I have a schematics where I have two DC/DC converters. One is the TEL5-1222 and the other is TEL8-1222, both from TracoPower.
Reason: it must be possible to interchange between the two devices, depending on the availability. So, both schematics as well as PCB must have them in.
Question: what’s the preferred way to handle this?
For the moment, I’ve drawn both DC/DC converters in my schematics so that I have them also both on my PCB when running the netlist and PCB footprint assignment.
Only drawback: they both have a +12V and a -12V output and I’ve connected them to the same net since on the PCB the corresponding holes must be connected to each other although of course only one of them will be stuffed in the end.
However, the ERC doesn’t like this since I’m connecting (short-circuiting) two power outputs (+12V and -12V) to one another. ERC does a fine job, however, since ERC doesn’t know only one of them will be stuffed finally.
Well ERC basically tells you: “I think there is something wrong. Could you take a look?”
Your brain is more powerful than what ERC and you have more information in this case. So this means you can decide “This message is a false positive, move on” (I think in future we will have a way to explicitly mark messages as “ignore” but that will also take a while)
Another option would be to place a net tie or even solder jumpers. The latter could be beneficial if the two converters are far apart and you don’t want to drive the unused part of the traces (would allow you to tailor the output and input filters to the converter in question and have it very near to the converter).
1). Disable ERC checking by hovering over one of the schematic symbols and press [Ctrl +e] to edit one of the DC/DC converters in the symbol editor, edit the offending pin properties by setting them to “passive”. (Edit: quite ugly hack).
2). Draw only one DC/DC converter in the schematic, and make your own footprint for the PCB on which both DC/DC converters fit.
If there is a “preferred” way, that should depend on the work flow of your company, and not on the opinion of some random guy on the Internet… Each way of doing it has it’s own characteristics. As long as you put both DC/DC regulators on the schematic (and don’t mark them with #) they will both show up on the BOM, and you may risk ordering both of them.
A short term hack that will bite you later. Just imagine you later reuse that part of the schematic in some later project. I am sure you will by then have forgotten that you have a special symbol for the dc/dc converter.
Really i would live with the ERC warning before i do such a dirty hack.