Official library poll: Should mounting pins for connectors have a connection on the schematic


#1

Clarification: I am not talking about shielded connectors here. This is only for connectors that have smd or tht pads purely for mechanical strength. These “pins” do not offer any electrical connection to the cable. Examples would be the two metal pins encased in plastic on the side of Molex picoblade connectors

Why would it make sense?
In some cases it might be a good idea to connect such pads to a larger copper area (=zone) to increase the mechanical strength or to allow that zone to connect to an area that would otherwise be blocked off by the mounting pads.

What would be the cost?
We would need to add special symbols to the library that include a mounting pin. This pin would get a special pin number (Example “MP”)
This would double the number of connector symbols in the lib. It would also mean we would need to add some suffix to footprints that have such a mounting pin to allow correct footprint filtering.

The discussion over at the library repo: https://github.com/KiCad/kicad-footprints/issues/117


#2

They do need a special filter anyway, just to ensure the mounting pin has somewhere to land.
I am assuming that these pins are isolated, so they might be connected to different nets.
On the other hand we don’t want DRC errors if they end up unconnected


#3

So you would even go further and offer the option to connect each mounting pad to a different net? Well that would result in even more symbols. (Not all connectors have exactly two mounting pads.)


#4

I suspect it is one of those cases where one size does not fit all. For example, safety regs might require all externally accessible metal parts to be safely grounded. Additionally, ESD compatibility might require metal contacts to be terminated in a particular. OTOH, connectors inside an enclosure might have quite different requirements. It is likely some “house rules” apply which differ by company/user.

As I said before, standard parts are like a “serving suggestion”. They likely meet most users requirements, but will never be all encompassing. The atomic part concept is a bit of a slippery slope…to capture every variant means a LOT of data.

It might help if it was easier for users to generate modified parts, but I think you would need to get into parametric part handling for users (e.g. “I want all connectors of type X to automatically connect shield pins to ground”).

In this case where tabs are intended for mounting, I would make them unconnected pads.


#5

Is the behaviour of NC pins suitable?


#6

In my opinion, only electrical pins should be present in the schematic.

If someone needs to connect the mounting pads for a special case, then he/she can add the pins to an own connector symbol.And the same for the footprint.


#7

The cases I can think of:

  1. Shield pins. These are connected to one or more of : a metal screen (e.g. a can enclosing the connector), metalwork intended to contact a metal enclosure, or will connect to a signal pin or shielding part of the mating half.

    Often these combine into the same metal piece, but not always.

    In all these cases I think the pin needs to be a numbered pin which can be assigned in the schematic, since the appropriate termination depends on application. The tab or pin used for shielding also helps with mechanical support.

    Examples

https://uk.rs-online.com/web/p/products/3316443/

http://www.hspcon.com/product/a/mini-din/pcb-socket/mini-din-pcb-socket-a-1005.php

  1. Metal tabs that are not connected to any of the features in part 1, and are only used for mechanical support.

e.g.


#8

Yes. Unambiguously. I would prefer that anything that can carry a charge should be able to be set to a specific potential.

While this is not important at low frequencies, it becomes very important at high frequencies and in rf-adverse environments. Having floating metal bits in high frequency chamber is asking for charge build-up, sparking and very bad behavior. There are probably other cases where this is relevant as well.


#9

This could be through-hole pins as well as SMT tabs. No electrical function; just mechanical support. They definitely need a pad on the footprint, but making them “NC” isn’t always desired. Suppose it is convenient to include them in, e.g., a ground zone? The “NC” designation prevents this.

Dale


#10

Sure, its a tradeoff. As I hinted earlier, if we want to encompass every possible use case then we are forced down the fully atomic road, i.e. each connector variant has a dedicated symbol and footprint.

I guess a compromise might be to group non-electrical pins under a single pad name (or number). DRC will then complain if they are left unconnected.


#11

I don’t like to see a schematic cluttered with mounting pins. (Didn’t we recently have this discussion regarding a symbol placed on the schematic to represent mounting holes?) On the other hand, if the pin is visible on the schematic symbol you can flag it “NC” or connect to an appropriate fill zone.

Dale


#12

Read my first post again. Specifically the first paragraph. I did specifically state that this discussion should be only about your case 2. Symbols for shielded connectors already exist. We only need to add the information about shield handling to the KLC. (Currently it is kind of unofficial.)


#13

Well, for completeness I was also considering the cases where there is a pin or tab with electrical connection but not to the cable, which strictly speaking wasn’t included in your definition. However, I think we are in complete agreement on the point in question. I apologise if that distracted from the main discussion.


#14

Purely mechanical stuff, not touchable from the outside of the completed device: nothing on the schematic, footprint with pad or PTH.
Anything else, “it depends”. Solving that on library level, for me that would be pure luxury, gladly accepted, but not a necessity.
I’ll take a symbol and a footprint from the library to make it fit to my whims (separation of protective and signal ground, ESD, EMI and so on) without thinking twice.

Regarding mechanical strength, for internal connections I expect the manufacturer’s footprint recommendation to be good enough, for connections to the outside world, I prefer tht connectors anyway. Yes, it would make sense, but for me, the price of at least doubling the library is a bit high.


#15

+1

I share the same view


#16

If people prefer only to have electrical pins present in the schematic, simply use the old symbol?
It doesnt give any Import netlist warnings, DRC warning etc.
With this approach we would get the new feature and still be able to use it the old way.
I dont really see any drawbacks.

both symbols have the same footprint assigned
OBS: pad names, symbolshapes etc are only examples



#17

Important point. You can hardly argue that it’s a drawback to add this.

Personally I think it would be a little more neat to just name all the mechanical pins more like exposed pads. IE, number of pins + 1, 2 or however many mechanical pads there are. This means you can also use the existing symbols.


#18

If we remake the footprints that will not work. That’s the problem. We can not add optional pins to footprints.

  • The footprint filter of the normal symbol will not find the correct footprint (Pin count differs)
  • and the net list import will should complain that it can not find footprint pads in the symbol. (For some reason it really does not throw a warning. I suspect that this could change with the new symbol format as it will allow better handling of NC pins.)

If we do this it must be done properly.


#19

This is sub optimal at best. If you use the 4 pin symbol to represent a 2 pin connector with 2 mechanical pins (that have no electrical connection to the outside world) and give your schematic to someone else, what do you think this person would expect to find on the pcb? Will they expect a connector with 4 outside connections or with 2? (What will you expect 1 year down the line?)

In your personal lib you can make such bodged footprint/symbol pairs but the official lib should do it properly.

Again if we want this, we will have at least double the amount of symbols for connectors and the user must choose a symbol with the correct number of mounting pads for their connector to get an error free pcb/schematic pairing.

It is double if we give all mounting pads the same pin number and only add one pin to the symbol. If we want to have one number per mounting pad the amount of needed symbols will skyrocket.


#20

I can see that’s troublesome

Is that a nightly thing? I can only get an error when symbol pins are not found in footprints.