Holes too small for usbc port

[Bouledogus]

Hello, I'm F4LBJ from AMSAT Francophone. I have made the CubeSatSim and I have encountered a problem with the USBC port on the STEM card. The holes for the connector harpoons are too small. I had to cut the connector studs to be able to solder it to the PCB. Could you modify the PCB to enlarge the holes?

Thanks

[alanbjohnston]

Hi,

What version of the PCB is it? Did you have PCBWay or another fabricator make the boards for you? What part number was the SMT USB-C part?

I will figure out what went wrong, but if this happens in the future, the board also has a footprint for the Sparkfun USB-C breakout board (https://www.sparkfun.com/products/15100)

73, Alan KU2Y

[Bouledogus]

Hello Alan, Thank you for your quick reply. The board version is 1.3.2b. The SMT part I'm using is USB4105-GF-A from CGT, the same one you suggest in the BOM. I used JLCPCB for manufacturing. As you can see in the picture, there is just four small holes, not enought for inserting the USB port

73 !

[alanbjohnston]

This is what my boards from PCBWay look like. I need to figure out why our boards are different using the same Gerbers.

Alan

[Bouledogus]

Hello Alan, The PCB version you have is 1.3.2.1, but on the github it is version 1.3.2b that is available. I did the test to import the gerbers 1.3.2b on PCBWay and the holes are not present as you can see on the picture below: 73 !

[alanbjohnston]

Hi,

I think I understand what has happened. For the USB-C part, there is a drill hole (.TXT file) and a mill hole (.GML file). The PCBWay Gerber viewer doesn't seem to show mill holes (in my experience, it sometimes isn't 100% accurate). If I look at the GML and TXT files from v1.3.2b in another Gerber viewer such as gerber-viewer.com, I see this:

The green is the drill layer (.TXT) while the red is the mill layer (.GML).

You might want to show this to JLCPCB and ask them why they ignored the mill layer. PCBWay did this once, but otherwise, they always follow the mill layer.

73, Alan

[Bouledogus]

Thank you, Alan, for your reply. I understand better now what's going on. I'm going to check with JLCPCB to see why the .GML file is being ignored. What CAD software are you using? I'm using KICAD and I don't have a .GML file.

73, Arnaud

[Bouledogus]

Hello Alan, I have continued my research. It seems that you are using Eagle CAD and that the gerbers are exported to the Altium format. I have studied the file naming conventions in PCBWay and JLCPCB and both do not recognize the .GML extension for Altium. Extentions for gerber files can be found here : PCBWAY : https://www.pcbway.com/helpcenter/generate_gerber/Gerber_File_Extention_from_Different_Software.html JLCPCB : https://jlcpcb.com/help/article/4-how-to-generate-gerber-files-in-different-software

I did find mention of the .GML extension at PCBWAY in a specific EagleCAD format.

This would correspond to the "Board Mechanical Layer" which should have the .GM3 extension in Altium format. I tried to simply rename the .GML to .GM3 but it didn't change anything.

Could you look into this to see if there's an error in the gerber generation?

Thanks again for your help.

73, Arnaud

[Bouledogus]

Hello Alan,

I contacted JLCPCB, he advised me to add the USBC port holes to the outline layer. Would it be possible for you to edit the gerbers in this way so that I can test whether this solves the problem? Thank you for your help,

73 !

[alanbjohnston]

Hi Arnoud,

Yes, I will give it a try.

73, Alan

[Bouledogus]

Hello Alan, I have started the PCB production with JLCPCB. I made a special request to them to consider the .GML file. They respected the request as you can see below:

However, it's not part of the automatic online process, so I think it would be a good idea to modify the files so that other people don't get trapped.

73 ! Arnaud