In our continued dive into bills of materials, today I dive deep into the Inventor Bills of Materials (BOM).
The Autodesk help describes the bill of materials as “a table that contains information about the parts within an assembly. The table includes quantities, names, costs, vendors, or any other information someone building the assembly needs. Quantities on the bill of materials are updated when a part is added or removed from the assembly.”
It starts with iProperties
As the Inventor Bills of Materials is a listing of the components contained within the assembly. The assembly stores some BOM information (quantities) but the majority is controlled via iProperties. What are iProperties? The metadata describing each component, like the description and part number.
Not only can the iProperty information be viewed from the BOM, but also be edited. Using the BOM can be a very efficient method of modifying iProperty information quickly. And not only on one component, but multiple components as well.
Within Inventor, quantity can be shown in different ways. This includes item quantity, unit quantity, and total quantity. Every component contains a Base Quantity and Base Unit, which defines how the quantity appears in the BOM (and subsequent drawing Parts List). You set this within the Document Settings of the part.
By default, the Base Quantity is Each, meaning the BOM lists the number of instances in the assembly. You adjust the Base quantity to represent a different parameter and a different unit of measure (UOM). For example, the length of the component. The selected parameter value appears in the BOM and always reflects the current value of the parameter.
Within the BOM you can add additional types of quantity. Item Qty always shows the number of instances of the component, regardless of its base value. Unit Qty shows the base quantity of one instance of the component.
Using the BOM Editor
As the Inventor bills of materials is a listing of the components in the assembly, it makes sense you access the BOM from the assembly environment. The BOM dialog displays 3-tabs: Model Data, Structured, and Parts Only.
- Model Data displaying all components, regardless the structure applied
- Parts Only listing just parts – no subassemblies or assembly structure. All parts promote to the top creating a flat view
- Structured showing a view of the assembly hierarchy. Expand subassemblies to display their children.
Within the editor, drag-and-drop columns to locate in the desired position. Use the Column Chooser to add additional iProperty columns. Click on a column header to sort by that column.
The initial listing is in the order the components were created or placed in the assembly. Drag rows to reorder or use the sort function to sort the data by a combination of iProperties. Once sorted use the renumbering feature to sequentially set the item numbers.
When in doubt, right-click. The right-click menu provides many options including Find & Replace, Capitalize, and the option to open components into their own window.
A Virtual Component is a special type of component that contains no geometry and acts as a placeholder for iProperties. As there is no geometry, no new files are generated. Virtual Components appear and behave in the BOM like a regular component and contain the full set of iProperties.
Components in an assembly with the same part number automatically merge into a single BOM line. If not desired, disable this with the Part Number Row Merge Settings. If iProperties of the combined items do not match, the BOM reports “varies”.
This is useful when creating bills of materials for parts with the same profiles but different lengths. By giving them the same part number they merge, providing the total length of material required. Or when you have the same part model in different configurations (think a spring) but do not need multiple lines for the quantity.
Each Model State supports unique iProperties, Parameters, and Bill of Materials. A suppressed component does not participate in the Bill of Materials. So the active Model State controls what you will see within the BOM.
New to Inventor 2022 is Instance Properties. Take a look at this article to see how this can impact the BOM.
Use Structure to create BOMs truly representing the assembly. You set structure from the Document Settings, iProperties Occurrence tab, or within the BOM Editor (Model tab). Set Reference additionally from the browser right-click menu.
- Normal (the default) sets your parts and subassemblies to appear as is in both the Structured and Parts Only list
- Use Phantom with subassemblies to group components into assemblies, but the subassembly itself is not required to be shown in the BOM. As assemblies do not appear in the Part-Only view, this only impacts the Structured where the children components promote into the view in place of the assembly.
- Purchased is for those components bought and not manufactured. They list as a single line in the Parts Only even when an assembly
- Reference is for components placed into the assembly for the sole purpose of construction. These components (both parts & assemblies) do NOT appear in the BOM (parts only or structured). Reference components are not included in mass calculations. They can be displayed differently in the drawing environment
- Inseparable is intended for subassemblies (like weldments) to be treated as a single part. They list as a single line item in the parts-only view UNLESS the child component is purchased, which will be promoted.
Purchased and Inseparable are similar. The difference, a purchased assembly never promotes children to the top. This is useful when wanting to model the individual components but the unit is bought as one item. Use Inseparable with items like weldments that need to behave as a single item once completed. However, purchased items promote to the top. We don’t want purchasing to miss them, right?
The Inventor Bills of Materials is the listing of components contained within the assembly. To display this information within a drawing, insert a Parts List. Think of the Parts List as a snapshot of the BOM showing only the information relevant to the drawing. Tweak the Parts List details to override it specifically for the drawing. Changes made to the BOM (or component iProperties) reflect in the parts list.
Within the Parts List, you can group items based on “keys” which represent the component iProperties. For example, with frame generator assemblies you can group items based on their Stock Number (First Key) and (Base Qty) which will group items based on their material type and component length.
A drawing view is NOT required to create a parts list. When placing the parts list you need to select an assembly (or Presentation file .ipn). Specify the assembly by browsing, selecting from the list of currently open documents, or selecting an existing drawing view. Manage the parts list format via the drawing’s styles.
Feature image transformer by Chris Yarzab