Forum Rule: Always post complete source code & details to reproduce any issue!
Results 1 to 8 of 8

Thread: Importing Ethernet Kit PCB Traces into Larger PCB

  1. #1
    Junior Member
    Join Date
    Apr 2021
    Location
    Colville, WA
    Posts
    4

    Importing Ethernet Kit PCB Traces into Larger PCB

    Hi,

    I am laying out a fairly extensive PCB for prototyping using a Teensy 4.1. I am already using the Teensy 4.1 with the Ethernet Kit and it is fully functional (except for the activity lights on theEthernet Magjack Cetus J1B1211CCD which I hope to one day figure out how to make operational but that is another story).

    I would like to incorporate the Ethernet Kit PCB into my project PCB to get rid of this tiny PCB flopping around on the end of the ribbon cable with the potential of shorting out to extraneous things/tools that I carelessly have laying around on my test bench. Is pjrc amenable to providing the trace patterns for both sides of the tiny PCB so I can incorporate it into my project board (I use KiCAD)? I hope you do not think this request to be too presumptuous.

    Thanks,
    Ken
    N7KD

  2. #2
    Senior Member
    Join Date
    Mar 2016
    Posts
    335
    Hi, Ken, there really isn't much magic to the traces. Since the goal is to have equal lengths, the Kit board traces won't help you very much. For the receive and transmit lines, I would use differential routing to get equal lengths on the P and N lines. Most EDAs have diff routing and it is generally pretty easy to make work (though Eagle is pretty quirky). Kicad's is far better than Eagle's. Unless you are doing fairly long traces, I wouldn't worry about impedance matching.

  3. #3
    Junior Member
    Join Date
    Apr 2021
    Location
    Colville, WA
    Posts
    4
    Hi Phil,
    Thanks for the quick reply. My traces would be ≈ 2 inches. Does that qualify as "fairly long"?

  4. #4
    Senior Member PaulStoffregen's Avatar
    Join Date
    Nov 2012
    Posts
    24,081
    Quote Originally Posted by n7kd View Post
    Is pjrc amenable to providing the trace patterns for both sides of the tiny PCB
    Sure, why not.

    Click image for larger version. 

Name:	eth1.jpg 
Views:	9 
Size:	9.8 KB 
ID:	24463

    Click image for larger version. 

Name:	eth2.jpg 
Views:	7 
Size:	14.8 KB 
ID:	24464

    Hopefully no big surprises here, since you should be able to see these traces by just looking at the PCB before soldering.

  5. #5
    Senior Member
    Join Date
    Mar 2016
    Posts
    335
    50mm is ok. Just length match them. Ideally, you would run the T and R pairs next to each other as much as possible. Here is what I did on my most recent T4.1 board. Note, that is for a different MagJack so different pinout - I think the designers take delight in making every one have different pinouts.

    Click image for larger version. 

Name:	traces.png 
Views:	14 
Size:	190.6 KB 
ID:	24465

  6. #6
    Junior Member
    Join Date
    Feb 2021
    Posts
    15
    Quote Originally Posted by n7kd View Post
    My traces would be ≈ 2 inches. Does that qualify as "fairly long"?
    The ethernet kit that PJRC sells for the 4.1 has a ribbon cable that is at least 4 inches, so I doubt 2 inches of PCB trace would be considered long. As Phil said: match the lengths.

  7. #7
    Junior Member
    Join Date
    Apr 2021
    Location
    Colville, WA
    Posts
    4
    Hi Phil,

    I have mostly worked this out except for KiCADs tuning of the differential pair of traces. One would think that you would use "Tune Differential Pair Length" but that produces bizarre results in that no matter which trace of which pair I select it tells me that BOTH traces of the pair are too short and should be 3.9370 inches long. I have no idea where 3.9370 inches comes from and this result is nonsensical. Using "Tune Differential Skew/Phase" produces sane results.

  8. #8
    Senior Member
    Join Date
    Mar 2016
    Posts
    335
    The UI is a little obscure.

    - Route/Differential Pair. Get as far as you can. hit escape
    - Finish using individual routing.
    - Route/Tune Track Length.
    - Click on which ever is the longest of the pair. It will tell you the current length (Too short: xx.yy mm/100 mm. Remember xx.yy.)
    - Voodoo Alert #1 --- Press <ctrl>L That gets you the Single Track Length Tuning panel. Enter xx.yy in the Target length.
    - You might want to play with Min and Max amplitude. I like .5 and 1 but play with it a bit.
    - Hit ok
    - Now, click on the shorter track and move the mouse cursor up and down along the track. See the pretty meanders!
    - Voodoo Alert #2 --- the 1, 2, 3 and 4 keys control spacing and height of the meanders. Play with it until you get an exact length match.

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •