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

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

    Downloads

    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

    Part Placement Shortcuts in Altium Designer

    Altium Designer
    |  March 13, 2018

    Picture of 3D component placement from Altium

    I read once that circuit board design is 90% placement and 10% routing. I’m not sure that I believe that, but it is fair to say that component placement is a critical part of the overall board design. Yet some designers will rush this part of the job so that they can get on with routing the board, only to have to come back later and re-place portions of the board.

    I wonder if one of the problems is that designers get frustrated during the Altium component placement process. It does take some time to get all of your components correctly located, aligned, and positioned so as to provide the most optimum routing channels. This is especially true if you are working with design tools that are limited in their placement capabilities, or if you just don’t understand the placement functionality that you have available in your design tools that can help.

    Fortunately, Altium Designer® has some powerful placement functionality that can make your job a lot easier. There are manual placement utilities to help with alignment, and you have the option of organizing your components for placement by selecting them first in the schematic. Also, if you need some help in finding and selecting specific components for placement, there’s a utility for that as well.

    Use the Alignment Feature to Straighten Out Your Placement

    I must admit, having to constantly move components around during placement can be annoying. I have often had a string of components lined up just the way that I want them, only to discover that a new component needs to be squeezed in. Once I move everything around to get the new part in, my perfect alignment is now shot and I have to tweak all the components to get them lined up again.

    Yes, manually moving each part it is a straightforward operation, but wouldn’t you agree that if there was some simple help available that it would be nice to use?

    Altium 18 has this help ready for you to use in its placement alignment tools. There is a whole menu of different alignment functions at your disposal, and here is an example of how you can use them. You will notice in this first screen capture that I have a row of misaligned components that needs to be cleaned up. There are even some clearance violations between pins that are too close together.

    Screen capture of AD with misaligned component placementComponents that are not aligned

    First I selected all of these components and then used my right mouse button to get to the “Align” menu. Once I was in the Align menu, I selected “Align” from the top of the list to pop up the “Align Objects” sub-menu that you see below.

    Screen capture of AD with Align Object menuSet your alignment parameters

    In the “Align Objects” sub-menu I selected the parameters that you see above. For my horizontal alignment, I directed Altium to give the components equal spacing. For my vertical alignment I elected to align by their tops, and then I clicked “OK.” As you can see below, my components are now aligned equally the way that I want them to be.

    Screen capture of AD with component placement now alignedYour components are now aligned as you want them to be

    This is not a feature that you will use every day, but when you have a row of components that need to be quickly cleaned up, this can be very useful. The key to getting the most out of a feature like this is to become familiar with it so that it is second nature to you when you need it.

    I have talked with many designers that have simply never taken the time to learn how to use all of the help that their design tools provide for them. Because of this, they miss out on functionality that is intended to help them. This alignment tool in Altium Designer can be a very handy tool to keep in your back pocket, use it.

    Altium Placement Cross-Select Mode from the Schematic

    Aligning your components is a great feature to use once your are placed on the board, but I know a lot of designers that struggle just with getting started on their placement. Having a bunch of components outside the circuit board outline with connections going everywhere can be a daunting puzzle to try to plow through. Again though, Altium Designer has a utility in place that will help you with this.

    By going into the schematic, you can select groups of circuitry that need to be placed together on the board. Once selected in the schematic, you can then designate a rectangle in the layout where you want those selected components to be placed. This allows you to quickly organize the components in your layout by how they are drawn in the schematic which in turn will facilitate a better placement on the printed circuit board.

    With the components spread around the exterior of the circuit board outline in layout, I opened the schematic to the sheet that I needed for a group of connected circuitry. I then went to the menu; “Tools > Cross Select Mode” as shown in the picture below.

    Screen capture of AD with both schematic and layout windows openUse the Cross Select Mode in the schematic

    Next, I selected the components that I wanted to be placed in the schematic sheet by dragging a select box around them. You can see in the picture below the selected components in the upper half of the schematic sheet.

    Screen capture of AD with components selected in the schematicSelect the components for placement in the schematic

    After activating the layout window, I next selected the menu item; “Tools > Component Placement > Arrange Within Rectangle” as shown in the picture below. The cursor in the layout window will show as a green crosshair indicating that it is ready for the placement rectangle to be specified. Click to establish the first corner of the rectangle, and then click again for the opposite corner.

    Screen capture of AD with the Arrange Within Rectangle function selected in layoutIn layout, select the Arrange Within Rectangle function

    After creating the rectangle in the center of the printed circuit board outline, Altium Designer populated that area with the selected components from the schematic. You can see the components that were moved into that area in the picture below.

    Screen capture of AD with selected components from the schematic placed in layoutThe selected components in the schematic place their counterparts in layout

    This won’t be the placement that you stay with, you will still have to move the parts around to optimize their final placement on the board. This is a very good way though to group together connected circuitry from the schematic without having to go through and identify and move each component individually. This trick alone can save you a lot of time during placement by allowing you to organize your placement based on how the circuitry is drawn in the schematic.

    Place Individual Components Using Choose Component

    When it comes time to moving individual components around, you can position the cursor on the component and hold the left mouse button down to move the component. Did you know though that you can also type in the shortcut “m” to get into the Move menu?

    Once in that menu, you will find different move commands that you can use. One of those commands is “Component”, which will pop up a dialog box allowing you to select by reference designator the component that you want to move.

    Screen capture of AD with components placedAltiumComponent placement with one component missing

    In the picture above I wanted to find and place the component U89. I typed in the shortcut “mc” (Move Component) and then clicked in an empty area of the board. This brought up the “Choose Component” menu that you see in the picture below. Note that I have the option to select the component from a list, or to type in the reference designator at the top. I also have the option to jump to the component or to move the component to my cursor.

    Screen capture of AD with the Choose Component menu in layoutThe Choose Component menu in layout

    After selecting U89 from the list I chose the option that moved the component to my cursor and clicked OK. With U89 on my cursor, I was able to easily place it into position as you can see below.

    Screen capture of AD with the missing component placedComponent placement with the missing component placed

    This feature will save you a lot of time when you need to find a specific part of placement. Instead of searching through the schematic, or looking at all of the parts scattered around the board perimeter, you can simply select the reference designator and place the component.

    Altium Designer 18 has many more time-saving features built into it making it the premier PCB design software tool. With placement aids such as what I’ve shown you here, your focus can be on creating the best placement possible instead of trying to figure out how to manipulate the design tools.

    If you’re not already using it, talk to an expert at Altium to find out more about how Altium Designer 18 can help you with your next PCB design.

    About Author

    About Author

    PCB Design Tools for Electronics Design and DFM. Information for EDA Leaders.

    most recent articles

    Back to Home