0
\$\begingroup\$

I am creating a package for Molex's MicroAB USB 47590-0001 component because I could not find one for Eagle. My question is will this work to create the custom slots as seen in the datasheet? I've not had to mess with slots yet. How would you handle the slightly oval G4 and G5 holes, or are slightly larger circular pads good enough?

The blue is the milling layer, where the board will be cut. I see OSH Park has a page about this and they say use that layer too. The green is a via pad, which I extend with the red pad on the bottom. I opened up the green layer on the red pad as well. From what I understand, the blue should take care of the hole and the pad also creates a hole (as it does for G4 and G5) but the blue will make the custom shape.

Eagle footprint

Below is the data sheet for the connector.

enter image description here

\$\endgroup\$
3
  • 1
    \$\begingroup\$ In my experience eagle does not have a good way to do it, and typically I end up just putting a note into whatever Fab house I use. Once they understand what you're trying to do they'll tweak whatever they have to. \$\endgroup\$
    – MadHatter
    Commented Nov 28, 2019 at 19:01
  • 1
    \$\begingroup\$ I've made similar microUSB symbols, but used all surface mount parts so as not to have to deal with the thru hole mess. \$\endgroup\$
    – CrossRoads
    Commented Jan 22, 2020 at 17:54
  • \$\begingroup\$ @MadHatter interesting, good to know that is an option. I ordered through OSH Park this first time and they seemed to understand without additional instruction beyond that of what was in Eagle. \$\endgroup\$
    – jakob
    Commented Feb 14, 2020 at 5:16

2 Answers 2

Reset to default
1
\$\begingroup\$

We have had the same issue with similar USB connectors. At the present Eagle doesn't have an option for creating slotted pads, however there is a workaround described in this Eagle forum.

In a nutshell, create a component in your library that has (as described by Rachael):

A PAD on each end of the slot and then draw each of the inner/outer layer pad areas with a polygon on each of the 16 routing layers. Then also draw the slot as a line on the Milling layer.

It makes creating slots more time consuming, but once it is in your library then it is reusable as much as you like and should manufacture correctly at there PCB factory.

\$\endgroup\$
1
  • \$\begingroup\$ This is what I ended up doing and it worked! I got the boards printed and the part soldered on just fine. \$\endgroup\$
    – jakob
    Commented Feb 14, 2020 at 5:15
0
\$\begingroup\$

After printing the board through Osh Park, I can confirm that this setup worked. I have uploaded the part in the jk-connectors library on my GitHub in case anyone would like to use it. In short, the extra red layer adds a copper pour/surface to solder to. You need to open up the PCB's protective green/purple/colored layer by adding a copy of the same outline in the tStop or bStop layer. Add the hole/slot shape using the milling layer. Add a pad/pin and select the shape to be oval if you want to have to have a logic pin in the Eagle schematic or its the case that the pad's hole will work for the slot and the green copper pour will be enough to solder to.

https://github.com/jkapala/Eagle-Libraries

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.