Using 0 ohm resistors

[mark9XJEG]

I am designing a single layer board, and the routing has split my GND polygon into two separate areas.

I have added a 0 ohm resistor, to act as a jumper and restore continuity between the two GND planes - but Eagle PCB continues to show an airwire between the two.   Is there some way that I can modify my 0 ohm resistor component so that Eagle PCB knows that it provides a connection between the two ends?

[one-of-the-robs]

Using a resistor component is the wrong way to fix this. If you show it properly in the schematic then you'd have to split the ground net, and then you're going to be forever messing with which net you use for what part (and why)

The easier way to design for a single-sided board with a few jumper wires is to design a double-sided board but be very sparing with top-side tracks. Avoid top-side connections to components, keep all the top-side traces short, straight and directly between two vias. Then ignore the top side when etching the board and use it instead as a guide to where you put wire links. This does mean you have to route it manually as the autorouter can't be told to behave that way. but then it's pretty hard to make an autorouter do the right thing on any board.

[mark9XJEG]

Thanks Rob, although I may not have been clear - the board is an aluminum board, all surface mount, so there are no wire jumpers - I am using 1206 O ohm resistors in lieu of wire jumpers.   What would be nice is if I could somehow fool the library into thinking that the 0 ohm resistor has only one pad, even though there are two physical ones.

[one-of-the-robs · Accepted solution]

Ah, right, I see.

I think there is a way you could do it. You will need to create a new device, with a symbol that has only one pin and a 1206 footprint. You would then "append" both pads to the same pin, using the "any" mode. Now populate as many of those as you need onto your schematic, all connected to GND.

I haven't tried this but I think Eagle will treat such a device as being able to satisfy the routing between parts of the net that connects to it.

[mark9XJEG]

Rob - I don't think that it works - as an example there are parts (the LM317 pops to mind) where there are two pads which are electrically connected together - in the case of the LM317, the main thermal pad and pin 4 (the middle of the three legs) are internally connected to the same node.   If you do not connect the two with a trace, Eagle flags this as an airwire.   Unless there is a trick that I am missing, I think that they need to fix something in Eagle which will recognize the ability for a part to have two pins, which are treated as one when looking at connectivity.

Mark

[one-of-the-robs]

---

@mark9XJEG wrote:

  If you do not connect the two with a trace, Eagle flags this as an airwire.   Unless there is a trick that I am missing,

---

That's why I very specifically mentioned setting the "ANY" option when appending connections. Pins with multiple pads can be defined as either "any" or "all". The latter case is the one that inserts airwires because you are declaring that all of these must be connected. This would definitely be the correct option for, say, the power and ground pins of a large CPU. However, if you set "any" then that means you only need to connect one of the pads but you can connect any number. I've certainly used that for switches with paired pins and built up a switch matrix on a single-sided board by using the switch itself as a jumper.

[mark9XJEG]

Rob - Still not working.

I have created a new 0 Ohm resistor component, with a single pin, and using the 1206 footprint, I connected both pads of the 1206 to the single pin on they symbol, using the 'ANY' condition (also tried ALL) - Still see the airwire, straight across the device.   I also verified that my Device for the LM317 has pins 3 and 4 (output) connected using the ANY, and if there is not a trace between the two pads, I see an airwire.

[one-of-the-robs]

Could you upload your library and design (zipped) for me to look at. I'm sure it should work and I've just checked with a bunch of four pin single pole switches. For me, Eagle produces the shortest set of airwires to fulfil the net, none of them across the device, and if I connect the net to a pin without an airwire then the airwire on the other pin of the pair disappears.

[mark9XJEG]

Rob - my apologies.   I updated my 0 ohm resistor to be a one pin component, with two pads, connected as ANY, but when I updated the library, it wasn't taking because I missed one of the 0 ohm resistors in my design which was a 2 pin component, so Eagle refused to update - once I got everything cleaned up, I am getting a clean DRC. 

[thomasjude]

Hi Mark,

I am facing the same issue in Aluminium PCB. In your post you mentioned 

"0 ohm resistor to be a one pin component, with two pads, connected as ANY"

What is this ANY mode? I am unable to locate this feature/mode