As I had mentioned in my previous post, by the time I was finished with this little piece of fence, I had already collected twenty five bodies that appeared listed under “cut list” in the Feature Manager. How can this cut list be used as a mean to convey information about the model? Well, first of all, it needs to be updated, which means that all the members in the weldment that are similar will be grouped together in folders. In order to do this, right click on Cut List in the Feature Manager and select Update.

As a result of updating the cut list, we now have six different folders of cut list items, each containing the members of the weldment that are the same. Notice that the number in parenthesis indicates the amount of items in each folder. Placing the cursor over the name of each folder or item lets you see which item it is in the graphic area.

The next step is to customize the cut list, so it can become really useful for us. The first thing we may want to do is to give each item in the cut list a more meaningful name by renaming the folders, like I’ve done in the image. To rename the folders simply click on their names once, wait a bit and click again, then the text will show up inside a white box and you’ll be able to delete the old name and write your own.

Once we’ve renamed the items, we now proceed to customize the properties of the items as we want them to appear in the cut list. Right click on any of the item’s name (the names of the folders) and select properties. This opens the following window. As you can see, Length and Angles have already been assigned and calculated by SolidWorks. To add another property to the list, click on an empty cell under Property Name and select from the different options, in this case I selected Description, to add a short name to identify the item.  Notice that whenever you use a weldment profile supplied with SolidWorks, there’s usually already a Description of the item, inherited from the profile. In my case, I didn’t have a description for my profile, so I’m adding one this way, instead.

On the corresponding cell, under Value/Text Expression, I wrote the short name/description that I wanted to associate with that item.  I could’ve also linked this value to a dimension in the weldment profile, for instance, by double clicking on the dimension in the graphics area. The Evaluated Value shows the way this information will appear in the cut list when you add it to a drawing document. It is also possible to add other properties, like Weight, Volume or Surface Area and let SolidWorks calculate them for you.

After adding all the properties to every item on the cut list, it is finally ready to be inserted in a drawing document. In the drawing document, select the view that will be associated with the cut list, then click Insert, Tables, Weldments Cut List.

A property manager will show up. It allows you to customize a thing or two about how the cut list is displayed in the document.

After you are done customizing, click OK and drag the table to wherever you want to position it on the sheet.

Finally, you can change the size of the table by dragging its corners, just like you would do with any other window. Notice how all the properties we specified appear in the table, except for the Angles.

I must admit that this is not precisely what I had in mind when I first heard about weldments in SolidWorks. I actually thought that it would be like a representation of the different kind of welds, but all I’ve seen on that is the Fillet Weld. It doesn’t matter; I think this way makes a lot more sense.