Tutorial - Output Documentation and Project Release in Altium NEXUS

This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer and a connected Altium 365 Workspace. Check out the FAQs page for more information.

 

Parent page: Tutorial - A Complete Design Walkthrough with Altium NEXUS

Main page: Preparing Your Design for Manufacture

Now that you've completed the design and layout of the PCB, you're ready to produce the output documentation needed to get the board reviewed, fabricated, and assembled.

Output types include PDF 3D, with full zoom, pan and rotate, and the ability to control the display of nets, components, and the silkscreen, in Adobe Acrobat Reader®.
Output types include PDF 3D, with full zoom, pan and rotate, and the ability to control the display of nets, components, and the silkscreen, in Adobe Acrobat Reader®.

Available Output Types

Because a variety of technologies and methods exist in PCB manufacture, the software has the ability to produce numerous output types for different purposes:

Assembly Outputs

  • Assembly Drawings – component positions and orientations for each side of the board.
  • Pick and Place Files – used by robotic component placement machinery to place components onto the board.
  • Test Point Report – as ASCII file, available in 3 formats, that details the location of each pad/via that has been nominated as a testpoint.

Documentation Outputs

  • PCB Prints – configure any number or printouts (pages), with any arrangement of layers and display of primitives. Use this to create printed outputs, such as assembly drawings.
  • PCB 3D Prints – views of the board from a three-dimensional view perspective.
  • PCB 3D Video – output a simple video of the board based on a sequence of 3D key-frames defined in the PCB editor's PCB 3D Movie Editor panel.
  • PDF 3D – generate a 3D PDF view of the board with full support to zoom, pan, and rotate in Adobe Acrobat®. The PDF includes a model tree, giving control over the display of nets, components, and the silkscreen.
  • Schematic Prints – schematic drawings used in the design.

Fabrication Outputs

  • Composite Drill Drawings – drill positions and sizes (using symbols) for the board in one drawing.
  • Drill Drawing/Guides – drill positions and sizes (using symbols) for the board in separate drawings.
  • Final Artwork Prints – combines various fabrication outputs together as a single printable output.
  • Gerber Files – creates manufacturing information in Gerber format.
  • Gerber X2 Files – a new standard that encapsulates a high-level of design information with backward compatibility to the original Gerber format.
  • IPC-2581 File – a new standard that encapsulates a high-level of design information within a single file.
  • NC Drill Files – creates manufacturing information for use by numerically controlled drilling machines.
  • ODB++ – creates manufacturing information in ODB++ database format.
  • Power-Plane Prints – creates internal and split plane drawings.
  • Solder/Paste Mask Prints – creates solder mask and paste mask drawings.
  • Test Point Report – creates test point output for the design in a variety of formats.

Netlist Outputs

  • Netlists describe the logical connectivity between components in the design and are useful for transferring the design to other electronics design applications. A large variety of netlist formats are supported.

Report Outputs

  • Bill of Materials – creates a list of parts and quantities (BOM) in various formats required to manufacture the board.
  • Component Cross Reference Report – creates a list of components based on the schematic drawing in the design.
  • Report Project Hierarchy – creates a list of source documents used in the project.
  • Report Single Pin Nets – creates a report listing any nets that only have one connection.

Individual Outputs or an Output Job File

Main page: Streamlining Generation of Manufacturing Data with Output Jobs

The PCB editor has three separate mechanisms for configuring and generating output:

  1. Individually – the settings for each output type are stored in the Project file. You selectively generate that output when required using the commands in the Fabrication Outputs, Assembly Outputs and Export sub-menus (accessed from the File menu), and the Reports menu.
  2. Using an Output Job file – the settings for each output type are stored in an Output Job file, which is a dedicated output settings document that supports all possible output types. These outputs can then be generated manually or as a project release.
  3. In the design release process – output documentation that is set in all Output Job files of the project can be generated as a part of the integrated project release process, with the ability to validate the design.

An Output Job file allows you to configure each output type, configure their output naming, format, and output location. Output Job files can also be copied from one project to another.
An Output Job file allows you to configure each output type, configure their output naming, format, and output location. Output Job files can also be copied from one project to another.

Although the individual outputs configured using the File and Reports menus use the same setup dialogs as an Output Job, the settings are independent and must be configured again if you switch from one approach to the other.

Configuring the Gerber Files

Dialog page: Gerber Setup

  • Gerber continues to be the most common form of data transfer between board design and board fabrication, with Gerber X2 and ODB++ becoming more and more popular.
  • Each Gerber file corresponds to one layer of the physical board: the component overlay, top signal layer, bottom signal layer, top solder mask layer, and so on. It is advisable to consult with your board fabricator to confirm their requirements before supplying the output files required to fabricate your design.
  • If the board has holes, an NC Drill file must also be generated, using the same units, resolution, and position on film settings.
  • Gerber files are configured in the Gerber Setup dialog, accessed via the PCB Editor's File » Fabrication Outputs » Gerber Files command, or by adding a Gerber output into the Fabrication Outputs section of an Output Job then double-clicking on it.

    Configure the Gerber outputs in the Gerber Setup dialog.
    Configure the Gerber outputs in the Gerber Setup dialog.


Configuring Validation Report Generation

The software includes a number of validation checks, which can be included as an output, during output generation. Each produces an HTML report file. During the project release process, these checks will be performed prior generation of other outputs, and if any validation checks are not passed successfully, the release will fail.


Configuring the Bill of Materials

Main page: BOM Management with ActiveBOM

Ultimately, every part used in the design must have detailed supply chain information. Rather than requiring that this information be added to each design component, or added as a post-process in an Excel spreadsheet, you can add it at any point through the design cycle in an ActiveBOM (*.BomDoc).

ActiveBOM is the component management editor included in Altium NEXUS, which is used to:

  • Configure the component information so that it is BOM-ready, including adding additional non-PCB component BOM items, such as the bare board, glue, mounting hardware, and so on.
  • Add additional columns, such as a line number column, to suit the requirements of the assembly house.
  • Map each design component to a real-world manufacturer part.
  • Verify the supply chain availability and price for each part, for a defined number of manufactured units.
  • Calculate the cost to build for the defined number of manufactured units.

ActiveBOM is used to map each design component to a real-world part.
ActiveBOM is used to map each design component to a real-world part.

This ability to inject supply chain details directly into the BOM changes the role of the BOM document in the PCB project. No longer a simple output file, ActiveBOM raises the component management process to sit alongside the schematic capture and PCB design processes, where ActiveBOM's BomDoc becomes the source of all Bill Of Materials data for the PCB project for all BOM-type outputs. ActiveBOM is the recommended approach to BOM management.
ActiveBOM queries the supply chain in real-time, using the Part Providers enabled in the settings of your connected Workspace. Because data is updated in real-time, the availability of the parts used in this tutorial will change over time. The list of available suppliers also changes over time. For these reasons, the results you get may be different from the results shown and described in this tutorial.

Preparing the Output BOM

Dialog page: Report Manager

The actual output BOM file that is generated is done using the Report Manager. The Report Manager is a highly configurable report generation engine that can generate output in a variety of formats including text, CSV, PDF, HTML, and Excel. Excel-format BOMs can also have a template applied using one of the pre-defined templates or one of your own. An Excel-format BOM can also be generated without Microsoft Excel being installed; select the MS Excel File option in the File Format drop-down.

  • The Report Manager generates BOM output from the Bill of Materials For Project dialog, accessed via:
    • The schematic or PCB editor's Reports » Bill of Materials, or
    • By adding a BomDoc to the project and running the BomDoc's Reports » Bill of Materials command, or
    • By adding a Bill of Materials into the Report Outputs section of an Output Job.
  • The default behavior is for the Report Manager to present the component detail in the same way it has been configured in the BomDoc if the project includes a BomDoc. Columns can be added and removed using the Columns tab in the Properties region of the dialog.
  • If the project does not include a BomDoc, the Columns tab includes an additional region, used to define how like-components are identified for clustering. Clustering is achieved by dragging and dropping component attributes to the Drag a column to group region of the dialog.
  • The main grid region of the dialog is the content that is written into the BOM. In this region, you can click and drag to reorder the columns, click on a column heading to sort by that column, Ctrl+Click to sub-sort by that column, and define value-based filters for a column using the small drop-down in each column header.
  • By default, the BOM generator sources information from the schematic documents. A variety of Sources are available. Use the buttons in the Columns tab in the Properties region of the dialog to enable other sources. For example, if you enable the PCB Parameters you can include detail such as component location and side of board if required.

    The Report Manager takes the configuration from the BomDoc if the project includes a BomDoc.
    The Report Manager takes the configuration from the BomDoc if the project includes a BomDoc.

Mapping Design Data into the Generated BOM

Design data can be passed from Altium NEXUS into an Excel-format Bill Of Materials by referencing an Excel template that includes special statements.

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 included with the software in the \Templates folder of the installation user files. Refer to the Mapping Design Data into the BOM section of the BOM Configuration in the Report Manager page for details of the available fields. Note that fields need to be defined above or below the Column region of the template.


Project Release

Main page: Board Design Release

With output documentation configured in OutJob files, the project is ready to be released to the connected Workspace. The board design release process is automated, enabling you to release your board design projects without the risks associated with manual release procedures. When a particular project is released, a snapshot of the design source is taken and archived along with any generated output – which represents a tangible product that is made from that design project and sold by the company.

The release process itself is performed using Altium NEXUS's Project Releaser, the user interface to which is provided courtesy of a dedicated view – the Release view. The release process is a staged flow, with the entries on the left-hand side of the view showing you at-a-glance, which stage you are currently at.

The Release view – the user interface to the Project Releaser.
The Release view – the user interface to the Project Releaser.

You started with a blank schematic sheet and worked through to a finished PCB with output files released to the Workspace, which is the entire design process in Altium NEXUS. Next, we will explore some features related to project management and collaboration.
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Content