Add TI TO-PMOD-11 / NDY0011A

[ottojo]

Add TI TO-PMOD-11 / NDY0011A

This adds the footprint for the TO-PMOD-11 package used by TI "SIMPLE SWITCHER Power Module" DC/DC buck converters.
PR for symbol at KiCad/kicad-symbols#1716.

I couldn't figure out in which footprint library this belongs, and would greatly appreciate if someone could point me towards a more fitting one.
Same with footprint naming: It seems to be both referred to as "TO-PMOD-11" and "NDY0011A".

The corresponding 3D Model is available for download from the manufacturer here.

Datasheet is here.

---

All contributions to the kicad library must follow the KiCad library convention

Thanks for creating a pull request to contribute to the KiCad libraries! To speed up integration of your PR, please check the following items:

• Provide a URL to a datasheet for the footprint(s) you are contributing
• An example screenshot image is very helpful
• If there are matching symbol or 3D model pull requests, provide link(s) as appropriate
• Check the output of the Travis automated check scripts - fix any errors as required
• Give a reason behind any intentional library convention rule violation.

[evanshultz]

Welcome and thanks for contributing!!

Review notes:

1. As shown at http://www.ti.com/lit/ds/symlink/lmz10505.pdf, and inspecting the package, this is a TO-style footprint so let's put it in the Package_TO_SOT_SMD library.
2. Please add to description with the size and other info along with the URL.
3. Consider the footprint and pads together, not just the body size to pick the footprint center.
4. Courtyard should be 0.25mm bigger than the extents of pads or board.
5. The fab layers needs a pin 1 mark. A triangle sticking into the fab outline would work nicely here. See many of our connector footprints for an example.
6. The silk also needs a pin 1 mark. Perhaps a vertical line next to pin 1 and meeting the existing silk outline, keeping at least a line width clearance (0.12mm) to the pad.

Also, we can't accept third party models for licensing reasons. The 3D model is OK for your library but we won't be able to accept it into the KiCad library. Just FYI.

[ottojo]

Thanks for the feedback, i think i resolved all your comments.
Also thanks for clarifying the 3D model situation, i anticipated it would be like that, but wasn't sure.

[evanshultz]

Thanks!

FYI, the three-letter name ("NDY" here) is the most accurate TI package naming system. I'm not sure why they make it so confusing...

Dimensioned drawing:

The only problem is excessive courtyard offset where I circled above. Then it's ready to merge!

You could also consider flipping the pin 1 mark on the fab layer so it touches the pin 1 pad. Or adding a bevel to the corner of the fab outline nearest pin 1. But I think any way is OK so you choose whichever version you prefer.

[evanshultz]

Thank you!

The corner of the fab layer for the flipped pin 1 mark now sticks out past the part boundary:

Perhaps make it 1mm wide instead of 2mm wide?

[evanshultz]

Nice. Thank you!