A new pad property warning

[Jonathon_Doran]

I am fighting with this USB C connector, as previously mentioned. Right now I am fighting a few DRC violations.  I switched out a footprint (not sure where I got it) for one that I exported from EasyEDA and then imported into KiCad.  This got rid of crazy edge cuts in the middle of the board.  But a couple of pads lost their net.

No problem, I assigned a net to them.  And there were violations with the pads being too near the drill holes.  So I shrunk the pads a bit (still plenty of room for soldering).

Attached it the warning that I received.  I could find nothing online about this.  KiCad shows a solder paste for the smaller area of the pad.  What in the world could this warning be trying to tell me?

Edit:  As near as I can guess, this might be telling me that it is truncating the solder mask to reflect the smaller pad area.  I would like confirmation if possible, given that it is saying that no solder mask will be generated.

[ataradov]

That connector must already exist in the KiCad library, it is the most generic Type-C connector out there.

Importing things from other EDAs is guaranteed to break something.

I think your imported connector also has incorrectly specified slots, so it may not be suitable for manufacture.

[Whales]

Please link to your previous topic, it makes it easier for people to help you.  https://www.eevblog.com/forum/kicad/how-to-route-this-usb-c-connector

You cannot trust auto-conversion of footprints between different PCB packages.  They all work slightly differently.  You need to go through every layer in the footprint and work out what it does.

This got rid of crazy edge cuts in the middle of the board

That's weird.  Were these cuts on a comments layer (suggesting where to put the board edge) or the actual Edge Cuts layer?

You can edit any footprint (including removal of edge cuts if they're in a footprint for some reason).

Also note that putting a right-angle USB-C connector in the middle of a PCB won't work, they are not high enough off the board to let you fit a plug.  The plug is thicker than the connector itself (it has a plastic shroud).  If it's designed to be used on the edge of a board then it won't work anywhere else.

[ksjh]

That connector must already exist in the KiCad library, it is the most generic Type-C connector out there.

Importing things from other EDAs is guaranteed to break something.

I think your imported connector also has incorrectly specified slots, so it may not be suitable for manufacture.

Even when you use the Connector_USB:USB_C_Receptacle_G-Switch_GT-USB-7010ASV footprint in KiCad 8 and leave all the board constraints at the default settings, you will get loads of Hole clearance violation errors for the NPTH pads. This is even before routing anything, just after placing the component, you will already get those errors. The distance of the GND pad to the NPTH is just 0.1751 mm in this footprint. So, please check if the default board constraints are fitting for your PCB manufacturer.

[Jonathon_Doran]

That connector must already exist in the KiCad library, it is the most generic Type-C connector out there.

Importing things from other EDAs is guaranteed to break something.

I think your imported connector also has incorrectly specified slots, so it may not be suitable for manufacture.

The connector in the library does not agree with the datasheet.  I went with the EasyEDA footprint because it matched the datasheet.  I realize now that I should have looked through the footprints in KiCad library and found one that matched a part that was in stock.

I don't have any experience with USB-C, so I am trying the best that I can.  There was one 16-Pin connector in the symbol library, and it doesn't match any of the connectors that I find in stock at JLCPCB.

My next plan is just to make my own symbol.

Please link to your previous topic, it makes it easier for people to help you.  https://www.eevblog.com/forum/kicad/how-to-route-this-usb-c-connector

You cannot trust auto-conversion of footprints between different PCB packages.  They all work slightly differently.  You need to go through every layer in the footprint and work out what it does.

This got rid of crazy edge cuts in the middle of the board

That's weird.  Were these cuts on a comments layer (suggesting where to put the board edge) or the actual Edge Cuts layer?

You can edit any footprint (including removal of edge cuts if they're in a footprint for some reason).

Also note that putting a right-angle USB-C connector in the middle of a PCB won't work, they are not high enough off the board to let you fit a plug.  The plug is thicker than the connector itself (it has a plastic shroud).  If it's designed to be used on the edge of a board then it won't work anywhere else.

Sorry about not linking, but in my mind this was a separate topic.   I wanted to know what KiCad was telling me.

I chose my words poorly there, when I said that the edge cuts were in the "middle of the board".  The connector is on the edge, but the footprint that I found (that matched the exact manufacturer and part# of an available connector at JLCPCB) had edge cuts for the shield holes.  These were not on the edge of the board, so were in the interior (middle) of the board.  KiCad did not like this, and I don't blame it.  The connector was on the edge, sitting a bit over it to be honest.

The cuts were in the edge cuts layer.

This is moot because I see that JLCPCB #C2894897 is in stock and has a footprint in the KiCad library.  The footprint looks like the datasheet.  There is no symbol to match it, but that is an easy fix.  In the time that I've spent trying to make the wrong footprint work I could have made 100 symbols. 

This is a learning opportunity.

That connector must already exist in the KiCad library, it is the most generic Type-C connector out there.

Importing things from other EDAs is guaranteed to break something.

I think your imported connector also has incorrectly specified slots, so it may not be suitable for manufacture.

Even when you use the Connector_USB:USB_C_Receptacle_G-Switch_GT-USB-7010ASV footprint in KiCad 8 and leave all the board constraints at the default settings, you will get loads of Hole clearance violation errors for the NPTH pads. This is even before routing anything, just after placing the component, you will already get those errors. The distance of the GND pad to the NPTH is just 0.1751 mm in this footprint. So, please check if the default board constraints are fitting for your PCB manufacturer.

That is going to be the case with any of these footprints.  They do not meet JLCPCB's capabilities.  I believe I can move the back of the pad away from the hole.  I don't think I need 1.118mm of pad for something JLCPCB will assemble.

And, as was stated earlier, if this the most generic Type_C connector out there, JLCPCB must have a ton of experience with it.  I asked them.  They told me to pick a different part...

I could see them going through thousands of these connectors in a month.  This is not their first rodeo.  Has anyone used one of these connectors with JLCPCB?  If so, I would like to know what part, and what footprint.  Plus what was done regarding the pads too close to the drill holes.  Also, as I look at the picture of this connector, there are metal tabs that look like they might need to sink into the board.  How do you handle these?

[ataradov]

Here is the exact connector I use in all my designs https://www.lcsc.com/product-detail/USB-Connectors_XUNPU-TYPEC-304J-BCP16_C2835315.html

I don't have a public library, but you can extract the footprint that works with all the regular manufacturers from one of my project. This one, for example https://github.com/ataradov/free-dap/tree/master/hardware/d11-nano-dbg

[ksjh]

They do not meet JLCPCB's capabilities.

And yet, I just hand-soldered a prototype PCB with exactly the footprint I mentioned earlier. The PCB was manufactured by JLCPCB without any complaints. Since I used some 0402 resistors, I had to use the microscope anyway and thus could inspect the USB footprint on the manufactured PCBs in detail. In this and all of the previous orders from JLCPCB, I did never see any problems with this footprint, even so it violates the official limits. For production runs, I would be more careful, but for prototyping, it was fine to simply go with the standard KiCad footprint. I used the connector the KiCad footprint is intended for this time, https://www.lcsc.com/product-detail/USB-Connectors_G-Switch-GT-USB-7010ASV_C2988369.html, but have also used the same footprint for even cheaper ones like https://www.lcsc.com/product-detail/USB-Connectors_DEALON-USB-TYPE-C-018_C2927038.html. I think Alex is right, I also believe this is one of the most generic USB-C footprints.

EDIT: I attached some PCB photos. As you can see, using the mentioned footprint, some of the SMD pads adjacent to the NPTH lost some copper in the corners during the manufacturing process by JLCPCB, but this is nothing that bothers me or caused me any problems for soldering. But I am not sure how a stencil would look like.

[ksjh]

There was one 16-Pin connector in the symbol library, and it doesn't match any of the connectors that I find in stock at JLCPCB.
My next plan is just to make my own symbol.

Why? What part of the symbol did not match?

The connector is on the edge, but the footprint that I found (that matched the exact manufacturer and part# of an available connector at JLCPCB) had edge cuts for the shield holes.  These were not on the edge of the board, so were in the interior (middle) of the board.  KiCad did not like this, and I don't blame it.  The connector was on the edge, sitting a bit over it to be honest.
The cuts were in the edge cuts layer.

Perhaps there was another problem with this footprint, but this is exactly how to specify routed slots in KiCad. Not only should this not cause any errors, it is simply the right way to do it.

There is no symbol to match it, but that is an easy fix.  In the time that I've spent trying to make the wrong footprint work I could have made 100 symbols. 

Again, why? Electrically, it is the same 16 pin USB-C connector. Why do you see the need to create another symbol? What is wrong with using USB_C_Receptacle_USB2.0_16P?

Also, as I look at the picture of this connector, there are metal tabs that look like they might need to sink into the board.  How do you handle these?

Hm? This is what the plated routed slots are for (those on the EdgeCuts layer). Or do you mean something else?

[Jonathon_Doran]

Please keep in mind that I am new to this, and so I don't know what compromises/changes can be made.  Unless everything matches, I'm convinced the project will catch fire and kill my pets.

The symbol for a 16Pin does not have the MID pins for one.  The footprint did, but not the symbol.  Not a big deal.  I'll look at your connector and footprint (thanks much!).  What I saw on my previous attempts was that the cutouts would fail DRC because of edge cuts not being contiguous.  There was also a failure due to some pads being too close to drilled holes under the connector.

I first looked at this Hirose part (C2889324), and the datasheet had pins that was not on the EasyEDA footprint/symbol (linked from JLCPCB).  So I went in search of other parts.  This Shou Han part looks good (#C668624).  But the footprint is a bit different.  This is what I was trying to layout last night.  I have no way of knowing which footprint in the KiCad library would be appropriate for this.  That is why I went off in search for another source, and eventually just installed EasyEDA and exported the footprint.  I now learn that was a bad idea.  I was starting to think I should  find a part that was available at Mouser, buy one, and go to town with some calipers.

I could just see JLCPCB saying "no" to that, and I wouldn't have a clue how to respond.

But not matching the connector (to me) means that there would have to be a perfect match.  And I was hampered by not being able to find many connectors in stock there.  Using LCSC's search engine has made my life a lot easier.  Sometimes just knowing a part number makes a whole world of difference.  "Nope, don't have any"...  "What about part #xxxxxxx?"....  "Oh, yeah, we have 2000 of them."

I feel like I am learning a lot about how to negotiate this process.

Sorry to ask so many beginner questions.  I wouldn't attempt something like this, but Logitech discontinued my favorite keyboards.  If anything happens to the ones I have (that still work) then I am in dire straits.


I just have a few things to clean up, and then I can submit the design in the projects forum for public comment.  I have spent weeks on this thing, and it isn't that complicated!

[ataradov]

The symbol for a 16Pin does not have the MID pins for one.

What are "MID" pins?

I first looked at this Hirose part (C2889324)

This is a midplane mount connector, it needs a board cut out and the connector is physically located in the board plane, not on top of it.

This Shou Han part looks good (#C668624).

This is the same generic connector size/pinout. If a connector visually looks like this one, it will be the standard size. Connector manufacturers are not stupid, they won't make parts that are almost the same, but slightly different. They all want to replace competition in the product, and designing compatible parts is a way to go here.

I could just see JLCPCB saying "no" to that, and I wouldn't have a clue how to respond.

You fix what they say is wrong. They won't just say "no" without explanations.