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Autodesk Inventor Displaying Parameters in BOMs and Parts Lists

By Jesus Robertson,2014-11-29 03:35
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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 Inventor? 4, you can specify that the model parameterssketch dimensions, extrusion lengths, assembly constraint offsets, and so onbe 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)

     Figure 1: Appearance of assembly on opening.

    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:

    1. Extract the files to a folder on your hard drive. 2. Start Autodesk Inventor software. 3. Click Open on the Standard toolbar. 4. Browse to the folder containing the extracted files. 5. Select Frame.iam. 6. Click OK. The assembly should look like the one shown in Figure 1.

     Figure 2: Length as driven dimension.

    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.

    Note: The length of the diagonal brace is a driven dimension (see Figure 2). This allows the length of the part to adapt, while the driven dimension value is stored as a reference parameter that can be used in equations, or displayed in a parts list.

     Figure 3: Revised parameter name.

    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).

     Figure 4: Export parameter checked.

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

    Note: This action copies the parameter to the part's custom properties. Custom properties can be displayed in BOMs and parts lists. Although they are visible in the custom properties list, you cannot edit the name or value of these exported parameters outside the parameters dialog box. 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.

     View Larger Image Figure 5: Frame.idw on opening.

    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 .

     Figure 6: Field matches parameter name.

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

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

     Figure 7: Length column reflects parts parameters.

    Note: The field name must match the spelling of the parameter to be shown, but it is not case-sensitive. 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).

     Figure 8: Adjusting mate offset.

     Figure 9: Out-of-date parameter.

    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.

    Note: The parts list is unchanged. You must update the parts list to reflect any changes in the model properties. 2. Double-click the parts list.

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

    Note: The length of the Support is marked as being out of date (see Figure 9). Both the Support and Diagonal frame members changed length to adapt to the new offset value of the constraint. Note that the Length value for the Diagonal member is not marked as being out of date. (More on that in a minute.)

    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).

     Figure 10: Edit-driven dimension.

     Figure 11: Out-of-date parameter for driven dimension.

    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.

     Figure 12: Updated length parameter.

    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).

     Figure 13: Up-to-date parts list.

    6. Click OK.

    Note: The parts list reflects the length of the parts in the revised frame.

    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.

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