Good morning everyone, my question is simple, I want to understand if during the placement of the components on the PCB it is possible to swap between equivalent Pins and/or equivalent Slots.To make my request clearer I give an example:Suppose we have a 74hc32 component. This OR component has four Slots (A, B, C, D), When placing the component, I may need to optimize the paths of the tracks, to exchange slot A with C and B with D, in addition to avoid annoying intersections,you may decide to swap between the input PINs of the same slot… for example PIN 1 with 2, PIN 4 with 5 etc., but I might need to be able to also swap between Slots of ICs of the same type… For example, I have U1 and U2 both 74HC32 of which for optimization I would like slot A of U1 to become U2 slot B etc. I worked for many years in design with Spark SUN and Cadnetix equipment, and I had this possibility, but here I don’t understand how to use it.Thanks for any replies.
I’ve edited your title to reflect KiCad terminology where they are called Units. And it’s done in the schematic, then you can update the layout from that.
Somebody will show you how. It’s quite straightforward.
Pin and gate swapping is not directly supported in KiCad as far as I know. There is also a very old (opened in 2007) issue for this on gitlab:
Gate swapping is equivalent to unit swapping if the multi gate part is drawn as multi unit with a seperate power block.
Pin swapping is a feature that hasn’t happened yet, although with a two input gate, selecting the symbol and hitting “ÿ” to flip vertically, has the effect
The gates are designed separately, but I didn’t understand how to swap between them… You say it’s possible, but it can be done directly on the PCB, or I have to go in and do it manually on the schematic. Swapping the pins, as you say, can only be done if I enter Schematic, from what you write, I understand that it is not possible on the PCB to select the PINs you want to swap, with the simple press of a button. Right?
Just do it manually on the schematic. Say you have a unit A in one place and unit C in another place in the schematic. Edit the properties of each so that they are C and A. You can also change the reference the same way if you are changing to another IC. Just don’t end up with duplicates, but ERC will catch that error.
As davidsrsb said, swapping pins can often be done by mirroring the symbol. If it’s more complicated than that, you have to reroute some of the wires.
Then update the layout and the ratsnest lines will change. If you already laid out the tracks, too bad, you have to layout the tracks again.
Sorry I don’t know of any way to do this on the layout. Or a shorter way to do it in the schematic. But I don’t do this often enough that it takes much time.
Correct.
This must be done with the schematic. After the changes are made in the schematic use Tools “Update PCB from Schematic”.
Using 74HC00 as an example:
- To change input pins on one gate: hover mouse over the symbol and press hotkey Y (or hotkey X if gate is displayed vertically).
- To change gates in the one package: Right Mouse Button Select Menu > Symbol Unit (Top of list) > Choose Gate from new list.
- To change gates from different packages: Use M hotkey.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.