Today we continue our discussion on using BOMs in SolidWorks 2008. Be sure you go back and read my previous post Creating Your BOM Template and Using BOMs in SolidWorks 2008 before reading on. I would also highly recommend Josh’s coverage of BOM at SolidSmack, SolidWorks BOM Superstar: 5 Moves to Avoid and How to Groove It.  Today we’ll dig more into the changes to BOMs in 2008 and we will even answer the question I hear most often: “What happen to the BOM Content command?”

Add Balloons to Drawing

Today I won’t spend too much time on adding balloons, or item identifiers, to the drawing. We will save that for a different day and a different post. Since this is a real simple assembly we can just go with the AutoBalloon tool in the Annotations toolbar.

Clicking our isometric view we now have balloons attached for all the components… or do we?

Where is the BOM Content Command?

Previous to SolidWorks 2008, you were able to click the BOM Content button in the PropertyManager for the select BOM. The BOM Content window allowed you to view the components in your BOM, see what components are missing balloons, see the type of components listed or reorder the items in your BOM. All that functionality is still available but instead of being a separate window it is now part of the BOM itself.

Viewing the Balloon Status and Assembly Structure

One of the functionality of the original BOM Content window was viewing the Balloon Status and Assembly Structure. Now you can view these directly in the BOM, nice and easy. Click the expansion arrows on the side of the BOM, the tree tiny little arrows pointing out from the BOM, and addition columns will be show.

In this view, we can quickly see which components have balloons attached to them. If we missed any, we should go back and make sure they are added. In this view we can also see the assembly structure. Since we currently have our BOM to show only parts we only see part icons with no real structure.

If our assembly was set to Indented Assemblies we would be able to see the full structure along with the component type icons.

Reordering the BOM

Another functionality that was originally available in the BOM Content window was the ability to reorder the BOM. I am personally glad that SolidWorks got rid of the window since now you can reorder the BOM in the BOM. How cool is that? It couldn’t be any easier, select the entire row at the row number…

…and drag the row to the desired location. Too cool!

Of course you cannot change the order of the BOM when you have Follow Assembly Order selected in the right-click menu. When you select Follow Assembly Order the only way to change the order of the components in the BOM is to reorder the assembly structure.

Splitting the BOM

As your BOM grows, it may become too large to fit vertically in your drawing. In this case, you want to split the BOM and move the second part somewhere else in the sheet or even another sheet. In the BOM select the row where you wish to apply the split and right-click. Select Split from the menu and select one of the options; Horizontally Above, Horizontally Below, Vertically Left or Vertically Right.

You can now drag the second section of the BOM anywhere you want. You can even use Cut and Paste to place it onto another sheet and it will remain linked.

To combine the two BOMs back into one, select Merge Tables from the right-click menu.

Insert a New Part

You can now add new parts directly from the BOM using Virtual Components. First, right-click the BOM and select Insert New Part.

This will insert in a blank line into your BOM. IF you expand the BOM you will see that new item is a Virtual Component shown with brackets, [ ].

In your assembly you will see the new virtual component added to the FeatureManager. We will be covering Virtual Components at a later date.

I hope you will find, after reading this, BOMs extremely helpful and easy to use. I encourage you to explore BOMs more in the future since there are more tools built into the BOM. If you enjoyed this post and all the other Tips and Tricks I offer here at The SolidWorks Geek, please subscribe to my RSS feed and you might just win our contest.

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