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

    Preparing Documentation for Output – Who needs What?

    April 22, 2019

    It is a very common misconception for beginners (and even some experienced) board designers to just push the “buttons” or menu “commands” in the software for outputting fabrication & assembly data. However, there are set-ups that have to be done before you can use those buttons and commands. (Altium Designer® commands highlighted in RED below.)

    While there are many ways to develop documentation for a board, it is important to realize the need to give separate information to each manufacturing process. The data needed to produce your board by the Fabricator is different than what is needed by the Assembler. So, first, let’s define what type of data each of these manufacturers really need. Please note that the setup for the data must be done in the design package even if you create an ODB++ file OR you use the IPC-2581 outputs. Remember – GIGO. (Garbage In, Garbage Out)

    Fabricator needs to know the following details

    These are presented in a FABRICATION DRAWING and accompanied by a set of processing files. The FABRICATION DRAWING can be done using Draftsman® and the processing files can be set up in the Outjob. These can all be ZIPPED into one package for the Fabricator. (A quick search on AltiumLive will give you many options for details on using these commands.)

    Size of the Board and location of features

    This includes defining an ORIGIN (0,0 point) where all dimensions can be measured and verified. NC Drill files do NOT do this for you. Neither does creating an NC route file (although these can be very useful to the fabricator).

    • Dimensions for the overall boundaries
    • Dimensions for cutouts & notches
    • Dimension for the overall Thickness of the board
    • Use GDT tolerancing methodologies.

    Holes & Slots

    This is best shown with a Drill Table and produced with an NC Drill File. (Check hole sizes with Panels/PCB/Hole Size Editor.)

    • Number of different hole sizes. These should be in increments of 2 mils (0.05mm) for consistent, cost effective results.  
    • Definitions for Plated, Non-Plated, and depth (Blind, Buried, and back drilled).

    Figure 1. Drill drawing view

    Number and definition of Layers

    This includes a GERBER for each process layer – copper, gold plating (if present), soldermask, and silkscreen. (Setup should be done in the Layer Stack.)

    • Show a Layer stack and define where the signal and plane layers are. Number the copper layers to prevent confusion. Name the Top & Bottom soldermask & silkscreen layers and any other additive process layers.
    • Thickness and material can be generic or specific depending upon your needs.
    • Some companies also show a view of each copper layer.
      • This isn’t really necessary but can help to quickly identify the “positive or negative” nature of the GERBER file. Many programs will produce “PLANE” layers as either a “positive” or “negative” image.
      • It can also be a quick reference for the designer or design team to be sure all expected features have been defined correctly in each layer.

    Figure 2. Layer Stack

    Figure 3. Gerber Views

    Test Point locations for fabrication or a list of the files included with the documentation.

    After defining features in the layout as a Fabrication Test Point, you can export these in the IPC-D-356a Netlist file. (Set up in Outjob/Fabrication Outputs.)

    • Sometimes the fabricator will want to have a copy of the Schematic to verify some of the nets. Depends on what requirements are being asked of the fabricator to ensure electrical features such as differential pairs and continuity through net-ties.

    Provide Notes for:

    • Tolerancing, manufacturing processes, and IPC product classification (helps to define the tolerances).
    • Plating requirements
    • Registration
    • Soldermask material & color
    • Silkscreen material & color
    • Any special coatings or finishes (Conformal coating materials, gold plating, HASL, etc)

    Figure 4. Fabrication Notes

    What the Assembler Needs to Know

    All the information that the assembler needs to know are presented in an ASSEMBLY DRAWING and accompanied by a set of processing files. The ASSEMBLY DRAWING can be done using Draftsman® and the processing files can be set up in the Outjob. These can also be ZIPPED into one package for the Assembler.

    View of the intended Assembly of the board from Top, Bottom, and side

    • If there are variants of the assembly, they should be noted in the view(s). This is where you SHOW which components don’t get installed and which ones do.
    • Also, a quick reference dimension of the overall size (X & Y) of the board and a dimension of the height of the tallest component(s) on each side of the board.
      • This gives the assembler a good quick reference to the type of machinery they will need to produce your boards.
    • A 3D view is nice, but not always necessary. A 3D view is to clarify assembly intent and facilitate good communication.

    Figure 5. Assembly View


    Figure 6. Assembly view from the side

    • Define the placement/alignment variables/tolerances for components that must interface with other mechanical features in the completed part (such as an instrumentation panel, switch or button interface, or light pipe).

    • Use the same origin used in the fabrication drawing to define these location tolerances.

    • Use GDT tolerancing methodologies for X, Y, & Z locations.

    • Use details to assist with alignment accuracy if needed.

    Provide a Pick & Place file from the layout

    • This is a generated text document with origin locations of each component. It is used in the set-up of the assembly machinery. The file lists the component locations relative to the PCB origin.
    • NOTE: All SM components are placed (and thus referenced for location) using the CENTER of the part, not an edge! This is due to the type of placement machinery used – a suction tube robotic arm. Many TH components (or heavy components) are placed using a “grabber” type of robotic arm. Their location reference may be “Pin 1” or may be “body center”. For headers & TH connectors, use “Pin 1”. When there is a mix of SM & TH in the same part, use the body center.

    Provide a BOM with approved second & third sourcing for components

    This can be included on the Assembly drawing or as a separate document. BOM output can be done from either the schematic or the layout. There are many ways to produce a BOM. 

    • Don’t leave alternate components up to the Assembler. Many components look the same and are NOT. All alternate components should have the same FORM, FIT, and FUNCTION!!

    Figure 7. Bill of Materials

    Provide NOTES for:

    • Tolerancing, manufacturing processes, and IPC product classification (helps to define the tolerances).
    • Special component programming requirements.
    • Additional assembly procedures AFTER soldering.

    Figure 8. Assembly Notes

    Define Assembly Test Procedures

    This also can be included on the Assembly drawing or as a separate document. Options can include:

    • Include Functional test requirements as needed.
    • Provide a test program file if needed.
    • Define assembly test points.
      • These should be located away from component soldering joints and outside of all component bodies.
      • They should be on a grid if using “bed-of-nails” test procedures. Specify the grid used.

    The issues we all face while doing the set-up for Fabrication and Assembly files and documents often lie in just a few places. Look at the workarounds vs “good practice” methods being used in your environment and consider what can be improved.

    Have more questions? Call an expert at Altium or read more to gain a deeper understanding of sending a complete documentation package to PCB fabrication with Altium Designer®.


    Team Up and Save

    Get Special Savings When You Add a New Altium Designer® Seat

    most recent articles

    Back to Home