No announcement yet.

micro usb footprint design help

  • Filter
  • Time
  • Show
Clear All
new posts

  • micro usb footprint design help


    Good day,

    I'm designing PCB footprint for 0475900001 molex micro usb connector. As you see in design guide, the PCB edge should have two arcs under the connector which will cut during PCB manufacturing. Please help me to design it into the footprint. I attach the following design and the assembly company reject it and ask me to correct it according to design guide.


  • #2
    fatemehjml can not you simply just use a different connector? It's not really necessary to place the connector "up side down", that is probably why the slots are required. For example, in some designs we used this 475890001 (datasheet attached here: 475890001_sd.pdf )
    Attached Files


    • #3
      Dear Robert

      Thanks for your answer.

      Unfortunately I can't change my design at this moment and I bought all my parts, But I didn't start PCB and Assembly manufacturing. WOuld you please tell me how I can implement this slots, I search a lot but I couldn't find a prepared library for that!!


      • #4
        One option could be define the slots directly in the board shape - manually. The other option could be to define slots (non plated through hole pads) inside the PCB footprint and make them longer - so they are over the PCB edge.


        • #5
          Hi fatemehjml,

          Robert explained the options you have quite well. I had a similar problem before and I ended up just changing the connector with one that doesn't require board cut-outs.

          In your situation I will just change the footprint to contain the slots using NPTH pads. To me it seems like this would be the better option during manufacturing, since they will drill out the slot at the drilling stage. Making the slot during the board cut out stage is less flexible, since the manufacturers normally offer a limited number of routing drill sizes.

          If you don't know how to make the slots using pads - it is simple. Create two pads (or better one and copy paste eventually) and from the pad properties use the following options:

          - For the hole shape select Slot and enter the appropriate dimensions
          - Enter 0 for the pad X and Y size
          - Deselect Plated to make it None-Plated


          • #6
            As an example I modified existing USB footprint, just to show how it maybe could look. This is not a real connector.

            Click image for larger version

Name:	slot example.jpg
Views:	975
Size:	329.9 KB
ID:	765


            • #7
              Click image for larger version

Name:	1.png
Views:	666
Size:	33.1 KB
ID:	2133

              Click image for larger version

Name:	image_236.png
Views:	1170
Size:	9.6 KB
ID:	2129 Click image for larger version

Name:	image_238.png
Views:	597
Size:	36.7 KB
ID:	2131
              Hi fatemehjml,

              Generally you don't need neither slot holes nor edge cutouts, nor pads overlap- all that can be easily done by usage region with property “board cutout”. The only stuff that requires slot holes is thru-hole mounting pads group- however, I can say with all confidence that manufacturer’s footprint isn't correct:

              - slot geometry is oversized
              - signal pads are oversized
              - edge cutouts are oversized

              I have experiencing of recognition various mistakes in manufacturer’s datasheet including Molex so it's not like a surprise- in this particular case, mentioned issues most probably will cause displacement during assembly: the part will be not oriented straight.
              Last edited by EVW13; 02-16-2016, 10:33 AM.