Actions
Forum Thread Details
  • State Not Answered
  • Replies 9 replies
  • Subscribers 180 subscribers
  • Views 1074 views
  • Users 0 members are here
Related

Overlapping connector pins not connecting

pars

Hi,

I did a brief search thru the forum but didn't see this asked already.

I am laying out a 2-sided board, and wanted to put 2 different connector footprints/pads/holes to allow the user to select which connector type to use. These are 3-pin Molex KK 0.100" and Phoenix 0.508" connectors. The center pin of each is connected to a top ground plane. In the past on commercial PCBs, I have manually added the Molex connectors in exactly this way, and they fit fine. There is also ample clearance between the pads for pins 1 and 3 of both connectors (no DRC errors).

 

If I superimpose the connectors on one another (same x-y location), the ground plane will not fill in the connection to either of these pads (2 airwires). If I move the connectors apart it works fine.

Any tips?

 

Also, I assume this might give DRC errors for drill distance? Can I just ignore those?

Thanks, and great forum!

Chris

Parents Reply Children
  • 0 in reply to pars

    On 20/09/2016 3:05 p.m., Chris Young wrote:

    Hmmm. I did a simple board (though the real one is not complex), and it seems to work fine. I've attached both board/sch files. Still can't get the actual one to work. Strange.

     

    --

    To view any images and attachments in this post, visit:

    https://www.element14.com/community/message/206041

     

    Attachments:

    molex-phoenix test.zip

    TKD 4CP test3.zip

     

     

    Hi

    You have a number of issues with your board

     

    (1) in your schematic

    Use the show command on the nets to the centre pin of J3 and X7. You

    will see the net is not connected and has a different name.

     

    J3-2 = N$1

    X7-2 = GNDL

     

    So rename N$1 to GNDL

     

    (2) Some of your thermal problem comes from the polygon wire width if

    you reduce the width to 24mil the results are better but not elegant.

     

    (3) You should use the same drill hole for the middle hole of the two

    connector styles.  The way you have it there will be two holes drilled,

    very close to one another and won't pass the board house clearance

    rules. You could move one element so that the centre hole aligns with

    the other but that would spoil the screen printing.

     

    I suggest you create a new package with the 5 pads and new tPlace

    outline in each place you have a connector choice.

    You can still have a schematic symbol with three pins. When you create

    the device, connect the pins 1 2 & 3 to pads 1 3 & 5 and append pad 2 to

    pin 1 and append pad 4 to pin 3.  Your connector position will have only

    one name on the schematic and board instead of two as you have it now.

     

     

    (4) The rear centre pin of P1 has the same drill problem of being to

    close to another drill. More thought is required here. If you are

    plating the milling then you could make a mill plunge to create the

    large hole. Board house tooling rules need to be investigated

     

    HTH

    Warren