Skip to content

Added USB_C_Receptable_G-Switch_GT-USB-7025

Joppe de Zeeuw requested to merge jdzeeuw/kicad-footprints:GT-USB-7025 into master

Hello,

I would like to add the G-Switch GT-USB-7025 footprint for a horizontal SMT USB-C receptable to the Connector_USB library. I have used the GCT USB4110 footprint as an example for the design of the footprint.

Datasheet: https://www.lcsc.com/product-detail/USB-Connectors_G-Switch-GT-USB-7025_C963213.html Manufacturer product page: https://dg-switch.com/woshitype/3247.html

Edit: See note at the end, the annural ring had to be larger than the datasheet specified due to klc-check returning an error on F7.5. This is the only dimension that does not follow the datasheet specifications.

The small pad sizes used are 0.83mm high (y) and 0.28mm wide, and the wider pads on both ends are 0.45mm wide, as defined in the datasheet. The square pads are changed to square pads with rounded edges, where I used the 25% rounding as suggested.

There are some points of attention though. I would like to refer to the dimensioned drawing of the footprint below to discuss those.

GT-USB-7025_3

First, note that the two measurements in the middle of the drawing (3,515mm and 4,595mm) are defined as 3,52 and 4,60 respectively in the datasheet. This is due to rounding, as the measurements above are all valid and in agreement with the datasheet.

Secondly, I am aware that generally a triangle is used to indicate the first pin of a footprint, but as there isn't really a 'first pin' in this footprint, I am not sure whether that also applies here. Instead, I have copied the small L-shaped indicator from the GCT-4110 and placed it above the first ground pin, as seems to be common, but I would like to hear whether this is actually appropriate, a triangle indicator should be used at that grounding pin instead, or the indicator can be omitted altogether.

My third point of attention is that I simply drew a straight line down on both sides for the courtyard, where the edges of the upper S1 holes are determinative for the width of the courtyard altogether. The wider slots below are slightly less wide though, so I could cut in there to make the courtyard ever so slightly smaller than it currently is. If this is necessary/desired, I will change the footprint accordingly. I had to redraw the courtyard after resizing the annular rings for pads labeled S1 anyway, so I made the cut already. If you would rather see this reverted, let me know.

Lastly, I have decided to only put silkscreen on the front where there is definitely going to be PCB when the footprint is going to be used, as the connector can technically overhang the pcb by quite a bit. Therefore, there is no silkscreen below the long S1 slot. I am not sure whether the PCB Edge drawing on the user drawing layer should be omitted. I would like to hear your opinion on this.

GT-USB-7025_1

GT-USB-7025_2

Thanks in advance for your consideration!

Edits after the checks have ran:

  • I changed the pad sizes for the S1 labeled pads to be 0.05mm wider. Else they would be invalid according to F7.5. These dimensions will no longer be the same as the datasheet.
  • I shifted the F.fab layer to the right by 0.03mm, as the klc-check returned that this wasn't centered.
Edited by Joppe de Zeeuw

Merge request reports