Autodesk Inventor: Displaying Parameters in BOMs and Parts Lists

Autodesk Inventor: Displaying Parameters in BOMs and Parts Lists

By Neil Munro

This month's tutorial is a quick exercise on displaying model parameters in BOMs (bills of materials) and part lists. In Autodesk InventorT 4, you can 24524f521y specify that the model parameters-sketch dimensions, extrusion lengths, assembly constraint offsets, and so on-be made available as columns in assembly BOMs and drawing parts lists. Unfortunately, the steps to accomplish this are not well-documented in the Help system. We'll remedy that with a simple tutorial, and show a workaround currently required for parameters associated with driven dimensions.

Download and Open File
First download, unzip, and save to a folder on your hard drive the Parameters.zip file.

Parameters (zip - 317 Kb)

The zipped file contains the following:

           Frame.iam (assembly file)

           Frame.idv (design views file)

           Rail.ipt Support.ipt

           Diagonal.ipt

           Frame.idw (assembly drawing file)

To open the file:

Extract the files to a folder on your hard drive.

Start Autodesk Inventor software.

Click Open on the Standard toolbar.

Browse to the folder containing the extracted files.

Select Frame.iam.

Click OK. The assembly should look like the one shown in Figure 1.

Capturing Component Lengths
The brown supports and the yellow diagonal frame brace are adaptive, while the green rails are not. We want to capture the length of each frame component in the assembly drawing's parts list.

Modifying Parameter Names
We need to assign a common name to the model parameter of each frame member that describes its length. We can then expose this parameter in a parts list or BOM.

1. In the browser:

           Right-click Diagonal.ipt and select Edit from the pop-up menu.

           Right-click Extrusion1 and select Edit Sketch.

2. On the Command toolbar, click Return  to exit the sketch.

3. From the Standard toolbar, click Parameters . The parameters for Diagonal.ipt are shown.

4. Under Reference Parameters, click the cell containing d0. Enter Length as the new parameter name (Figure 3).

5. Click the Export Parameters checkbox next to the Length parameter (see Figure 4).

6. Click Done.

7. Right-click and select Finish Edit.

You can edit the Support and Rail parts and examine their parameters. A Length parameter (along with others) has been defined and exported for the rail and support parts.

Parameters In a Parts List
Now that we have a common parameter name, we can add a column to a parts list to display the length of each frame member.

1. Open Frame.idw.

2. Double-click the parts list above the drawing view.

3. In the Edit Parts List dialog box, click the Column Chooser tool

4. In the Parts List Column Chooser dialog box, click the New Field button.

5. Enter Length in the Name edit box (Figure 6).

6. Click OK.

7. In the Edit Parts List dialog box, click Description in the Selected Properties list and click the Remove button.

8. Click OK. The parts list should match the one shown in Figure 7.

9. Click OK to close the Edit Parts List dialog box.

Edit Assembly
1. Return to Frame.iam (reopen it if you closed it).

2. Expand Rail.ipt:1 in the browser and click the Adjust Me (18.000 in) assembly constraint.

3. Enter 30 as the new value for the mate offset between the two rails (see Figure 8).

4. Save Frame.iam.

Updated Parts List
The drawing parts list must reflect the length of the revised frame supports and diagonal brace.

1. Return to Frame.idw.

2. Double-click the parts list.

3. In the Edit Parts List dialog box, click the Compare tool

4. Right-click the yellow Length cell and select Update value from the pop-up menu.

5. The cell reflects the 30 in length of the revised supports.

6. Click OK.

Updating Driven Sketch Dimensions
The Length parameter of the Diagonal frame member is a driven dimension, and a workaround is currently required to update parameters from driven dimensions. But: in the prerelease versions of Autodesk Inventor 5 that I've seen, driven dimensions will update without the workaround.

1. Return to Frame.iam.

2. In the browser, right-click Diagonal.ipt and select Edit.

3. Right-click Extrusion1 and select Edit Sketch.

4. Double-click the 32.187 in Dimension.

5. Click the green check mark in the Dimension edit box (see Figure 10).

6. Right-click and select Finish Sketch.

7. Right-click and select Finish Edit.

Update Parts List
1. Return to Frame.idw.

2. Double-click the parts list.

3. In the Edit Parts List dialog box, click the Compare tool  (Figure 11). The Length parameter of the Diagonal frame member is now recognized as being out-of-date.

4. Right-click the yellow Length cell and select Update value.

5. The cell reflects the 32.187 in length of the diagonal brace (see Figure 12).

6. Click OK.

Summary Using named model parameters is an efficient method for capturing model data. Assigning logical names to important model dimensions and parameters can improve the readability of your designs, and allow you to capture design data in assembly BOMs and drawing parts lists.

I'd like to credit Quinn Zander, an Autodesk Inventor Newsgroup regular, for identifying the workaround for updating driven-dimension values.