Altium Designer, change pin map of multiple components

[fernazza]

Hi all,

I'm new with Altium and I am in the following situation. I have a schematic and routed PCB board with more than 500 SMD LEDs. Footprint for LEDs is PLCC4. For the LED I'm currently using everything is fine. However now I want to use another LED brand and the pinout is the other way around. Therefore I would need to change pin map of each LED in schematic, then update PCB document and finally rotate each LED in PCB manually. All that is a lot of work so I wonder if there is a way to automate that process. Any thoughts are appreciated. Thanks in advance!!!

Fernando

[DutchGert]

Uhm, if it has the same number of pins just make a new part in the library, select all 500 leds en in the schematic inspector change the poart to the new part. Then update the pcb and you ar good to go.

On pcb level, just select all leds and in the pcb inspector give them a new rotation

[T3sl4co1l]

If you want to support both brands in the future, create a SchLib symbol for each, place them on the schematic and connect them in parallel.  Create two Assembly Variants, one with all "LED A" and the other with "LED B".  Update the PCB and place all the new "LED B" footprints over the "LED A" ones.  (Since AD15, this can also be done within a single symbol, by specifying a variant component from the library; multiple parts don't need to clutter up the schematic then.)

The result is that Pick-And-Place information will be outputted with the correct rotation for either variant.

If you don't need a compatible solution and just want to update them all, then go to Tools/Footprint Manager and edit the footprints for the correct pinout; update PCB, select all the LEDs and, in the Inspector, set Rotation to "Rotation+180".

Or just add a note to the assembler that the different LED parts are wired backwards. They may even figure it out on their own, because footprints have inconsistent position and angle references.

Tim