I am using a multi-unit component in my design (74LS139 if it makes any difference). Normally you would place a A,B, and C units on a single schematic page, and all would be good. However I am using a complex hierarchy of schematic pages, with one sheet repeated 4 times. On each of the 4 sheets I need one half of the 74HC139, this would be 2 chips in total.
Unfortunately when I place the 74LS139 I have to select either the A unit or the B Unit. And when I annotate the overall schematic I end up with 4 chips rather than 2 chips. Is there a way to wildcard the selection of the A or B unit and have the annotation minimize the number of chips?
The same problem would occur if you needed a single NAND gate (74LS00) on each page, only worse since you would end up with 4 chips instead of 1.
Hmm, I have no problem editing the subsheets to use only part of a component. For example in one design, I have a compound component on a subsheet that uses one NOR gate of a 74LS02. So one chip is spread across 4 subsheets. As to whether this can be done automatically without manual intervention, I don’t know.
Actually thinking about it further, I don’t see how KiCad could wildcard units in new or copied instances of subsheets. You might think, ok when you copy the subsheet, use another unit that hasn’t been used yet. It would have to be the same type to present the same symbol. But which unit? KiCad knows that 74LS00 has 5 units, 4 NAND gates and the power unit, but it doesn’t know that A-D are identical but E is different. All it knows is A-E are not all the same.
So I think manual editing is inevitable with the current data that KiCad has on the components.
I went into each sheet and manually selected the B Unit on all the even pages and changed the U number to match the odd pages. running the checker it didn’t like the fact that I had two C sections for each chip, so I had to move the C sections to another page. Not the easiest way to do this, but in the end I have what I need on the BOM and netlist.
I suspect that KiCAD would need extra info in the symbol to be able to automate this. first, what sections (if any) are identical and swappable (A nd B in this case), and second what sections are common and can have multiple instances (section C in this case) as long as all of the pins in the multiple instances, are connected to the same nets (power and ground in this case).
Manual annotation is needed even if all components are on the same sheet. At least from my experience I don’t want the program to choose the the arrangement of the units.
What I don’t understand is why do you need two instances of the C unit of the same chip.
I’m guessing that the C unit is the power pins. If that is placed on a subpage which is used twice (one with A and one with B unit), this will cause issues… This is a bit unfortunate but I don’t se any other way then to place C on another page which is only used once.
Unit C must be placed only once for each chip no matter how many sheets are used.
A symbol is a representation of a component with a one to one match of symbol and component pins. Your unit C has two pins, 7 and 14. Duplicating these two pins in the schematic has no sense.
What I was ‘trying’ to do is build a module that I can use over in other schematics, hence the reason unit C (the power pins) was on the sheet. I never know if I will need 1, 2, or many instances of the module. If the power section could be repeated, and the auto numbering would select different identical sections, then I could just drop down as many modules are needed with no thinking. As it is I have to hand edit the sections in the module. This isn’t a huge problem when there are only 2 or 4 modules, but could become a much larger problem in a larger system.
At least one CAD system I have used in the past could deal with this, it is not an insoluble problem, but pretty low priority.
It’s only a problem in KiCad if a chip is split across modules. I have a subsheet that uses both logic units of an IC so the power unit can go on the subsheet too.