Free Trials

Download a free trial to find out which Altium software best suits your needs

How to Buy

Contact your local sales office to get started on improving your design environment


Download the latest in PCB design and EDA software

  • Altium Designer

    Complete Environment for Schematic + Layout

  • CircuitStudio

    Entry Level, Professional PCB Design Tool

  • CircuitMaker

    Community Based PCB Design Tool


    Agile PCB Design For Teams

  • Altium 365

    Connecting PCB Design to the Manufacturing Floor

  • Altium Concord Pro

    Complete Solution for Library Management

  • Octopart

    Extensive, Easy-to-Use Component Database

  • PDN Analyzer

    Natural and Effortless Power Distribution Network Analysis

  • See All Extensions

    World-Renowned Technology for Embedded Systems Development

  • Live Courses

    Learn best practices with instructional training available worldwide

  • On-Demand Courses

    Gain comprehensive knowledge without leaving your home or office

  • Altium 365 Viewer

    View & Share electronic designs in your browser

  • Altium Designer 20

    The most powerful, modern and easy-to-use PCB design tool for professional use


    Annual PCB Design Summit

    • Forum

      Where Altium users and enthusiasts can interact with each other

    • Blog

      Our blog about things that interest us and hopefully you too

    • Ideas

      Submit ideas and vote for new features you want in Altium tools

    • Bug Crunch

      Help make the software better by submitting bugs and voting on what's important

    • Wall

      A stream of events on AltiumLive you follow by participating in or subscribing to

    • Beta Program

      Information about participating in our Beta program and getting early access to Altium tools

    All Resources

    Explore the latest content from blog posts to social media and technical white papers gathered together for your convenience


    Take a look at what download options are available to best suit your needs

    How to Buy

    Contact your local sales office to get started improving your design environment

    • Documentation

      The documentation area is where you can find extensive, versioned information about our software online, for free.

    • Training & Events

      View the schedule and register for training events all around the world and online

    • Design Content

      Browse our vast library of free design content including components, templates and reference designs

    • Webinars

      Attend a live webinar online or get instant access to our on demand series of webinars

    • Support

      Get your questions answered with our variety of direct support and self-service options

    • Technical Papers

      Stay up to date with the latest technology and industry trends with our complete collection of technical white papers.

    • Video Library

      Quick and to-the-point video tutorials to get you started with Altium Designer

    Automate Output Job File Processing with PCB Release View in Altium Deisgner

    David Cousineau
    |  April 12, 2016

    There are many ways to peel an orange - so to speak - and some are better than others. And when it comes to generating fabrication and assembly outputs from your designs this adage holds true. In this PCB design tip, FAE Dave Cousineau describes a re-usable, highly effective way of managing output jobs using the PCB design release capability of Altium Designer®.

    Using Output Job files to define and store the necessary documentation needs for any Altium project is an extremely efficient and powerful feature. As more output types are supported by Output Job files (footprint comparison report, STEP file export, and 3D Movie creation have been added for AD10), or your company’s documentation requirements increase, the number of Output Containers needed can get quite large. There is currently no method within the Altium Output Job file editor itself for generating the content for more than one Output Container at a time for a batch job. Therefore, it may take many mouse clicks to generate your entire documentation package.

    AD10 introduced a new Design Data Management process with standard output for releasing designs to production. The aim of this process is to make use of Altium’s revision control integration and the new technology to provide an automated, high-integrity job output design release system. However, customers not using revision control or Vaults can still make use of some of the automation provided. This automation can be used to batch-process one or more Output Job files and is outlined below.

    Editing the Output Job files

    The first step in output file process is to set the Output Containers so that the Release Process will detect that Container. This is done by first clicking the Change link in a Container’s setup:

    If the Base Path is not set to [Release Managed], click the name of the current base output folder.

    This will drop down a small window showing [Release Managed] and [Manually Managed] choices. Select the [Release Managed] option. Now, instead of the outputs being written to the location specified by the [Manually Managed] folder name, the main output location will be determined by the Release Process.

    If the Base Path is currently set to [Release Managed], then it can be left as-is. The sub-folder names can be edited, if desired.

    Repeat this process for each of the Containers. If there are multiple Output Job files, edit those as well.

    Creating a Configuration

    The next step is to use a new area in AD10 called the Configuration Manager. This is accessed by right-clicking the .PrjPCB file name in the Projects panel, and selecting “Configuration Manager.” Additionally, if any file in the Project is currently opened, the Configuration Manager can be accessed via the Project menu.

    As part of the official release process, a Configuration is a way to set up how a project is to be output in order to map it to a particular Item to be manufactured. More on this concept can be found here:

    For the purposes of automating the Output Job execution, the only thing that needs to be done is to edit the existing default Configuration:

    The name of the default Configuration should be changed as this name will be used as the Base folder name when the outputs are generated. This folder will be created in the Project folder. For this example, the Configuration will be named “Outputs.”

    The next step is to enable which Output Job file(s) are going to be run. Notice the names of two Output Job files from the Project are shown in the image below. Both will be run in this example.

    Since no Vault is being used, the Target Vault can be left at [None] and the Target Item can be left empty. The resulting Configuration is as shown here:

    If desired, multiple Configurations can be created to accommodate different combinations of *.Outjob files. For instance, if there are two documentation Output Job files (one for each of two board manufacturers) and need to run a validation Output Job file, create the two Configurations as below:

    Click OK to dismiss the Configuration Manager. The information created here is stored in the .PrjPCB file, so save the Project at this point.

    Releasing the Design

    The last step is to create the outputs. Another new view for AD10 is the PCB Design Release View, accessed via the View menu. This view loads the Configuration(s) created in the Configuration Manager and allows the user to run all of the Altium Output Job files in the Configuration at once. Notice that the name of the Configuration is shown. If multiple Configurations existed, they would be shown here in a tabbed view, allowing you to choose which one to run.

    In the official release process (targeting a Vault item), you have the option of working in Design Mode or Release Mode. Release mode is only available when the design is checked in and current with revision control, and when a Release Vault is set up. Since neither of those is true here, only Design Mode will be available.

    In Design Mode, only two steps of the release process are available – Validate Design and Generate Outputs.

    Validate Design will be available if any of the Validation Outputs were added to the Output Job file. They include Design Rules Check, Differences Report, Electrical Rules Check, and Footprint Comparison Report. Three of these checks are present in the Validation.OutJob file used here.

    Clicking the Validate Design button will run just those checks at this point. Any Errors or Warnings will show in the Messages panel. Once the Validate Design step has been completed, the status of those checks will updated in the list as shown in the image below:

    It is important to note that because this is meant to support an official release flow, any validation checks that fail will cause the output generation process to stop. The failures must be addressed before continuing.

    When all validation checks have been marked as "Passed," the rest of the outputs can now be generated by clicking Generate Outputs. Keep in mind that it is not necessary to first run the Validate step prior to running the Generate Outputs command. If any of the validation checks are not in the Passed state (i.e., Missing, Out Of Date, Failed), running Generate Outputs will automatically run Validate Design first. If all validation checks pass, the rest of the outputs will be generated and sent to the folder defined by the Configuration name. The full path to the folder is listed at the bottom of the Release View as shown below:


    Once you have a good understanding of the job output process outlined above, it might be helpful to have a short checklist of the steps necessary to automate the output file process. There are really just three main steps:

    1. Edit the Containers in the Output Job files to be [Release Managed] instead of [Manually Managed].
    2. Right-click the Project name to access the Configuration Manager. Set the Configuration name as the name of the main output folder name desired. Enable the necessary Output Job files.
    3. Go to View/PCB Release View, and click Generate Outputs to run the validation checks and generate the outputs.


    About Author

    About Author

    Dave has been an Applications Engineer for 20 years in the EDA industry. He started in 1995 at a mid-Atlantic reseller that represented PADS Software, ViewLogic, and a host of other EDA tools. He moved on to work directly for PADS Software, and stayed on as they were acquired by Innoveda and then by Mentor Graphics. He and a business partner formed a VAR of their own in 2003 (Atlantic EDA Solutions) to represent Mentor's PADS channel, and later on Cadence's OrCAD and Allegro products. Since 2008, Dave has been working directly for Altium and is based at his home office in New Jersey.

    most recent articles

    Back to Home