Properties (figure 2).

Next, go to the Occurrence tab and check Reference (figure 3). You can specify parts, subassemblies, or a mix of both as reference items. When you designate a subassembly as a reference, Inventor treats all components inside it as reference parts.

Inventor now treats the components differently-for example:

• It ignores reference components when calculating the assembly's CG (center of gravity).
• It ignores reference components when it creates the assembly bill of materials.

Reference Components in Drawings
Inventor offers several options for placing a 2D assembly drawing view that contains reference components.

To create a new drawing, start by making a base view of the assembly that contains reference components. In the Create View dialog box, choose the Options tab (figure 4).

Figure 5. Control the display of the reference assembly.

Select from three display options for the reference components, as well as options to control the view-clipping boundary, or margin (figure 5). Increasing or decreasing the margin displays more or less reference data.

By default, reference component view geometry is displayed using the As Reference Parts option. Inventor automatically places this geometry on a layer called Reference. This layer has the thin lineweight of 0.7mm and the line type Double Dash Dot. To change the lineweight, color, or style, simply edit that aspect. To automatically put geometry on a layer of your own making, edit the object defaults for your standard and select the layer you want to use instead. Use the object default filter called Model/View Objects to more easily find the Reference Part Edge setting (figure 6).

You also can display components by using the As Parts option. This setting places the geometry of the reference components on the same layer as the other visible parts in the design. The reference parts appear just like any other part in the assembly view. Alternatively, choose Off to hide all reference parts in the view (figure 7).

Using reference parts adds powerful display options to design views, but avoids the risk that those parts will show up on the drawing's parts list. Reference components can make it easier to create designs and share them with others, knowing all the while that the system won't incorporate those reference elements into production drawings. When a design requires reference components, Inventor makes the job fast, easy, and automatic.