---
+ Post New Thread
Results 1 to 4 of 4
  1. #1
    Newbie level 2
    Points: 438, Level: 4

    Join Date
    Jul 2010
    Posts
    2
    Helped
    0 / 0
    Points
    438
    Level
    4

    Differential routing in altium

    Hello,

    I am creating a small PCB that basically condenses two usb jacks into one smaller socket. I want to maintain the standard 90 ohm differntial impedance between the diff pairs and It also needs to be emi shielded. my layer stackup I wanted to use is:

    layer 1 - GND
    layer 2 - usb 1 data and usb 2 power
    layer 3 - usb 2 data and usb 1 power
    layer 4 - GND

    So basically Im sandwiching the signal planes between two ground pours. In order for Altium to run the diff pair routing, you need your diff pairs adjacent to an actuall power/gnd plane which would mean an extra 2 layers in the design. So i downloaded satrun PCB Design which is a software that lets your calculate deminsions for all sorts of pcb transmission lines. I chose the differential offcenter strip line but It doesnt seem to be giving me the proper outputs.

    Is this the correct choice because layer 2 needs a reference to layer 1 and 4 which would make it off center. Likewise for layer 3. or am I missing something.

    •   Alt8th July 2010, 20:09

      advertising

        
       

  2. #2
    Full Member level 4
    Points: 3,970, Level: 14

    Join Date
    Feb 2002
    Location
    USA
    Posts
    201
    Helped
    24 / 24
    Points
    3,970
    Level
    14

    Differential routing in altium

    Here is what I have just as a general rule.
    (Note: you should always talk with your fabrication vendor and ask them to propose a stackup)

    1. 4 layer board assuming fr4 material
    2. .5 oz copper on internal layers (1.5oz on external after plating... 2.05mil to 2.2mil or there abouts)
    3. layer 1 and layer 2 will be a core (10mils)
    4. layer 3 and layer 4 will be a core (10mils)
    5. between layer 2 and 3 will be prepreg )approx: 36mils)
    6. trace width= 9mils
    7. space will be 5.5mils
    8. traces on layer 2 will reference layer 1 plane.
    9. traces on layer 3 will reference layer 4 plane.

    You will want to avoid crossing traces over between layer 2 and 3.
    Because of the distance between L2 and L4, there is very little effect from having the mixed dielectric. The same is the story between L3 and L1.

    You should have no trouble setting up differential pairs in altium. Having to have a reference plane is not true. Unless you are trying to autoroute. I am not sure why that would be wanted for usb signals.

    regards,
    Eda



    •   Alt8th July 2010, 22:45

      advertising

        
       

  3. #3
    Newbie level 2
    Points: 438, Level: 4

    Join Date
    Jul 2010
    Posts
    2
    Helped
    0 / 0
    Points
    438
    Level
    4

    Re: Differential routing in altium

    Edab,

    Thank you very much for your reply. I have some things I would liek to discuss though.

    This is a 4 layer using FR4
    I agree with the copper weigh

    For the layers if I was to set it up the way you are specified in altium. It puts the power planes on layer 2 and 3 and the signal on 1 and 4. This is not what I want cause I want to isolate the signal layers inside the board in a differential stripline configuration. The way I have it set up now is:

    Layer 1 gnd pour
    then a 6 mil prepeg
    Layer 2 signal layer
    then 45.4mil core
    layer 3 signal layer
    then a 6 mil prepeg
    layer 4 gnd pour

    traces on layer 2 will reference top and bottom gnd pour
    likewise for traces on layer 3 (hence the reason for the differential offset stripline)

    With that configuration and the program I used to determine the width and spacing. I got a 15 mil width and 8 mil spacing using a 4.6 er. does this look right to you.

    You were right with the differential routing. I am able to do that in altium, what I meant was that I was unable to do impedance controled routing without a power/gnd plane reference. You are also not able to do differential impedence controlled routing. That is why I started to look for programs to help me compute the proper dimensions.



    •   Alt9th July 2010, 19:38

      advertising

        
       

  4. #4
    Full Member level 4
    Points: 3,970, Level: 14

    Join Date
    Feb 2002
    Location
    USA
    Posts
    201
    Helped
    24 / 24
    Points
    3,970
    Level
    14

    Re: Differential routing in altium

    Uh....

    With the exception of of distance from signal layer to GND reference my suggested stackup is identical.

    The formula in Altium is setup for single ended impedance, I believe you can edit this to enable modeling for a differential pair.

    Regards,
    Eda



+ Post New Thread
Please login