Hello, I frequently use USB connectors which have shield pads that aren’t connected to earth (or anything), however they insist on being connected to each other because they have the same net name. How can I stop this other than manually editing each pad every time I update the PCB from the schematic? Thanks. I can’t upload a picture here can I?
You are a basic user so you should be able to upload a picture. No connect symbols on the schematic don’t solve this?
I can upload pictures by replying to you apparently, so here we are:
No, setting no connection makes no difference, it expects pads with the same net name to be connected. I can manually set properties on each pad to stop this (by selecting no net) but updating from the schematic clears this and once again it’s the same problem. USB client connectors shouldn’t have grounded shields, only host connectors.
To be clear. On the schematic, the pads have the ‘no connect’ X chosen from the right side tool bar
and placed like this:
@hermit , this is not the case since the 2 pins of the resistor have different pin numbers.
Two pins with the same pin number still have a ratsnest line even with the non-connect x set.
If you do not want the pads on the PCB to want to connect to each other, edit the footprint and give each pad a different name.
KiCad will then probably complain that your footprint does have pads that are not represented in the schematic (and it’s right in that). You have a few options to solve this.
- Ignore during ERC.
- Flag it as exclusions during ERC.
- Adjust your schematic symbol so it does have these pins.
- Maybe more?
1 Like
Could you printscreen schematic area of this connector, with “hidden pins” option off? As far as I remember, I was not forced for same numbered symbol pins to be connected in pcbnew (or maybe I do not have symbols with same numbered pins, not sure…)
One of the ways I would try would be to add extra layer to PCB and connect that pads at that layer (and not send that layer to PCB manufacturer). May be not the best solution but I believe working one.
The shield pins are physically shorted together by the part itself, so why do you want to do this?
1 Like
He does not want to do anything.
It’s KiCad that insists on connecting pads (with the same pad number) to each other with copper.
He only wants KiCad to stop nagging about it.
Hello thanks for the replies. Updating the PCB means pressing the Update PCB… button (importing netlist), which will clear any changes I make, unless I stop it from doing that. I think creating a new footprint for non-grounded shields might be the way forward. I prefer not to ignore the ERC warnings.
This means that there should be two different footprints. You should copy the footprint (to another, personal library if it’s in the official non-writable library now) and edit it, then point the symbol to that new footprint. Then update the pcb.
I think this is a problem with the way footprints are designed. Individual distinctive pads are given the same pad number because electrically they are connected together and thus, it’s expected they should be connected together by tracks/zones by the ERC which considers them to be the same net.
Simply assigning different numbers to electrically connected pads should prevent this I think - as paulvdh says.
USB connectors do have a bit of a problem…
And once you’ve checked vendors, parts and datasheets and verified that it all works, which may easily take the better part of an hour, then renumbering some pads along the process would add about 30 seconds t that process.
And now, which of the blue USB connectors match these yellow ones?
1 Like
The problem is more complicated that it seems at beginning. Your method of giving them different numbers is not good in some other situations. Consider typical touch button. It has 4 pins connected internally in pairs.Of course you can have a symbol with 4 pins and make at schematic connection only to two of them as (from PCB) you see that you should use that pins and not the others. But the touch button symbol looks just better at schematic having only two pins (schematic should tell you how thinks works and not how it is organised at PCB). The same with coin battery having 3 pins (two of them being the part of the same badge).
Because of this something about 2…3 years ago I have (at bug system) reported my suggestion that KiCad should assume that footprint pins having the same number are just internally connected and need not to be connected at PCB. As I was told there by developers there are some important reasons against it. As I remember they are connected with generating (now or planned in future - don’t know) the files to be used in automatic testing during PCB manufacturing. I don’t understand why it is a problem but I accept that I know nothing about the internal operation of the program. Or may be it is a problem of long ago defined (by PCB manufacturers) the file format that simply don’t allow to specify that during PCB electrical checking that pins can be shorted at PCB or can be not shorted. May be at testing they simply need for each pair of copper pieces to have clear info if they are shorted or not and not accept ‘may be, may be not’.
If I were writing now form other PC I could try (not sure if successfully) to find a link to that bug report in my old mails but here I can’t and am not enough skilled to search it another way (2…3 years ago is rather long time).
In most cases I don’t agree with that sentence.
If you have two devices (like PC and printer) and each of them has its own connection to the building grounding system then yes - we should avoid ground loops.
But in most cases only one of them is really grounded (like PC and mouse, PC and keyboard, PC and small bluetooth plug for wireless mouse, …). Not all notebook supplies ground them (I think) so there are also many cases when even PC in our USB devices pair is not grounded.
In such cases I see nothing wrong in ‘grounding’ USB connectors at both sides (connecting to GND of mouse is not grounding). Connecting cable shield to mouse ground should improve its EMC.
Yes, connecting the USB shield to the equipment casing is an effective way of giving some ESD protection and avoiding damage when hot-plugging cables
I tested a bunch of USB cables and most of them have the shield connected through from connector to connector, so there must be a reason for doing that.
Some of them test open from metal to metal. Probably the cheap stuff from unknown origin.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.