Welcome back to a new week filled with SolidWorks tips and tricks. Over the next couple of post we’ll be concentrating on SolidWorks Bill of Materials. SolidWorks 2008 brought some changes on how one uses BOMs in the drawing environment. A lot of the controls for BOMs that were previously available in the PropertyManager are now available in the BOM. Using the BOM template we created last week on Creating Your BOM Template with a few further tweaks, we will go over the changes that applies to BOMs in 2008. Feel free to use any BOM template you choose since there is nothing custom about what we are going to do today.

Inserting BOM into Drawing

To insert a BOM into a drawing click Tables -> Bill of Materials in the Annotations toolbar. I use the Shortcut Bar almost exclusively, to bring up the shortcut bar select ‘S‘ on your keyboard. For more about Shortcut Bars refer to: Improve Productivity – Use Shortcut Bars.

After clicking the Bill of Materials button you will be prompted to “Select a drawing view to specify the model for creating a Bill of Materials.“. You may select any view but I would recommend select the primary view in your drawing, usually the isometric will work. What ever configuration and display state is shown in the view will be used to populate the BOM.

After selecting the view used to populate the BOM you will be prompted to select the options for the BOM. We covered all of the options last week, feel free to go back before continuing on.

Once all your options have been set, click the green check mark to insert your BOM into the drawing.

Make Sure Your BOM is Properly Filled Out

You will notice in the example below that all of the fields are not properly filled out. Depending on how your BOM template was created, all of your cells should be populated from the part properties. Of course you can always go back into the original parts and fill out the all of the appropriate Custom Properties, but as of SolidWorks 2008 that is no longer necessary. All of the cells that are linked to the custom properties of a part are now bi-directional. This means that information can be added in either the part file or the BOM and it will be updated in both.

When you double-click on a cell to edit the information you will be prompted with the following alert box. Clicking Keep Link will allow the updates you make to the BOM to also be made to the part file. Clicking the Break Link button will make the changes only to the BOM and any further changes to the property of the part will not be made to the BOM. I highly recommend you select Keep Link since any and all changes made to the part will be be directly reflected in your BOM.

Don’t Know What an Item is?

Sometimes, if you have no properties filled out for an item and you have no item identifiers in the drawing, you may not know what line of the BOM goes to which part. In these cases you can give yourself a little hint as to which item is being referenced by the BOM line. Right-click the row or a cell in the row to view the menu.

In the right-click menu you have the ability to open the referenced part, this command Open also has the file name of the part. Without opening the part you will get a hint as to how to proceed with filling out the row information.

If all steps were followed properly, we have filled out our BOM and the part properties have been updated as well.

Table Cell, Row or Column Toolbars

As of 2008, instead of using the PropertyManager to update the BOM cells, rows or column; a context toolbar is used to update the BOM contents. Click anywhere inside of your BOM you will see the context toolbar.

Adjusting Fonts

By default, the cells in your BOM should be set to Use document font. I always tell my users to make sure that Use document font is enable at all times, not just for BOMs but for notes and dimensions as well, since it allows for font changes to be made globally.

When the Use document font option is enabled, you can globally update the font in the Document Properties. First, click the Options button in your Standard Toolbar.

Then, select Annotations Font -> Tables to access the Choose Font window. Here any adjustments to the font will update all the cells that have been set to Use document font. For those who use it, the Design Checker excels in this area since it checks to make sure that the document fonts match your company standards, but that is a different post.

If you do want to change the font of a cell manually, deselect the Use document font button in the toolbar. The toolbar will expand to include the standard information for adjusting fonts. Be forewarned, any changes you make to the Document Properties will not be made to cells that are next set to Use document font.

Fit Text

One of the new features in SolidWorks 2008 is the addition of the Fit Text tool. Click the Fit Text button overrides the document font for the specified cell and automatically adjusts the font to fit the entire string in the cell.

The text in the cell, rather then getting scaled down, actually gets condensed to fit on one line. Since the Use document font option is overridden the toolbar expands to include the font information.

Adding Equations

On the toolbar you will see a equation symbol. Clicking this symbol opens the Equation toolbar.

In the Equation toolbar you can create simple equations for quantities, create simple conditions statements, even adjust the property a cell or column points references.

Adjust Cell Padding

Cell Padding refers to the space between the border of the cell and text. In the toolbar you can adjust the cell padding of the entire row, column or just cell.

Hide/Show Rows or Columns

In the toolbar, you have the ability to hide or show entire rows or columns.

This tool works much like the Hide/Show Annotations command. When you click the Hide/Show button your mouse pointer will change to indicate that the command is active. Click the rows and/or columns you wish to be hidden, the entire row will be highlighted.

Click the Hide/Show button once again and the selected rows and/or columns will be hidden from view. The items numbers will not be renumbered, instead if you hide a row in the middle of the BOM the item number will be skipped.

To show the hidden rows once again, click the button once more and deselect the rows you wish to be displayed once again.

Group/ungroup selected rows

The Group/ungroup button allows you two group two more more items in the BOM. When items are grouped they share the same item number. To group rows, select two or more rows and the button will become active in the toolbar.

Clicking the Group/ungroup buttons changes the items numbers of the rows to be the same number. To ungroup,  select the rows and click the button once again.

Well that’s it for today, I don’t want your head to explode with too much information in one post. Later this week I will be covering more BOM usage. So until then, Have fun with SolidWorks and as always feel free to contact me with any questions and/or problems you may have.

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