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

Downloads

Download the latest in PCB design and EDA software

  • PCB DESIGN SOFTWARE
  • Altium Designer

    Complete Environment for Schematic + Layout

  • CircuitStudio

    Entry Level, Professional PCB Design Tool

  • CircuitMaker

    Community Based PCB Design Tool

  • NEXUS

    Agile PCB Design For Teams

  • CLOUD PLATFORM
  • Altium 365

    Connecting PCB Design to the Manufacturing Floor

  • COMPONENT MANAGEMENT
  • Altium Concord Pro

    Complete Solution for Library Management

  • Octopart

    Extensive, Easy-to-Use Component Database

  • PRODUCT EXTENSIONS
  • PDN Analyzer

    Natural and Effortless Power Distribution Network Analysis

  • See All Extensions
  • EMBEDDED
  • TASKING

    World-Renowned Technology for Embedded Systems Development

  • TRAININGS
  • Live Courses

    Learn best practices with instructional training available worldwide

  • On-Demand Courses

    Gain comprehensive knowledge without leaving your home or office

  • ONLINE VIEWER
  • 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

    ALTIUMLIVE

    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

    Downloads

    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

    Using Net Ties to Meet PCB Design Requirements

    December 20, 2017

    Download the PDF to keep learning offline

    The Net Tie is a Component Type that allows PCB Engineers and Designers flexibility when Handling a Variety of Design Challenges. This Paper Explores the Advantages to using Net Ties in Altium Designer to Join Multiple Nets (shorts) Into One Single Net at Very specific Locations in the PCB.

    Using Net Ties to Meet PCB Design Requirements:

    Defining a Net Tie component can just be a matter of specifying it in the Type field of the Component Properties dialog in the right software.

    The Figure Shows The Library Component Properties Dialog for each type of Net Tie

    Figure 1: Net Tie Component Properties Dialog

    TYPES OF NET TIES FOR PCB ASSEMBLY

    When using net ties to meet pcb design requirements, there are two types of Net Ties to consider: Net Tie and Net Tie (In BOM). Each type is available on the pulldown options for Type in the Component Properties dialog. When using a Net Tie, the component schematic symbol graphic is attached to a specific type of footprint containing copper features connecting (shorting) the pads together. Net connectivity between the schematic symbol pins and printed circuit board PCB footprint pads is established in the customary way; however, no line item will appear for this component in the Bill Of Materials (BOM). Using the Net Tie (In BOM) allows materials to be called out in the BOM. Both types will be explored in this paper.

    The simplest form of a PCB layout net tie is a two pin component associated with a two pad footprint in which the pads are connected together with copper features.

    As with other schematic symbol types in board layouts, the display of symbol pin designators and display names are optional, schematic wiring between pins determines net connectivity, and there is a pin-to-pad connectivity established between the schematic and printed circuit board PCB. The graphic for a Net Tie component is arbitrary and in some cases unnecessary. For instance, a two pin Net Tie component may be represented to look like a piece of wire in a schematic sheet (totally hiding its existence).

    This Figure Shows An Example Of Two Pin Net Tie Schematic Symbols

    Figure 2: Pin Net Tie Schematic Symbols.

    A Net Tie footprint Possibly Used To Short Two Polygons Of Differing Net Names.

    Figure 3: A Net Tie footprint Possibly Used To Short Two Polygons Of Differing Net Names.

    Together. This Component Would Call Out The Header Part In The BOM. The Shorting Copper May Be Removed At A Later Date To Allow The Application Of An Optional Shorting Jumper.

    Used To Designate A Two Pin Header With The Pins Initially Shorted Together.

    Figure 4: Net Tie (In BOM) Used To Designate A Two Pin Header With The Pins Initially Shorted

    While routing to the pads of a Net Tie footprint, the Design Rule Checking (DRC) allows routing the nets associated with each pad to other same net copper features without flagging a violation, allowing the connecting (shorting) copper feature of the footprint to connect the two differing nets.

    DRC Allows Routing The Nets Associated With Each Pad To Other Same Net Copper Allowing The Connecting Copper Feature Of The Footprint  To Connect The Two Differing Nets.

    Track Of Two Different Nets

    If the two track ends from differing nets short together across the footprint, the DRC will flag a violation. This is due to the short circuit being generated between two differing nets outside the constraints of the Net Tie footprint.

    The Short Circuit Being Generated Between Two Differing Nets Outside The Constraints Of The Net Tie Footprint

    Track Of Two Different Nets Associated with a violation flagging

    Net Ties can be Set Up to allow Routing two differing Nets together with Various Track Widths.

    Figure 5: Net Ties with various Track Widths Net Ties can be Set Up to allow Routing two differing Nets together with Various Track Widths.

    Net Tie components created to allow routing between various routing layers by incorporating through hole Multilayer pads

    Figure 6: Net Tie components can be created to allow routing between various routing layers by incorporating through hole (Multilayer) pads.

    This Allow The designer options for component placement at a later time. In this example, the short may be replaced with a surface mount resistor or inductor.

    This Allow The designer options for component placement at a later time. In this example, the short may be replaced with a surface mount resistor or inductor

    Figure 7: Net Tie footprints can be created to allow shorting between nets, and later the shorting copper may be removed to allow components to be placed between nets. In this example, there is an 0805 and a 0602 footprint placed on top of each other with a shorting copper feature placed between them. This will allow the designer options for component placement at a later time. In this example, the short may be replaced with a surface mount resistor or inductor.

    Net Tie components allow establishing a connection between two differing nets at and only at the location of the Net Tie footprint on the PCB layout schematic. The DRC will flag any other short circuit violation between these differing nets elsewhere in the design.

    Planar inductors pose a special challenge in board layout. When various windings of the inductor are placed directly on the Printed Circuit Board, each winding is composed of routing tracks creating the various inductor coils. Each coil is a continuous copper track with differing nets at each end of the winding. The inductor winding track typically introduces a short circuit between each of the nets on the ends of the winding resulting in a DRC violation.

    You can use Altium Designer PCB design software to place a Net Tie component in series with the inductor windings. This provides a means of connecting differing nets, one net representing the winding and one side of the electrical circuit and the other net being the second electrical connection.

    The Net Tie component provides a means of tying AGND to the EGND net, which is extant throughout the planar winding

    Figure 8 Circuit bridging

    Figure 8: A circuit bridging two differing ground plane nets with a planar inductor winding. The Net Tie component provides a means of tying AGND to the EGND net, which is extant throughout the planar winding.

    In this example, silkscreen and reference designators have been shown to illustrate the placement of the components within the board layout; however, these features may be left off the actual design to elevate clutter and confusion in a high-density design.

    Silkscreen and Reference Designators have been shown to illustrate the Placement of the Components

    Silkscreen and Reference Designators have been shown to illustrate the Placement of the Components

    Here nets NT5, NT6, NT7, NT8, and NT 11 have been placed in a Component Class labeled NetTieDirect.

    Polygons and Net Tie components

    Polygons and Net Tie components

    Figure 9: Net Tie components may be used to connect polygons of differing nets to allow shorting at one and only one place. Other short circuits between these two nets will be flagged as violations by the DRC across the board layout.

    Design Rules and Polygons

    Design Rules and Polygons

    Figure 10: In the above example, multiple Net Tie components have been placed on a PCB to illustrate how design rules can be scoped to specify polygon connect style in order to achieve the desired result.

    Figure 11:Two Polygon Connect style rules have been created for the example NetTieDirect and NetTieRelief, which are scoped to the Component Classes NetTieDirect and NetTieRelief respectively.

    This Figure shows the example of  NetTieDirect and NetTieRelief

    Example of NetTieDirect and NetTieRelief

    Net Ties are connected to the polygons following the Relief connect rule

    Figure 12: In the upper area of the PCB, the Net Ties are connected to the polygons following the Relief connect rule.

    Note that NT1 has a polygon connect on the left side and the DRC allows routing from the right pad to the polygon.

    Examples of multi-pin Net Tie schematic symbols.

    Figure 13 Examples of multi-pin Net Tie schematic symbols.

    Extreme example of what can be achieved with Net Tie footprints.

    Figure 14: Extreme example of what can be achieved with Net Tie footprints.

    The lower portion of the Circuit Board Design follows the direct connect style. Notice how the polygon pulls back from the connecting (shorting) copper feature according to the clearance rules.

    Net Ties may have an unlimited number of pins and pads electrically connecting an unlimited number of nets.

    Net length tuning provides an interesting challenge when the signal path of time critical signals must arrive at the load end of the net at the same time within a reasonable delta. In the example below, the clock signal is generated and routed to two different IC packages. It is critical that the signal path of this high-speed signal has to achieve the same length within a reasonable tolerance.

    The Clock Signal is Generated and routed to two different IC

    The Clock Signal is Generated and routed to two different IC

    The use of a multi-net Net Tie allows the net to be broken out into separate nets for the purpose of length tuning. The associated footprint allows the same signal to travel different net paths

    .

    The nets CK1 and CK2 are associated into a Net Class labeled CLK and a Length rule is then created for this class.

    Once the nets CK1 and CK2 have been routed they can be length tuned to the Length rule which specifies the total length and tolerance.

    The associated footprint allows the same signal to travel different net paths

    The associated footprint allows the same signal to travel different net paths

    The nets CK1 and CK2 are associated

    The nets CK1 and CK2 are associated

    CK1 and CK2 have been routed they can be length tuned to the Length rule

    CK1 and CK2 have been routed they can be length tuned to the Length rule

    CONCLUSION:

    The Net Tie is a unique component type that allows the electronics engineer and PCB designer the flexibility to short different nets together. Following the steps above while using the top rated PCB design software Altium Designer can help you address requirement challenges when designing Printed Circuit Boards.

     

    most recent articles

    Back to Home