Working with Parts or Assembly BOMs

After creating a part or assembly BOM, you can open assembly BOMs in a separate window from the assembly view, export assembly BOMs into different formats, and copy an assembly BOM into a referenced drawing.

Opening Assembly BOMs in a New Window

To open assembly BOMs in a separate window:

  1. Right-click the BOM in the FeatureManager design tree.
  2. Select Show Table in New Window.
You can modify the BOM in the new Window. When you close the window, the BOM appears in the graphics area with the assembly.

Exporting Assembly BOMs

After creating an assembly BOM, you can right-click the BOM and:
  • Save it in a variety of formats including:
    • Template (.sldbomtbt)
    • Excel (.xls or .xlsx)
    • Text (.txt)
    • Comma-separated values (.csv)
    • Drawing interchange format (.dxf)
    • Drawing (.dwg) file
    • eDrawings (.edrw)
    • Portable document format (.pdf)
  • Print it.

Copying Assembly BOMs into Drawings

You can insert a BOM saved with an assembly document into a referenced drawing.

To insert a BOM saved with an assembly into a referenced drawing:

  1. Select Insert > Tables > Bill of Materials.
  2. In BOM Options, select Copy existing table.
  3. Select an assembly BOM from the list.
  4. Select Linked to link the BOMs.

Linked BOMs have certain parameters and restrictions. You can edit the original assembly BOM or the copied drawing BOMs. Changes in one BOM update the other BOM. Formatting of linked BOMs is independent; only the data is linked. Formatting items include row height, column width, font size and color, and text direction.

You can unlink the drawing and assembly BOMs at any time, but you cannot reestablish the link. You need to create a new BOM to re-link the BOMs.