Announcement

Collapse
No announcement yet.

How to show nets on only selected components during placement?

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • How to show nets on only selected components during placement?

    Hi, I have videos from the layout course that shows that when a component is selected, during placement, nets are hidden until the component is selected. This, I can see, makes it easy to see the best position or layer for a component. On my system, using Altium 18.1, I have options to view->connections where all connections are visible or no connections are visible. I have not been able to see in the documentation how to show nets on a component while moving it around.

    Thank You
    Tom

  • #2
    Hold SHIFT: https://www.fedevel.com/designhelp/f...g-highlighting

    I am also showing it here: https://youtu.be/L36KicrU45Q?t=903

    Comment


    • #3
      Robert, Some components, when selected, show net hightlighting. Other components, when selected, do not show highlighting.



      Hopfully, this video will show what I mean.

      Tom

      Comment


      • #4
        Hmm, I do not know. Sometimes this happen to me too, but I have never really investigated why it is happening. Did you try to close the PCB and open it again? Also, are not the connectors locked down?

        Comment


        • #5
          Robert, "It's not a feature, it's a bug". I spoke to Altium tech support and they said the following:

          "This is a bug that seems to affect larger component. The suggested workaround is to open Preferences>System>General>Click the Advanced... button located on the bottom right. When the advanced settings dialog pops up go to PCB.ComponentDrag.ConnectionLimit and change the Value from 50 to a much larger number like 500. "

          I tested this workaround and it works.

          Regards
          Tom




          Comment


          • #6
            WOW! Thank you miner_tom for sharing this. That really is interesting.

            Comment


            • #7
              Cool I did not know this either!
              I used to do this:

              in the PCB push "N" hide connections -> all , then "N" again choose Show connections on component, this way only connections from that component are shown. use this a lot when placing components on the board. (make sure you have nets shown on in the view configuration - system colors)

              Comment

              Working...
              X