Avatech Tricks: Parametric Design Using Inventor Part Files

15 Jul, 2005 By: John Hackney Cadalyst

Link and parametrically drive your assembly and part models using an Inventor part file

When you need a parametrically driven assembly, your first thought is probably to link it to a Microsoft Excel spreadsheet. This solution is viable, but the efficiency and dependability of linking Excel to Inventor files can be problematic. This tech tip will show you how to link and parametrically drive both your assembly and part models using an Inventor part file, eliminating the need to use Excel.

I'm using an example of a roller conveyor section that contains a sheet metal conveyor pan as one part (figure 1). I will demonstrate the connection of the parameter part file with the roller conveyor section assembly and conveyor pan. I will not describe the procedures to connect the parameter part file to other parts, but you can use same method.

Figure 1. The original roller conveyor section with a length of 21 in.

The controlling part file does not contain any geometry, only the user parameters in the Parameter table. You can set up these parameters before or during the development of the individual conveyor part models and the conveyor assembly model. In this example, I used both. I assigned user parameters for the various required part and assembly sketches, features and constraints in the Parameter table. You can export the user parameters assigned to the assembly and part models by checking the box in the Export Parameter column.

In developing the conveyor pan, first derive the parametric file into the part file. In the Derived Part dialog box, select only to use the exported parameters (figure 2).

Figure 2. When the derived part is placed into the Inventor part file, only the parameters are selected.

Next, develop the part model features using the derived parameters in place of numerical entries in sketches and feature development. You can select derived parameters directly from the List Parameter dialog box (figure 3).

Figure 3. When you create sketches and features, select Controlling Parameters from the Parameter table.

Use the Link function at the bottom of the Parameter table to establish the assembly model link to the parametric part file. The assembly constraints and feature values are taken from the linked part file (figure 4). After everything is saved and debugged, it is time to test the assembly.

Figure 4. You can link the parametric part file to the assembly drawing by using the Link button at the bottom of the Parametric table.

This example was developed so a change in the length parameter of the parameter part file will make all required changes for the assembly. The original length of the conveyor pan was 21 in., and it had four roller assemblies. Opening the parameter table in the parameter part file, I changed to length to 36 in. and clicked done (figure 5).

Figure 5. Change the length in the parametric part's Parameter table to update all parts and assemblies.

Immediately the Update icon flashes on. Switching to the conveyor assembly, select the Update icon to bring the assembly and parts into full compliance (figure 6).

Figure 6. The roller conveyor section updated to 36 in. in length.

The speed and dependability of using an Inventor part as the controller of parametric design makes it a good choice in your design. This method is not intended to replace Excel in the design of parametric parts; it is just a great alternative.

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About the Author: John Hackney

John Hackney

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