Intel Curie Soldering Footprint ? Eagle File

Official Hardware Retired 101
1

Hey All

How I cant find the exact Information for the Intel Curie Soldering Footprint
to make my custom board.

Is there an Eagle file containing it ?

Greetings
Raphael Lang

2

I am looking for this as well. I will really appreciate that if someone finds it and posts it here.

3

The Curie layout details are in the CAD files. You'll need the Allegro viewer.

4

After looking at the datasheet and info on ball grid array footprints, my best guess for the diameters of the pad, stop, and cream layers are as follows:

Pad: 0.25 mm
Cream: 0.27 mm
Stop: 0.36 mm

I created an Eagle library with the package (no Symbol yet) that you'll find attached.

intel-curie.zip (1.66 KB)

5

Does anyone else have files to share? Or does anyone have feedback on the one I created?

6

Thanks for the library part Danterp. Did you look at the CAD files in ljardo's post? In those files, it seems to me the pad/stop/cream layers are:

Pad: 0.28
Cream: 0.25
Stop: 0.23

Note that the Stop is smaller than the Pad, it seems they opted for a Solder Mask Defined (SMD) design for this part.

For reference, they also appeared to use trace/space of 4 mil/3 mil when breaking out the pads.

Hope that helps! I am modifying your library part and can upload if you want it.

7

You can find the footprint at pag 33 of the Intel's datasheet

Hope this help!

8

Thanks you very much for the PCB library Danterp. I was wandering if there is a new updated version of the Intel Curie Footprint.
GParke, could you please upload or send a download link if you have updated version of the Intel Curie Footprint.

9

I see there has been an update with the Intel Curie Module Datasheet - now Revision 1.2.

If you look at section 6.2 you will see the following PCB pad design guidelines:

  1. pad size: 10 mil (0.254 mm)
  2. pad type: metal defined (MD) - traditional dog bone Via to BGA-Pad
  3. no non-critical to function (nCTF)

I've attached an image of Figure 6-1: PCB Pad Layout

This new information seems shows that my choosing 0.25 mm (~10mil) and Metal Defined (i.e. Stop larger than Pad) was indeed the correct choice.

I chose to make the Cream 0.02 mm larger than the Pad from what I had read online, specifically Note 5, page 7 of this document:

http://www.nxp.com/documents/application_note/AN10778.pdf

footprint.JPG
footprint.JPG784×624 56.7 KB

10

Dear All,

I also created a eagle library for the intel curie. All pins are located on the position which is mentioned in the last version of the datasheet.

There is also a symbol and a device which is ready to be used. All pins are already connected to the pads.

Hope it will help you!

best regards Ghost

untitled.zip (3.06 KB)

11

Here is an updated EagleCAD symbol and footprint for the Intel Curie.

Note that pad 1 of the Intel Curie does not have a ball, so my and Ghost's previous footprints were not correct.

intel-curie.zip (3.83 KB)