A while back I used KiCAD V5 to build a whole bunch of PCBs. Then the pandemic happened; we know all about that. Anyway, I now have a new PC, I installed KiCAD V6 and set about building a new PCB. I was just about to send it for fabrication when I noticed: none of the ICs are connected to power!
In V5, this just happened automatically. But in V6 it seems I’m missing some setting somewhere (or I’ve just forgotten how the software works), because I can’t for the life of me figure out how to force the power pins to auto-connect. What am I doing wrong?
Pins will auto-connect to planes of the same net.
So, if you have power and ground as inner planes on a 4-layer board, then any through-hole pad on those nets will get connected when you re-fill the plane.
I’m not sure but suppose that you are speaking about automatically connected at schematic VCC and GND pins of ICs. That depends on how symbol is defined. I think using symbols with hidden (automatically connected) power pins was popular in 80s but it is rather not used now.
Indeed.
It made sense when PCB’s had hundredths of TTL IC’s combined with old limited PCB design software on small monitors, but the practice is obsolete.
In modern designs, the number of IC’s is quite limited, and multiple power supply voltages and different power domains are all to common.
Previously KiCAD would just connect pin 14 to VCC and pin 7 to GND automatically, provided I set up the right power flags. Now these seem to not be connected at all.
(I’m also confused as to why this doesn’t raise any errors. Surely having all these pins unconnected should be an error, no?)
Have I somehow mis-remembered how power flags are meant to work? Or is there some setting somewhere I need to set to make these auto-connect?
Some time ago the “old fashioned” 74xx symbols (with hidden power pins) where replaced with new symbols with a explicit added power-unit. This unit must be manually placed in the schematic and than manually connected to 3V/5V/GND (whatever).
If you attach the project (Kicad-manager–>File–>Archive project) we can look an tell if the autoconnect doesn’t works (bug, unlikely) or if you just used a symbol without hidden power pins.
remark: for attaching a archived project you need to promote yourself to the “basic user” level. Read level for information.
I do seem to recall while drawing the schematic, every 4th gate I tried to draw, it gave me a power block symbol instead of a gate. So I guess that means I’m using the “new” gate symbols then.
I’m a little surprised that taking away a feature is considered an “improvement”. What’s the rationale for this? Like if you have more than one voltage level or something?
So what are my options at this point?
Manually place a power symbol and wire to the power rails for all 85 ICs.
Downgrade back to KiCAD V5.
Write a Python script to modify the netlist file before feeding it into the PCB editor.
Auto-connecting power and ground is a really bad idea, and always has been. As you note, there can be multiple supply voltages. I have boards with 12v, 5v, 3.3v, and 1.8v - what is the correct power? And, more subtly - what about multiple grounds? I often use DC-DC converters which isolate input power and ground. How is the software supposed to know which ground to connect to - ground or isolated_ground?
I’m a little surprised that taking away a feature is considered an “improvement”. What’s the rationale for this?
The feature is (until now) not taken away.
But for this feature the symbols (in the symbol library) mustbe drawn to use this feature.
As this created always problems and confusion the decision for the standard libraries was to switch from integrated hidden power pins to a extra dedicated unit which shows the power pin.
For your own symbols/symbol-libraries you are free to define symbols which use integrated hidden power pins. But you should read first the manual - so you understand what you do: Schematic Editor | 7.0 | English | Documentation | KiCad, section “hidden power pins”
A short list of some of the reasons for the library-switch:
it’s hard to work with multiple voltage-levels on the same schematic. Nowadays it’s not seldom that you work with 1,8V…3,3V…5V and sometimes 12V (gate drivers) as supply voltages on the same schematic
creating isolated parts of circuit is hard (all hidden power pins refer to the same “GND”)
it was a “hidden” feature , which resulted in many errors and problems for users, creating unwanted connections. The number of such questions on the forum has decreased → so the switch was the correct decision.
options for you:
use the standard symbols and place power-unit for every of these standard symbols and connect to Vcc/Gnd. You could use copy-paste to reduce the amount of work.
make your own version of the symbols in your personal symbol-library. Keep the same pinnnames/pinnumbers. Draw your own symbols with the hidden power pins. Than replace the existing with your own symbols.
You can take the V5 library. When opened in V7 it should be updated to current file format but symbol definitions will be as in those library so with hidden power pins. Hidden power pins work in V7 as they are still used in power symbols.
Ahhh the cursed symbols … First time I have come across someone that liked this.
The problem with said symbol is they assumed a PSU naming structure … Gnd and 5V and thus there was no way to use on a different gnd or a different rail and because it was a symbol level there was no way to (easily ) gain access to the implied power rail net to align to your needs
Best case, a bunch of TTL IC’s had their power connected to each other BUT not to an actual power source. Worst-case you now provide a “short” across a 1000V isolation barrier as you were using such a chip on an isolated area and named the main area +5V
I guess I’m so focused on my own project that it never occurred to me that somebody might be building a PCB that isn’t digital logic. I can see how if, say, you were building a power supply or something, there could be a dozen voltages on that.
In the interests of actually getting the board sent for fabrication, it seems just manually drawing all 85 power symbols is probably the fastest route to success. Does KiCAD have any way to quickly insert N copies of a component? Mind you, I don’t suppose 85 power symbols will fit on one sheet. Maybe I can fill up one sheet and then duplicate the whole sheet a few times…
And put in the decoupling capacitors next to the power symbols to make it clear which capacitor belongs where. The hidden power pins often led to forgetting to add the capacitors
