Including Design Data in an Excel-format Bill of Materials (BOM)

Created: June 4, 2015 | Updated: March 10, 2017

Now reading version 15.1. For the latest, read: Including Design Data in an Excel-format BOM for version 21

Contents

Design data can be passed from Altium Designer into an Excel Bill Of Materials by including special statements in the Excel template used to create the BOM.

For detailed information about creating a Bill of Materials, click here.

When creating the Bill of Materials template in Excel, a combination of Fields and Columns can be used to specify the desired layout. Several example templates are provided with Altium Designer in the \Templates folder of the installation user-files. A full list of available fields is provided below.

Fields

Fields provide project-level information. These are not usually attached to each item in the BOM, but are often used in the header of the document. Fields are used in the format Field=FieldName (e.g., Field=Currency). The available fields are:

Currency
DataSourceFileName
DataSourceFullPath
GeneratorDescription
GeneratorName
OutputName
OutputType
ProductionQuantity
ProjectFileName
ProjectFullPath
ReportDate
ReportDateTime
ReportTime
Title
TotalQuantity
VariantName

Columns

Columns provide information that is supplied on a per-component basis, and would usually appear on each line in the BOM. Columns are used in the format Column=ColumnName (e.g., Column=Description). Column information can be taken from several sources, including:

Default component parameters (such as Designator or Description).
User-defined parameters added to components.
PCB data.
Supplier data.

These are discussed separately below.

Default Parameters

The following columns are provided for all components:

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

Document Parameters

The following document parameters are available for all components by default. They are obtained from the schematic document that contains the component.

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

PCB Parameters

Pick and Place information can also be included from the PCB. In order to use these columns, the checkbox Include Parameters From PCB must be enabled in the Bill Of Materials Report Manager dialog.

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

Supplier Data

In Altium Designer, it is possible to retrieve online data from suppliers and feed 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.

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

Custom Parameters

Additional information also can be imported from a database library or from parameters added to components by the user. In these cases, simply use the parameter name as the column name.