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

    The History and Use of Cross-Hatched Planes

    Kella Knack
    |  October 12, 2020
    The History and Use of Cross-Hatched Planes

    Cross-hatching of PCB planes refers to a method wherein certain planes or other large areas of copper within a PCB appear as a latticework of copper. Regular openings are placed at regular intervals, much like those that appear in a screen door. The requirement for cross-hatching a plane is rare these days in rigid PCBs, but they are used in flex and rigid-flex implementations where they can provide a number of benefits. So when is it appropriate to use hatching, particularly hatch ground or hatch power regions?

    Although not so useful anymore in rigid PCBs, they've become quite important in flex/rigid-flex PCBs, where the hatch ground pattern plays dual roles as a structural support and a ground element. This article will describe the history of cross-hatch planes, how they are made, the reason they were initially used in rigid PCBs, and their ongoing role and benefit today in flex and rigid-flex boards.

    Definition and History of Hatch Ground

    As noted above, a hatch ground plane is a latticework of copper with regular openings at regular intervals. The actual process of creating a cross-hatched plane occurs in the CAD or CAM system, where the region to be hatched is the filled area with a series of regularly spaced lines much, like the traces plotted in signal layers. Then, the area is edged with a thin border trace that connects the ends of the lines that form the crosshatch. Connections, such as power or ground connections, are made to this cross-hatching in the same way that they are made in solid planes.

    In the earlier days of the multilayer PCB fabrication process, the final step of inner layer processing involved roughening the copper surfaces so that they would adhere tightly to the resin in the prepreg system during lamination. This step was necessary because the copper surfaces as they emerged from the DES (develop, etch, and strip) process were very smooth. In fact, they were so smooth that it was difficult to create a strong bond between the resin used to laminate the PCB and the copper. As a result, if the copper surfaces weren’t roughened, delamination would occur between the laminate and the solid copper planes of the PCB. This same problem occurred with component mounting pads on outer layers resulting in pads coming loose from the PCB while soldering during rework.

    Note: The same adhesion problem also exists when pieces of laminate are manufactured. The same resins, used in manufacturing a PCB, are employed during laminate manufacturing. Here, resin impregnated glass cloth is combined with a piece of copper foil bonded on each side to create the laminate. In this instance, the surface of the copper foil that is bonded to the resin gets its rough finish as part of the plating process that creates the foil.

    Implementation in Rigid PCBs

    To address the foregoing copper adhesion problems on rigid multilayer PCBs, cross-hatching was created. The actual process involved creating small openings in the copper plane so that the resin would bond to the laminate through the copper, rather than attempting to force a bond directly between the resin and copper. As long as the bond to the laminate was sufficiently strong and distributed throughout the board, the board would be study enough to resist delamination.

    This basically solved the delamination problem but created an expensive proposition because of the complex CAD files that had to be created. Much like the beloved Gerbers of today, these files were used to describe layers and plot the film that was required to image those layers. During this time, CAD tools were nowhere near as powerful as they are today, and designers couldn't simply export these files with a few clicks of a button.

    In the late 1980s, a new process was developed that solved the foregoing adhesion problem so that cross-hatched planes on rigid PCBs were no longer necessary. This process is accomplished through one of two approaches. One is called black oxide treatment, and the other is called alternative or brown oxide. After this step, the appearance of the copper on an inner layer is matte black following the black oxide approach or brown in color following the alternative oxide approach. An inner layer with black oxide is shown in Figure 1.

    An Inner Layer Pair After Etching and Application of Black Oxide
    Figure 1. An inner layer pair after etching and application of black oxide.

    Both of these approaches micro etch the copper so that it is rough enough to bond with the resin in the prepreg. Essentially, they provide the “teeth” to which the resins can bond. The treatments are done to all inner layers after etching and just prior to lamination. The result is a very strong bond between prepreg resins and the layers of copper in a PCB.

    Note: Copper roughness is often discussed as a problem with very high-speed signals due to increased skin effect loss in the traces of the PCB. In order to reduce the roughness of the copper trace surfaces an alternative surface preparation such as Atotech Bondfilm is used which does not increase the surface roughness.

    Cross-hatching in rigid PCBs is rarely done these days. In fact, if a fabricator or other source asks for cross-hatching to be applied to inner layer planes or copper fills on outer layers, one of two things are at work:

    • The fabricator or other source is operating with very old, outdated rules.
    • The fabricator does not have adequate process control and should be avoided as a board manufacturer.

    Cross-Hatching in Flex and Rigid Flex Circuits

    While cross-hatching is rarely used in rigid PCBs these days, it does have practical application for both flex and rigid-flex circuits. These applications come in two areas for flex and rigid-flex circuits:

    • Controlled impedance in flex regions: Using a hatch ground is a good method for providing the reference plane required in controlled impedance routing for high speed digital boards. The hatch ground provides wider, more manufacturable dimensions while retaining the flexibility of the circuit and assembly. It should be noted that cross-hatching reduces the amount of copper under a transmission line, which decreases the capacitance and raises its impedance.
    • Structural support for flex regions: Using a hatch ground provides structural support needed for a dynamic or static flex ribbon without increasing the rigidity of the copper layer. on a two-sided flexible circuit. The layer can still be used for controlled impedance routing creating undesired rigidity, or the ribbon can be permanently deformed.

    In order to calculate a trace width that results in the correct impedance, it is necessary to use a modeling tool that accounts for the missing copper in the crosshatched plane. Because the impedance for a given trace over a hatch ground region is higher than that over a solid ground region, the inductance of the trace needs to be decreased to maintain controlled impedance. Therefore, we would want to make the trace a bit wider as this will reduce the trace's inductance and increase the total capacitance with respect to the hatch ground. Both effects will contribute to set the impedance to the correct value. 


    There was a time when it was necessary to use hatch ground planes and pour as a way to guarantee proper adhesion of prepreg resins to the copper foils in rigid, multilayer PCBs. Poor adhesion to smooth copper resulted in delamination of the inner layers. However, this is no longer necessary due to the development of surface treatments that create a secure bond between the resin and copper. As a result, the use of cross-hatch planes in rigid  multilayer PCBs have gone by the wayside. However, the use of this process in rigid-flex and flex circuits is of benefit as it ensures a polyimide region in a flex/rigid-flex board can remain flexible.

    Would you like to find out more about how Altium can help you with your next PCB design? Talk to an expert at Altium.


    1. Ritchey, Lee W., and Zasio, John J., “Right The First Time, A Practical Handbook on High Speed PCB and System Design,” Volume 2.

    About Author

    About Author

    Kella Knack is Vice President of Marketing for Speeding Edge, a company engaged in training, consulting and publishing on high speed design topics such as signal integrity analysis, PCB Design ad EMI control. Previously, she served as a marketing consultant for a broad spectrum of high-tech companies ranging from start-ups to multibillion dollar corporations. She also served as editor for various electronic trade publications covering the PCB, networking and EDA market sectors.

    most recent articles

    Back to Home