A dual purpose footprint - Page 1
Forum section: electronics / projects

author: matt6ft9
author_rank: Contributor
timestamp: June 12, 2015, 02:37:58 pm
content: In one particular PCB layout, there is a location that can have either a resistor or a diode stuffed depending on the board configuration. How should this be shown in a schematic? (two possible components, but on only one footprint)I’m using P-cad 2004 (which does link schematic symbols and PCB footprints), but also interested in how other EDA software might handle this.Matt

author: suicidaleggroll
author_rank: Super Contributor
timestamp: June 12, 2015, 02:52:46 pm
content: Quote from: matt6ft9 on June 12, 2015, 02:37:58 pmMake a custom schematic symbol that has a box with 2 pins, and inside the box it shows a resistor and diode in parallel with some kind of label next to each of them (A and B). At least that's how I would probably do it, depending on the circuit.

author: matt6ft9
author_rank: Contributor
timestamp: June 12, 2015, 03:18:41 pm
content: Hmm. Makes sense. What about the silkscreen graphic? Probably a good idea to show the diode cathode mark.

author: suicidaleggroll
author_rank: Super Contributor
timestamp: June 12, 2015, 05:00:32 pm
content: You'd make a custom footprint that has whatever silkscreen information you want on it.

author: daedalus
author_rank: Regular Contributor
timestamp: June 13, 2015, 03:52:50 am
content: do you really need to save the space of a 0603/0402? if not just put both footprints in, and mark one as DNP depending on the variant. Actually I might even suggest stuffing both on the board, then using a jumper to select. Variants drive up your production costs, and being able to turn stock from type A to B is handy if you get your demand wrong.

author: slateraptor
author_rank: Frequent Contributor
timestamp: June 13, 2015, 06:57:47 am
content: Quote from: matt6ft9 on June 12, 2015, 02:37:58 pmIt really depends on your documentation standards.If you play by ASME Y14.100 rules, one possible way is to make up a non-standard reference designator (like DR), then define what DR means in your notes section on sheet 1. Then create a generic placeholderfootprintschematic symbol (like a euro-style resistor symbol with dash outline and numbered leads); place a note marker wherever this symbol is used in the schematic. Place a note on sheet 1 identifyingappropriatesubstitute component symbol (drawn out individually, with labeled leads for diode) with its associated configuration. This will allow you to map 1 symbol to 1 generic footprint without ambiguity.For the footprint silkscreen, I would create a generic dash outline with a bar on one end denoting cathode to account for diode configuration. Next to the assembly P/N identifier xxxxxx-, the "" part would be a blank placeholder box with soldermask removed to allow for manual labeling of configuration with permanent marker during assembly.In your component installation drawing, assembly drawing and parts list, you'll also have to account for configuration variants by placing a note on the applicable find number(s). I would also poka-yoke that shit and place a note in component installation drawing which instructs to verify that diode cathode is aligned to silkscreen bar end.In Altium Designer,component type features are built into handle different scenarios like:1) common schematic symbol, different pcb footprint-- e.g. capacitor in radial, axial, surface mount packages2) common pcb footprint, different schematic symbol-- e.g. zigzag-style resistor vs. euro-style resistor or NAND gate vs. BOR gate (modes)-- e.g. 7400 series combinatorial logic handled as individual gate symbols (parts) vs. a single symbolic entity representing the chip3) non-standard components-- e.g. graphical symbol included for clarity but isn't linked to a net or pcb entity