Altium Designer Documentation

Including Design Data in the Excel BOM

Modified by Phil Loughhead on Aug 28, 2019

A common approach to BOM generation is to export the BOM data from Altium Designer, into a company-preferred Excel format spreadsheet. The BOM is generated from the Report Manager, which can be accessed from:

  • ActiveBOM's Report menu
  • The schematic and PCB editor's Report menu
  • A BOM Report Output configured in an OutputJob
  • Learn more about BOM Configuration in the Report Manager.
  • For complete control over the BOM configuration process, including an interactive view of supply chain information as well as custom BOM rows and columns, add an ActiveBOM document (BomDoc) to your project. The BomDoc gives instant visibility into the component supply chain and also supports user-defined rows and columns, ideal for including those extra items, such as glue, labels, and so on. Creating and managing the BOM through a BomDoc is the recommended approach to BOM Management in Altium Designer.

The Report Manager's Export Options includes two XLS File Format options:

  • MS Excel File - Native (*.xls, *.xlsx) - requires Microsoft Excel
  • MS Excel File (*.xls, *.xlsx) - uses a built-in XLS file generator, Microsoft Excel is not required

Select the required Excel file format option, then select the required Excel template

When an Excel option is selected a pre-defined Excel template can then be selected in the Template dropdown. When the Export button is clicked in the Report Manager the BOM data is generated and loaded into a new Excel Worksheet, using the format defined in the chosen Excel template.

The list of templates available in the drop down comes from:

  • For an unmanaged design, the default location is configured in the Data Management - Templates page of the Preferences dialog. Several example templates are included, in the \Templates folder of the installation user-files.
  • For a managed design, the available templates are stored in the \Templates\BOM Templates folder of your managed content server.

How Design Data is Mapped in the Excel Template

Altium Designer data is mapped into the spreadsheet by including special Field and Column statements in the Excel template. The Field statement is used to map a single parameter, for example a document parameter called Title. The Column statement is used to map per-component parameters, for example the Designator component parameter.

Fields

The Field statement is used to map a document or project parameter, for example the Title, into the BOM. The Field declaration is replaced by the passed value, as shown in the images below.

Fields are used in the format:

Field=FieldName

An example would be Field=Currency

Fields should be defined above or below the Column region of the template.

Columns

Column declarations are used to map per-component parameters, for example each component's Designator, Description, user-defined parameters, and so on. This can also include: line numbers, PCB location data, and custom column data entered into the BomDoc, if there is a BomDoc in the project. The Column declaration in the template is replaced by the ColumnName string, with each row below being populated by that column value for each BOM Item, as shown in the two images below.

Columns are used in the format:

Column=ColumnName

An example would be Column=Designator

Notes:

  • Each column defined in the template must be displayed in the Report Manager, for that column of data to be transferred.
  • The data will present in the Excel spreadsheet in the same row order that it has in the Report Manager. Use the Report Manager's column sorting and sub-sorting feature to sort the rows as required.

Example of a simple Excel template, showing how the design parameters are mapped into the template

Example of a BOM created from the simple Excel template shown in the previous image

  • Several example templates are included with Altium Designer, in the \Templates folder of the installation user-files.
  • The default template location for an unmanaged design is configured in the Data Management - Templates page of the Preferences dialog.
  • For a managed design, the available templates are stored in the \Templates\BOM Templates folder of your managed content server.

Mapping Project-Level, BOM Header Information

Project-level information is typically mapped using the Field= statement, into the header of the BOM document.

Field Description
Currency The currency chosen in the Supplier Options region of the Report Manager dialog.
DataSourceFileName The filename of the source used for the BOM data.
DataSourceFullPath The full path + filename of the source used for the BOM data.
GeneratorDescription For a BOM, this field displays Bill of Materials.
GeneratorName Name of the generator - BOM when output is generated by the Report Manager.
OutputName Title of the BOM, as displayed in the Report Manager (excluding the text "For BOM Document [<DataSourceFileName>]").
OutputType For a BOM, this field displays BOM_PartType.
PCBDataSourceFileName The filename of the PCB data source.
ProductionQuantity Production quantity defined in the Report Manager dialog.
ProjectFileName Name of the PrjPcb file (including file extension).
ProjectFullPath Full path + the project filename.
ReportDate Date on which the report was created.
ReportDateTime Date and time at which the report was created.
ReportTime Time at which the report was created.
TotalQuantity Sum of the values in the BOM Items Quantity column.
Title Title displayed at the top of the BOM Reports dialog.
VariantName Name of the variant, as defined in the Variant Management dialog.
VersionControl_RevNumber Current revision of the BomDoc.
VersionControl_ProjFolderRevNumber Current revision of the project (incremented when a Commit Whole Project is performed).
<UserProjectParameter_n> Displays the value assigned to the user-defined UserProjectParameter-n.

Mapping Document and Project Parameters

As well as the Field statements listed above, schematic Document Parameters (both default and user-defined parameters entered in the schematic document's Properties panel) and Project Parameters (Options for PCB Project dialog) can also be used as Fields, or as Columns.

Address1 Address2 Address3
Address4 ApprovedBy Author
CheckedBy CompanyName ConfigurationParameters
CurrentDate CurrentTime Date
DocumentFullPathAndName DocumentName DocumentNumber
DrawnBy Engineer ImagePath
Index ModifiedDate Organization
Revision Rule SheetNumber
SheetTotal Time  

If the same parameter exists as both a document parameter and a project parameter, the project parameter takes precedence. If the same document parameter exists in multiple documents, the document parameter that is higher up in the heirarchy takes precedence.

Mapping BOM Item Information

The core region of a BOM is the grid of BOM Items, typically using a row for each component. Each column in this grid represents a component property, such as the designator, value, and so on. Columns are defined by entering the component property/parameter (BOM column heading), in the format:

Column=ColumnName

An example would be Column=Description, or Column=Designator

Column information can be taken from several sources, including:

These ColumnNames are available for all components

Comment ComponentKind Description
Designator DesignItemId Footprint
LibRef LogicalDesignator PartType
PhysicalPath Quantity UniqueIdName
UniqueIdPath <UserParameter_n>  

PCB component location information can also be included. In order to use these columns, the Include Parameters From PCB option must be enabled in the Report Manager dialog.

Center-X(Mil) Center-Y(Mil) Center-X(mm) Center-Y(mm)
Pad-X(Mil) Pad-Y(Mil) Pad-X(mm) Pad-Y(mm)
Ref-X(Mil) Ref-Y(Mil) Ref-X(mm) Ref-Y(mm)
Layer Rotation    

It is possible to retrieve online data from suppliers, and include that into the BOM. Note that these are updated live, and are retrieved when the BOM is generated. Multiple suppliers can be set up for each component. In the table below, these have been described as Supplier Info x - replace x with the appropriate number.

Manufacturer x Manufacturer Part Number x Supplier x
Supplier Currency x Supplier Order Qty x Supplier Part Number x
Supplier Stock x Supplier Subtotal x Supplier Unit Price x

User-defined columns are includes in the same way:

Column=ColumnName

 

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Sounds exciting! Did you know we offer special discounted student licenses? For more information, click here.

In the meantime, feel free to request a free trial by filling out the form below.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.