Announcement

Collapse
No announcement yet.

Width of single-ended signals (Advanced PCB Layout Course)

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

  • robertferanec
    replied
    1) For high density designs and the stackups what I normally use, 50-55OHM impedance is 0.1mm and smaller inside of the PCB. Of course for cheap PCBs you may want to use different numbers e.g. start layout with a track 0.2mm or 0.3mm so you can go down to 0.15mm if needed.

    2) You do not have to, but it will make it easier if a PCB manufacturer needs to manipulate with track width to adjust the impedance. By putting them back to 0.1 and routing after that, you will be sure, there will be minimum clearance same between all the tracks (even when you make tracks thinner). If you do not change the width back to 0.1mm, you may for example end up with 0.08 tracks routed with 0.1mm gap and if needed, these would not be possible to make wider (e.g. increase them to 0.09mm), because then you would go below 0.1mm standard clearance.

    Leave a comment:


  • Width of single-ended signals (Advanced PCB Layout Course)

    Hi Robert,
    I just finished lesson 7 of the Advanced PCB Layout course. Thank you, there is a lot of wisdom in the course. However, I would like some addition clarification on the issue of dealing with the width of the normal (single-ended) signals. Here is my understanding of your recommendations, followed by 2 questions.

    In the course you referred to two phases of routing as described below.

    Phase 1: In the first phase you do not have the final stackup from the PCB vendor yet, so you just start with a basic stackup and for a dense board you recommended to start with 0.1mm traces and 0.1mm gaps. You just connect up all the signals in this phase, with the expectation that you will likely be changing them in phase 2.
    Phase 2: Before you start phase 2 routing, you should have a final stackup from the PCB vendor, so you can generate rules to drive the impedances of the high-speed signals. You will then redraw the differential signals using the widths and gaps specified by the PCB vendor, and do preliminary length matching on the signals which require that treatment. In the final stage of phase 2, final length matching is performed. The very last step you suggest is to adjust the width of the single-ended signals (which should all still be 0.1mm) to result in the desired 55ohm impedance.

    In Lesson 7 you stated that if you ever needed to change the design, you would change those single-ended signals back to the 0.1mm width before making the changes, and then change them back to the proper width after making the changes.

    Question 1 - In the course, the traces of the single-ended signals on the module needed to be made smaller, the 0.1mm traces went to either 0.093mm or 0.08mm (depending on the layer), so that would not be a problem. But what if the widths had to be bigger that 0.1mm? That might create the need to do significant re-routing. If you have the detailed PCB stackup at the beginning of Phase 2, why wouldn’t you change the rules to use the correct width/impedance, so that during early Phase 2 routing you would be using the correct widths? Why wait until the end to change them?
    Question 2 - If changes need to be made to the board after the board is released, why would you need to go back to 0.1mm on those traces before making the needed changes, and then change them back to the proper width after making the changes?

    Thank you!

Working...
X