Multiple pins with same designator?

[Araho]

Hi!

I'm having a slight hiccup with my thinking in a PCB project here. I've created a schematic symbol and footprint for an Atmel SAM4L MCU, spanning several sub-parts so I could put them on different pages. However, I get a warning when compiling the project, saying that I have

[Warning]   IC Power.SchDoc   Compiler   Duplicate pins in component Pin U1-4 and Pin U1-4

as well as some errors for duplicate net names where I have open pins.

This is kind of annoying, since I've for example put the Reset pin available on both the Power-subpart as well as the JTAG-subpart, as I feel it's logical to place all connections that are logically grouped together, together. Is this bad form, or is there a nice way of doing this?

I could probably have the pin available in only one place, and then put a port there and in the JTAG sheet, but... when I already have a part where all the other JTAG related connections are grouped, I'd be sort of miffed if I have to remove / redo the ones that are used more than one place (See picture 1 & 2). Another example is the HL6528-chip I'm using; Some pins that can be GPIO in one configuration and specific, different pins in another should be possible to group together in my head. Is this totally crazy from my side?

Same goes for ICSP-connectors and other stuff (not for this project though). So the generalized question is:
Do pins that are needed in different parts of a circuit, have to be located only one place in a schematic component?

[free_electron]

You can't do that. A schematic symbol ,even multipart is not allowed to have duplicate pin numbers.

[T3sl4co1l]

Correction, multi-parts are allowed to have duplicates.  Op-amps for example.  I'm not sure offhand if you have to tag the pins as "power" or something like that.

You can ignore the warning (or if you prefer not having the warning at all, disable it in Project Options).  Verify manually that it is creating the correct netlist.  Or, just remove the extra pin on whichever block.

Personally, putting reset on a power block seems... dumb to me.  Any block with general-purpose or system-level pins on it should be a fine place to put it.  JTAG is fine by me.  JTAG is a system-level protocol, so it could very easily be used by other chips on the board, in which case off-sheet connectors or ports would be not only desirable but required!

For sure, having the same logic pin available in multiple locations is confusing at best, and could be dangerous (say if the part gets reused later by someone who doesn't know about this..).

Tim

[ajb]

Seems to work fine as long as the duplicated pins are connected to the same net.  For instance I've got dual diodes setup as two separate diode symbols with the common pin in both parts.  Leaving one of the two symbols unconnected or connected to a different net results in a duplicated pin error.  Connecting both common pins to the same net does not.  This is a helpful sanity check that the part is connected properly.  I believe if the two pins are in different nets pushing an ECO to the PCB will attach the physical pin to both nets, one after the other--which results in whichever net is attached second being the one that sticks.

In the OP's case, naming the net at both locations ought to eliminate the error.  That said, I agree with Tim that it's kind of an ugly solution for something like a reset net.  Using a global net label at least clearly indicates that the net may pop up elsewhere, whereas unless otherwise indicated you'd assume that a pin has a strictly local scope.

[free_electron]

  PLEASE DON'T DO THIS

Soon we'll have schematics with five instances of pin 4, each on a different corner of the page, one with a pullup resistor, one with a cap to ground , one with a diode to vcc and another with a switch to ground..

the internet schematics are already total and utter crap, we don't need to give them idea's like this one.

pins in a schematic symbol need to be unique. i need to be able to follow a single pin and see ALL that is connected to it. not have to dig through five pages to see if there is another instance of the same pin with more junk attached to it.

[Christopher]

It's the kind of thing that would seriously ruin my day if I had to debug this board 

One pad on the PCB = One pin on the schematic

[Araho]

Hmm, I definitely see your points. Can't remember where, but I picked it up from a schematic I saw floating around somewhere. Won't be too hard to fix though.

I had an incling suspicion that it would be a bad idea, hence the question in the first post: "Is this bad form[...]?" - Thanks for the help clearing this up, guys!

[free_electron]

It's the kind of thing that would seriously ruin my day if I had to debug this board 

One pad on the PCB = One pin on the schematic

perfectly worded !

[Christopher]

Back in a previous body I connected all ground pads of a SOP28 to one pin in the schematic. All well and good till I powered it on and figured out I connected VSS and VDD on a non-limiting supply  .

Live and learn from stupid mistakes.. I've only been in this game out of college for almost three years and the amount of practical design/debugging I've learnt is crazy (also from your long wisdom posts on here Free_Electron).

But can I remember how to differentiate equations? Nope.

[KenGaler]

I have to agree that the pin should only have one instance.  That's truly out-of-box thinking and an interesting idea to show a pin in multiple places but I think it will cause more problems than it solves.