I created a multi-unit capacitor, like the old “can” capacitors with multiple internal caps. I found that the individual units cannot have dissimilar values.
In other words, when the part is placed in a schematic, a value change to one unit is applied to all units, even though in the Symbol Properties “All units are interchangeable” is unchecked.
Is this not supported in KiCad? If there is a way to make this work, please educate me. I haven’t found any help in the manual on this detail.
As a work-around, I placed 3 individual caps in the schematic with reference designator like C1A, C1B, C1C.
I’m on V8, can’t comment on V9.
AFAIK it’s not possible. The “Value” field refers to the whole part. This is unproblematic with eg, ICs, but in your special case it won’t work.
The C1A…C1C solution is not good. IMO, best would be to place three discrete caps and draw a square/circle/whatever around them to show a group/assembly.
In KiCad, the RefDes must always end in a number, If it does not, then KiCad adds a number during annotation. This happens always, (except of course for the symbols which have real suffixes “A”, “B”, etc. So after annotation, your capacitor will likely be “C1A1” and “C1B1”.
I’m also struggling with multi-part symbols. A few days ago, I experimented a bit with Relay_THT:Relay_DPDT_FRT5 and when I move a pin of one of the switches, the pin of the coil also moves around in the symbol. I’m not sure what’s going on there.
It can create potential problems for ERC, netlist generation, BOM generation, PCB layout, simulation etc. KiCAD is somewhat strict about reference designators (which is good!)
But if you just want to draw a schematic for documentation, go ahead.
I myself used KiCAD for drawing the layout of our garage basement with 40 parking slots.
Perhaps this is a clue: I discovered that symbol changes in one unit were occurring in another unit. Careful examination revealed that the primitive shapes had “Common to all units in symbol” checked. When I unchecked that option, I was able to create unique symbols for each unit.
…the bad news is that I had to redo the whole device. I considered it as the cost of education
Treat the Symbols as three separate capacitors. (Note the Pin Numbers).
Create a single footprint with all the required pins in the correct position along with Silk, Courtyard and Fab layers (centre bottom) PCB image.
“Save as” the created footprint twice to finally have three identical footprints.
Delete pads 2 & 3 from A footprint.
Delete pads 1 & 3 and silk etc. from B footprint.
Delete pads 1 & 2 and silk etc. from C footprint. See top 3 examples in the PCB image.
Move B & C onto A using the anchors and maybe turn them into a group to ease pushing around the PCB.
Tracks and Ratlines work. but I didn’t try DRC.
Since it’s for documentation purposes using graphics to indicate a common can should do. A custom symbol just slows down comprehension if someone wants to recreate the circuit and singles would be used as replacements now.
