Inventor automates the heck out of making BOMs
The bill of materials (BOM) is an important communication component for manufacturing. It is a list of parts. You could say it has all the ingredients for producing the equipment and machinery you design. It lists the material, sub-assemblies, purchased items and everything else that goes into the product.
Inventor’s bill of materials forms a table. It holds information about the components contained within an assembly. Information including part numbers, descriptions, quantities and other key details. It’s really all the information someone building the component needs.
As you add components to an assembly, these add to the BOM. Quantities update when adding or removing a part from the assembly. This is done by iProperties which is in charge of the component details. What is a iProperty? It is any of the metadata describing a component such as the description and part number.
Using the bill of materials editor
Access the BOM Editor from the Assemble ribbon tab.
The BOM Editor shows three-tabs: Model Data, Structured and Parts Only.
The Model Data tab lists all the assembly’s components, regardless of their structure. This is equal to the assembly browser without the item numbers.
Within the editor, click a column header to sort by that column. Drag-and-drop a header to reposition the column. Drag a column header below the heading to remove it from the table.
Use the Column Chooser to add iProperties columns.
Not only can you view iProperties information from the BOM, but it can also be edited. Using the BOM editor is an efficient method of changing the iProperties of multiple components. Changes made with the BOM Editor are written back to the source file.
As you select rows in the BOM Editor, the corresponding component highlights in the graphics window, making it easy to check that you are editing the right component.
Use Add Custom iProperties Columns to add a custom iProperty to the table. iProperties can be created with types of Text, Date, Number or with a Yes or No. When accepting the changes to the BOM, Inventor writes the new iProperty to all components within the assembly.
The right-click menu provides many options including Find & Replace, Capitalize and the option to open components into their own window.
The Structured and Parts Only tabs may be disabled initially. Use the View Options to enable the tab.
The Structured tab shows the assembly hierarchy. The available level of detail is set by the View Properties. You can choose to show only the first level or to show all levels. Expand subassemblies to display their children.
The Parts Only tab is just that, a listing of just parts – no subassemblies or assembly structure. All parts are promoted to the top creating a flat view.
Use the View Properties to set the item number formatting and the minimum number of digits.
The initial component listing is in the order the components were created or placed into the assembly. You can drag rows to reorder them or use the sort function to organize the data by a combination of iProperties. Once sorted, use the renumbering feature to sequentially set the item numbers.
A virtual component is a component containing no geometry. It acts as a placeholder for iProperties. As there is no geometry, Inventor creates no new files. Virtual Components behave in the BOM like other components with a full set of iProperties.
From the BOM Editor, you can create new virtual components. After setting the component’s name you can edit its iProperties within the table. The new virtual component adds to the bottom of the Model browser view.
You can export the Structured and Parts Only BOM views.
From the Export Bill of Materials dialog, select the view to export. If exporting the structured view, additionally select the hierarchy structure to include.
Then from the BOM Export dialog set the file name and the data format. Inventor allows you to export to Microsoft Excel (.xlsx and .xls), tab-delimited text (.txt) and to CSV.
Component equivalence
By default, Inventor rolls up components with the same part number into a single BOM line. If iProperties of the combined items do not match, the BOM reports “varies.”
You might be asking, why do I want this? This can be useful for parts with the same profile but different lengths. By giving them the same part number so they merge, it provides the total length of material required.
Or you may have the same component but in different configurations, like a spring. You need different models, but you do not need multiple lines in the BOM.
If the merging is not desired or not needed, disable this feature with the Part Number Row Merge Settings.
Instance properties
Instance properties are iProperties assigned to specific instances within an assembly. This property information is not written back to the file but stored in the parent assembly. This allows you to change the iProperties for one instance but leave all other instances as is.
Within the BOM, Instance Properties appear in custom iProperties columns. Inventor shows the overridden property values in blue.
The Model Data tab always displays all components with instance property overrides. By default, Inventor merges instance rows as it does with those with the same part numbers. To separate the instances, uncheck Merge Instance Rows in the Part Number Row Merge Settings dialog.
Quantity
Not all quantities are the same. Within Inventor you can show quantity in different ways.
Every component contains a base quantity and base unit. This defines how the quantity appears in the BOM. 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. However, you can change this to use a parameter with different units of measure (UOM). For example, a parameter representing the length of the part could be in inches, millimeters, feet or any length unit.
In the BOM, the Unit Qty shows the base quantity of one instance of the component. Item quantity always shows the number of instances of the component, regardless of its base value. It is a read-only property and cannot be changed manually but can be overridden.
Total Quantity is the Unit QTY multiplied by the Item QTY.
In this example the Hex Bolt has a base quantity of each. As there are four in the assembly the QTY and Item QTY are both 4. The pipe has a base unit of inches. As the pipe is 52.5” long (Unit Qty) and there are two in the assembly (Item QTY) it makes for a (Total) QTY of 105”.
Because of the part number merging the same type of tubing but of different lengths are merged into a single row. This is why the Unit QTY varies, but Inventor still reports the total quantity.
Model States and suppression
Model States support unique iProperties, parameters and component suppression. This means each state could produce a different BOM.
A suppressed component does not participate in the Bill of Materials. If all instances of the component are suppressed the component appears in the BOM as a zero quantity.
To hide zero quantity items from the BOM display, use the BOM Settings and enable Hide Suppressed components in BOM.
Additionally, consider whether you want the items to renumber automatically. For some it is important that the part keeps the same item number even if it means gaps in the sequence.
Structure
Structure is important in making the BOM represent your design intent.
You set the structure in the Document Settings, iProperties Occurrence tab or within the BOM Editor (Model tab). The state applies to the component, meaning all instances use the same structure.
The exception is Reference, which can be set on specific instances.
The Normal structure type is the default and is what you will use for most of your components. With normal, the components appear as-is in both the Structured and Parts Only lists.
Purchased is for those components you buy and do not manufacture. When applied, components list as a single line in the Parts Only view even when they are assemblies. This is useful when there are benefits to having an assembly with individual components to manipulate, but it is purchased as a single item.
Inseparable is like Purchased. The difference? Inventor never promotes children within a purchased assembly. With Inseparable, Inventor promotes Purchased children to the top so they list in the Parts Only view. Use Inseparable with items like weldments that behave as a single item once completed. However, you do not want purchasing to miss buying the needed parts.
Use Phantom when you use assemblies to group components but do not want the assembly itself to appear in the BOM. As assemblies do not appear in the Part-Only view, this only impacts the Structured view as Inventor promotes the children’s components into the view in place of the assembly.
Reference is for components used to aid construction. These components (both parts and assemblies) do not appear in the BOM (parts only or structured). They are not included in mass calculations. They can be displayed differently in the drawing environment.
Vault Professional honours the structure when creating items. For example, it will create a single item for purchased assemblies, ignoring the assembly’s children components.
Drawings
A parts list is the drawing equivalent of a bill of material. It is a snapshot of the BOM, configured with the iProperties and BOM information you want shown in the drawing. Changes made to the BOM or to component iProperties reflect in the parts list.
A drawing view is not needed to create a parts list. When placing the parts list you need to select an assembly (or presentation). 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.
Tweak the Parts List to present the information specifically for the drawing. This includes selecting columns (iProperties), modifying the table layout, adding custom parts and substituting the sum of one property’s values into another field.
You can also turn rows off and override iProperties details. Turned off rows appear in grey and overridden iProperties in blue.
Apply filters to show only the required components. Filters affect row visibility but do not adjust the part data (quantity stays unchanged).
As with the BOM, you can sort the list by any of the visible columns. Then renumber the items to be sequential. With the parts list the renumbering applies static overrides, making the item numbers different than those in the BOM. Use the Save Item Overrides to BOM right-click feature to write that item number back to the BOM.
You can group items based on keys. 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.
