They have 2 “pins”, each pin might have multiple holes. On the schematic you would have 2 pins as per the standard fuse/battery symbol. The footprint will have 2 pads, each of which might have multiple through holes. How you choose to draw that footprint is up to you. You might use one large pad with several holes, you might use several pads but they would all have the same pin number and belong to the same physical pin. This is already easily accomplished with KiCAD.
Even in the OP’s case of having a daughter board with several pins of the same name, I don’t see what the issue is. I do this all the time, currently I have a project with 3 boards each of which has a daughter board that plugs into it. As usual there are multiple power supply pins for these daughter boards. But I have never had any issues with this. I suspect the OP was misusing these pins in his design, using one GND pin for example, to supply ground to the board and another GND pin to supply ground elsewhere. I can see that causing problems but that is simply bad design. The multiple power and ground pins of a daughter board are usually intended only for supplying power to the board and should never form part of the ground path of any other circuit.
I don’t believe that KiCAD needs to change in any way to support some notion of external connections made by other boards.
I (the OP) can confirm the suspicion that I was misusing the daughter
board’s GND pins for creating kind of a second layer on my single sided
PCB where I needed to cross the GND through several signals and I
couldn’t route it any other way.
FYI, I solved it by naming the pins on the daughter board as GND1 and
GND2 and wired it in schematics the way I needed the PCB to look like.
It worked so well that I left the GND[12], TX[12], RX[12] and few other
pins in my copy of Arduino Pro Mini library since then. Granted, I have to
think a bit about the board design even when drawing the schematics but
it pays off greatly when routing the PCB.
When I do this with my battery holder, pcbnew doesn’t understand that the multiple pads are electrically connected and draws ratsnest lines among them and DRC observes it as unconnected:
Are you meaning to suggest there’s a way to not have that ratsnest line appear?
At one time I remember seeing an option to “Hide footprint ratsnest” but now I can’t find it.
I think most of us here are concerned about something called electromagnetic emissions.
If an electronic part has multiple gnd or v+ pins they should be connected to a power plane.
Yes a battery holder does not necessary need two V+ pins. (As long as the one connected can transport the whole current of the battery, In your example the trace looks quite thin. I hope the current over this trace does not exceed a few mA. Otherwise the voltage drop might be to much.)
If you want the second pin not connected to anything you can achieve it by changing the footprint. (Give it a different or an empty pin number. See for example Molex series 53398 connector mechanical pins)
It should never be the standard behavior that two pins with the same name are counted as connected if one of them is connected to the “source” of this “signal”. (how should DRC know where GND is connected to the power supply?)
I have some background in IC design. If i design an IC with multiple ground pins, the PCB designer needs to connect all of them to GND. (I would assume that they have the same electrical potential in all time instances.) Otherwise the IC might not behave as described within the datasheet.
DRC is strictly correct, they are same-net pads that are unconnected.
I have often thought it would be useful for PCB CAD tools to have a virtual-copper layer, that you could route that ratsnest on, ‘to keep DRC happy’.
The user knows they can use either pin, but DRC does not understand that, so some simple ‘jumper layer’ would allow designers to indicate what they know is OK, and DRC can find real problems.
I have exactly the same issue with switches and battery holders. In this case, using the internal connections would be perfectly acceptable and would make layout easier. I am not saying that it should be the default, but having it as an option would be great!
No, they are rated for max. 440 VAC or max 16A, not both. They are rated for 4 KVA with a resistive load, not 7 KVA. Current carrying capacity drops rapidly beyond about 25 VDC.
Those pins are only 0.5 mm dia. (.2mm2) so those ratings are based on both pins being connected.
I can’t understand why (virtually) nobody understand the real task. From an outside view (I’m just a hobbyist) this shouldn’t be worth more than 3 lines. There are so many components outside in the real world with inside linked pins. It shouldn’t need more than 3 clicks to connect them virtually inside the Footprint.
I get a headache here routing a switch matrix. The PCB is very tight. This shouldn’t be a problem if I could use the 4-pin-switches also as bridges. These are very common tactile 4pin Switches. Every switch has 2 paires of 2 pins connected inside. As they operate at very low current, it shouldn’t rise a problem to "mis"use them as Bridge or Jumper.
The divide comes from the fact that the DRC is correct in this situation. Its job is to alert you to any pins that share the same net, but are not connected on the board.
To flip the situation, what happens if someone says all of a micro controller ground pins are linked internally. Its safer to say no this is an error. I much prefer it does and leaves me to choose to work around it. If i end up making a mistake, well then its on me.
There are 2 ways to easily work around this,
1: Create your own part with different pin numbers for the internally connected pads, e.g. 2a 2b, and plonk a No-Connect to the one you don’t want to connect to.
2: edit the pad you don’t care about and delete the net entry. It no longer has a matching record so is treated as a Not-Connected until you re-import the netlist.
For most such components you must always tie these pins together on the outside. In most of these cases this is either because of EMI or current capacity.
For relays it is the later. (As @1.21Gigawatts mentioned) For most IC pins it is the former. Always connect all GND pins in the shortest possible way to ground. Don’t ever use two GND pins to jump over other traces. The same is true for VDD pins and of course for all other pins that are there multiple times.
Always remember: Bonding a package pin to the chip costs money. So if a pin is connected to the chip the manufacturer has done so because they found it is necessary that the chip is connected at all these pins.
For relays something similar is true. It also costs money to have a pin that is connected to the internals.
If your component for some reason does not need the internally connected pins to be connected externally then you can have two pins in the schematic and don’t connect them in the schematic.
Example have a NO1 and a NO2 pin. And for them not to be connected you need a NO1 net and a NO2 net. (Two different nets. In the picture by simon just remove the connection between pin 5 and pin 4)
Edit because you edited your post while i wrote mine:
Depends on your usecase really. If you have high frequency (>10kHz) signals using the internal switch connection might not be a good idea at all. (EMI)
If not you need to tell kicad that these are different pins. (Most switch footprints have the same pin number for both connected pins.)
You then need a switch symbol with four pins as well and connect them as you please. (But don’t tell kicad you need the two internally connected pins to be connected. Otherwise you are back at square one.)
Maybe there is a problem in communication. I’m not a native english
So I have no idea, what “necro-posting” means. If it means, I posted on an outdated post: The problem isn’t obsolete to me.
Rerouter, I also understand your proposal “No-Connect” as the oposite of “already linked inside”.
I did my very first steps with KiCad (switched over from Diptrace - which has it’s own problems not to discuss here).
My basic question is: If KiCad struggels at such a simple task (connecting two pins outside the copper plane), what’ll happen if it gets serious?
I am far away from insulting KiCad, cause it’s free and open.
What makes me slightly upset: it looks like nobody (virtually) understands the task.
There should be an easy way to tell the program, “these pins are already linked inside the component, you don’t have to/you mustn’t route them again”. That simple.
I love the idea of a “virtual-copper layer”. Thank you, PCB-wiz.
Concerns about current rates or other (e.g. EM-) side effects should kept in the responsibility of the designer. No matter if there is a battery holder, daughter board, micro-processor or even a simple switch.
Yes necro-posting is the act of digging up a very old thread.
I see the issue as one of defining it to the DRC, To me it is definitely and edge case, where defining it with separate pin numbers in the schematic level would ensure that it cannot come back to bite you later on.
Essentially by having one pin set as not connected, you have told the program that they don’t need to be linked, if they do you modify your schematic, push through the netlist and now they are linked.
If you really wanted to use the tool in the way your hoping with the virtual plane, you can change the project to a 4 layer board, route the trace and then change back to 2 layers, it does not delete the routing on those layers. but i warn you, this will come back to bite you if your not careful, and is not recommended
Upgrading the PCB to 3 or 4 layers (even if temporary) is the wrong way.
The clean solution should be to add one (or if necessary more) conductive layers to the component in the Component-Editor itself. Unfortunately I wasn’t able to find out, how to do this.
If I have a component in my hand (no matter if it’s an Arduino, a switch or a piece of copper wire) with two or even more physically linked pins: wouldn’t it be dorky to twiddle a workaround with extra layers on the board?
I am the only one who’s able to see that?
And what will show us the fact, I had to dig out this very old Thread?
Maybe I am the stupid myself.
Read my post. I told you the way to tell kicad that this is the case.
I also outlined where you can use this without problems. Now lets look at your examples:
Most likely either there are multiple pins for current capacity or simply for mechanical stability. If it is the later you can without problems ignore one of the pins electrically. Make a symbol and footprint that represent this fact. Or use the Not connected workaround posted by @Rerouter (The workaround is where you remove the net in pcb new from one of the pins.)
Here you always need to connect all pins together. In kicad this can be done by either stacking the pins in the symbol (preferred way). Or by creating a custom footprint that has the same pin number for all these pins. (This is how the switch footprints in the official lib are currently made.)
What is pin stacking?
Putting multiple pins on top of each other where only one pin is set to visible and all other pins are invisible. They normally have the same pin name and electrical type.
Be careful when stacking power input pins though. There the hidden pins should not be of type power input because hidden power input pins are global labels. (Yes this is a dirty hack but we need to live with it for now.)
And similarly output and power output pins also need their hidden pins to by of a different type to make ERC happy. (preferred way for these exceptions is to use passive for the hidden pins.)
Depends on application. (Current capacity and frequency of your signals)
Again if you think your application permits the use of the switch as a bridge you need a footprint that represents this fact. (The footprint needs different pin numbers for the pads that are internally connected.)
And the symbol needs to represent this fact as well. (It also needs more than one pin to represent the connected pins)
You then can tell kicad in the schematic what specific pin should be connected to what part of your circuit. This is as you already said the responsibility of the designer.
Why is it hard to do so? Well the switch footprints that are in the official lib have the same pin number for the internally connected pins. This allows the use of only one symbol for all switch footprints but makes your usecase impossible.
this is “my” thread (I was the original poster) so I thought I’d let
you know that I do understand you perfectly what you want to achieve -
as I also wanted to use the different internally connected pins as
bridges.
I am not sure if I ever posted my work-around so here it is: I mark the
pins as different ones (RX1, RX2; TX1, TX2; GND1, GND2) and then when
designing the schematics I simply use the fact that I know the e.g.
GND1 and GND2 are interconnected.
I know it’s a bad approach, it’s totally cryptic, unreadable to others
etc, but it keeps DRC happy and the final PCB works the way I want it.
I mentioned that I was the OP only to explain why I have the courage to
post an obviously wrong (yet working) work-around.
Feel free to use it. It takes a bit of imagination when drawing the
schematics (I often modify the schematics to ease the manual routing
later) but it works and Kicad is happy with it.
