Free Trials

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

Altium Online Store

Buy any Altium Products with few clicks or send us your quote to contact our sales


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

    Altium Online Store

    Buy any Altium Products with few clicks or send us your quote to contact our sales


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

    • 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

    Avoid Holds for Common Data Package Errors

    Tara Dunn
    |  August 20, 2019

    Ever had one of your data packages placed on hold by your fabricator? If so, you are not alone. A significant number of new flexible circuit or rigid flex designs are placed on hold for engineering questions and clarifications almost immediately after the order is placed with the fabricator. Tara Dunn reaches out to Director of Engineering at Summit Interconnect Technologies. His current position is focused on cutting-edge high-density interconnect, high speed digital, Flex/Rigid Flex and RF/microwave printed circuit board fabrication for the military and commercial industries. He is a certified IPC trainer, a member of the IPC-6012 and IPC-6018 review committees, and an excellent resource for a wide range of PCB related topics. Gerry was kind enough to lend his expertise and provide a response to my question. 

    What is one thing, or things, that are commonly missed in the flex and rigid-flex data packages that causes a hold in engineering, or impact on the final product?


    Currently, we experience design holds about 60% of the time. The number one reason for jobs being placed on hold is the documentation. Most of these documentation issues could have been avoided by the designer and procurement team by simply reviewing the entire documentation package and purchase order requirements before submitting the order to the fabricator.  

    Fabrication Data Set:

    The first step is to confirm that the fabrication dataset is complete and the correct revision. Are all the circuit layers, drill files, solder masks, legends, netlists, array instructions (if required), and fabrication drawings generated? There are many instances when the drill files are from the previous revision while the circuit layers are the new revision, or vice versa. 

    Fabrication Drawing:

    The fabrication drawing needs to be completely reviewed for accuracy. A mismatch between a drill chart and the supplied drill file will cause the job to go on hold at the very start of the CAM process. If you are wondering why, a mismatch indicates that the drawing and supplied data may not be the same revision. A review of each note of the drawing and each detail (stack-up, impedance table, details and PCB dimensions) must be reviewed and confirmed correct. Many jobs go on hold because dimensions do not match the PCB design data, or when an impedance line width is specified on a drawing but doesn't exist in the actual design layer.  

    What things impact final product? 

    Annular Ring and Drill to Copper:

    Regarding impact on final product, I would like to touch on finished annular ring requirements and drill to copper distance. It’s much more difficult to maintain inner layer registration with Flexible materials compared to glass reinforced materials. Additional annular rings should be designed into the flex layers when possible. Many designs have the same annular ring requirements as rigid cores. There is greater risk of a finished flex core with a .005" annular ring failing a tangency requirement or a .006" annular ring failing a class 3 minimum finished requirement of .001", even though the PCB has passed electrical test and all other cross section requirements. Additionally, more annular ring should be factored in for more than one lamination cycle. The first lamination cycle can have the typical annular ring, but additional lamination cycles will benefit from an increased annular ring.  

    Lastly, on the subject of annular ring, do not remove the nonfunctional pads while "laying out" your traces. The nonfunctional pads serve as the safe keep-back distance between a drill and a conductor. IPC-2221, IPC-2222 and IPC-2223 require a keep-back distance as if the annular is present. Removing the nonfunctional pads and routing closer to the drill will reduce the reliability of your finished product and could be in violation of the requirements of IPC design guidelines.  

    Annular Ring Example:

    Following is an example of the danger of removing the non-functional pads and routing closer to the drill: 

    • The design is .008" drill to copper.

    • Tangency is permitted with a .005" annular ring, that will allow drill to copper to be .003" before etch back or drill removal.

    • Etchback is required—allowing the removal of .0015". The distance now is .0015" between the copper plating and a different conductor.

    • CAF migration allows for up .001" growth. Worst case condition is now .0005".

    • IPC-2221/2222 requires a minimum space .002" for 0-50 volts in finished product. 

    When the worst-case scenario is added up, the plated hole is over budget by .0015". This may be acceptable for class 2 product but is a concern for class 3 product and field reliability. 

    I want to thank Gerry for sharing his experience and giving input and suggestions for how to improve flex and rigid-flex data packages to avoid the common items that cause holds at fabrication and for the detailed explanation of annular ring tolerance build-up. This has been helpful for me and I hope for you.

    Watch Gerry Partida discusses about Wrap Plating and Via Filling.

    Link to Summit Interconnect?  

    Would you like to find out more about how Altium can help you with your next PCB design? Talk to an expert at Altium or discover more about sending complete documentation packages to PCB fabrication.

    About Author

    About Author

    Tara is a recognized industry expert with more than 20 years of experience working with: PCB engineers, designers, fabricators, sourcing organizations, and printed circuit board users. Her expertise is in flex and rigid-flex, additive technology, and quick-turn projects. She is one of the industry's top resources to get up to speed quickly on a range of subjects through her technical reference site and contributes regularly to industry events as a speaker, writes a column in the magazine, and hosts Her business Omni PCB is known for its same day response and the ability to fulfill projects based on unique specifications: lead time, technology and volume.

    most recent articles

    Back to Home