I’d like to have a schematic symbol that has an array of pins that do not physically map to a pad in the footprint, considering the footprint won’t really have any copper pads in it anyhow (just some User.Comments layer features which will help me place some 0.1" headers from another symbol/footprint). Suffice to say the reason is rational and reasonable to achieve in other packages.
So is there a way to have a symbol pin that doesn’t have a corresponding footprint pad? I don’t care about DRC flags. This is my absolute first KiCAD design, so still trying to learn how to work the way the tool works, vs making the tool work the way I work.
The mapping between symbol-pins <–> footprint-pads uses the pinnumbers (from the symbol) and the padnumbers (from the footprint). Same numbers are assigned together.
So if you have a footprint assigned to your symbol which has no pads at all - you will get warnings at the “update board from schematic”, but generally it will work.
On the other side: If you have no pads on the footprint, why do you have pins on the symbol?
For such auxiliary footprints I have defined a auxiliary symbol which also has no pins, but only graphics.
example picture is my helper-symbol for mounting-parts (it should symbolize a screw, I#m better with electronics than as an graphic artist).
Thanks. This is what I was expecting but was hoping there was a way to simply suppress the errors after “update board from schematic”.
The graphic approach is the one that I’m taking, but was hoping to avoid it, as it’s far more manual and time consuming. It seems to me that features in both symbol and footprint are generally more manual in KiCAD than I’m used to… copy paste between layers is a no go, primitives and parameters cannot be group edited, auto increment during copy/drag isn’t possible, etc. I’m getting used to it slowly though. Hopefully I’ll have time to learn the scripting / plugin capabilities soon to accelerate custom operations. Always a struggle to adopt different workflows. Seems worth the time though. Cheers.
just some additional hints for an easier learning curve:
copy paste between layers is a no go, primitives and parameters cannot be group edited, auto increment during copy/drag isn’t possible, etc.
symbol editor:
Edit–>pin table allows to modify multiple/all pins at once
modifying different graphic items is currently much manual work
but copy/pasting from other symbols works quite well
it might be a good idea to open a second symbol-editor (from a second kicad-instance) in parallel - so you could use one as a source for copying without permanently switching between a source-symbol and a destination symbol
with the “Insert”-key you can repeat the last operation step with automatic incrementation of numbers. Works also in schematic editor.
footprint editor:
check the Edit–>Edit Text und Graphics dialog → much options, can do many things on your graphics
if you have time: wait one year, the properties panel from the board-editor will sneak into the footprint-editor in next years kicad (v8).
if you want to unify pad-settings: look into the context-menu and use the five different pad-commands
Hopefully I’ll have time to learn the scripting / plugin capabilities soon to accelerate custom operations
Notice that python-scripting currently works only on the board-editor (and FP-editor??). For schematic/symbol-side there is a scripting feature planned, but severely delayed. No fixed release date is announced.
Always a struggle to adopt different workflows. Seems worth the time though.
I second both statements. I had these struggle 1 1/2 years ago (after 25years working with eagle).
@mf_ibfeew This feedback is gold. Thanks for putting these hints in one place. I’ve been looking in the various docs / forums / videos, but as with learning most new tools, I haven’t quite learned the most efficient ways to find the details I’m seeking (hence my first post on the forum). Still figuring out how to figure it out
The most efficient is to ask at forum. Looking through FAQs is also good.
In 2017 I decided to move from Protel 3 to KiCad (V4 those time). I found KiCad in some aspects better than Protel and in some aspects worse concluding that they are comparable. But now (V7) is certainly better.
I fell into the following pitfalls of KiCad:
to position text at schematic I changed grid - it is mistake as if you forgot to change it back you can get symbols positioned not in 50mils grid. Keep it set to 50 and never change. To position text use CTRL key why mowing it,
I placed power symbol (like VCC) and changed its name to V9. Then I was surprised that KiCad wanted me to connect them at PCB. In such case you need to define new symbol. In symbol not its name specifies net but the pin name (not visible at schematic). It is probably the residue of conception of digital ICs symbols with hidden power pins - two power pins so their names have to specify net and they are invisible.
I didn’t used plugins and don’t plan. May be because I don’t know in what they can really help.
