LM339, no Vcc Pins

Schematic Library Symbols
1

I’m close to the finish line on my first KiCad project, but this is one of two things in the way of that goal:

When I added LM339 to the schematic, no Vcc pins appeared. Naturally, the router is complaining of this missing data:

Warning: No net found for component U1 pad 12 (no pin 12 in symbol).
Warning: No net found for component U1 pad 3 (no pin 3 in symbol).

image

I’ve clicked on the LM339, hit “E” and gone to the Pins tab to verify that there IS a Vcc + and - node for the IC. However, I do not know why it isn’t showing up on the schematic. I went hunting through preferences to see if perhaps there was a global option to unhide Vcc pins, but found nothing specific to that.
Surely others have run across this issue and perhaps have a solution they could share?

2

The concept you need to read up is units:

https://docs.kicad.org/9.0/en/eeschema/eeschema.html#symbol-units-and-body-styles

Note that unit E is designed to fit over one of the op amps / comparators, if you wish.

3

You will find that there are 5 parts to the symbol. Check for part E.

Edit: The “not so young” cat beat me. :frowning_face:

4

Or spawn off your own opamp symbol and add the power pins to one of the ‘Units’. I don’t really like the notion of (5) units for a ‘quad’ device:

quad
quad380×510 23.1 KB

PinTable
PinTable1291×824 41.4 KB

1 Like
5

So something like this… I’ve added power flags for the 90V rails. Added part E over the top of one of the other parts:

image
image394×973 9.92 KB

6

Your method seems more elegant, and I agree about the number of devices. Is this a process for the symbol editor? I assume I can take a standard part, use as template and save as new library item?

7

It’s a good idea to get acquainted with the KLC:

1 Like
8

Yes. Kicad makes it easy to copy a symbol from wherever and paste it into your own libray(s). Once you have the victim in your own basement, you can massage it or molest it to your liking.

1 Like
9

Modifying KiCad’s symbols for the sole reason that DaveL does not like a 5th unit in a quad opamp seems a bit silly to me. A separate unit for the power connection has been common in nearly all PCB design program ever since the '80-ies. Not only for Opamps and such, but also for TTL IC’s. If you wish so, you can of course change those symbols, but I would just leave them as they are.

2 Likes
10

Fortunately I’m too lazy to spend time on this ilk of cavil. :grinning:

11

Actually, I do it the way I do it because I’ve used PCB design programs since the '80s. OrCad Capture specifically. I place all my symbols from my own libraries. I appreciate that KiCad has plethora of symbols and footprints, I use them as springboard and change what I don’t like. The symbol editor is intended to edit symbols, Eh?

One of the nice things about Kicad is there’s often more than one way to skin a cat and more that one road to Rome. You can do what works for you and I can do what works for me. It’s not like it’s Apple that tries to dictate one way. More like Linux.

I made an alternate suggestion, and the OP seemed to agreed with it. The end result to the PCB netlist is identical either road he takes.

1 Like
12

I like the idea of separate units for the power. That way I can choose to which other symbol it can be attached for aesthetics of the schematic, or placed out of the way if the schematic is very busy.

5 Likes
13

With a separate power unit, it is easier to show associated decoupling capacitors. The schematic around an opamp amplifier symbol can get crowded.

2 Likes
14

For this reason I always modify the single op amps so that they have two units, one for the amp itself and one for the power pins, which I like to have grouped together with all the power pins of all the other devices. If that was made so for the default libraries, I would be delighted!

15

Thanks for all the input on pros and cons of separate Vcc units.
I think the separate Vcc unit gets the approval from me.
I was able to place Part E right over the op amp, so the schematic looks traditional in the manner I have drawn them 50 years ago.

image
image243×948 6.33 KB

The whole PCB has come along nicely. I got creative, adapting the PCB to a plug in relay I have already bought.

image
image1190×1014 234 KB

Board checks look good, except for some overlapping silkscreens. No electrical problems flagged.

1 Like
16

I try to partition my designs and make extensive use of a hierachical subsheet for power.
This normally contains the power supply plus decoupling caps, with a note at each cap as to which IC it belongs to.
On the main sheet and the subsheets, the “E” units are just tucked away in a corner somewhere.

This thread gave me the idea of placing the “E” units in the “power” subsheet, and it works a dream. The “E” units now have their decoupling caps directly connected, And it removes the remaining “power clutter” from the other sheets (except for the complex devices).

I think I’ll go this way in the future.

Cheers.

2 Likes
17

You should find that this is the case for all symbols drawn with a separate power Unit (part).

1 Like
18

Sure about that? Try one of the 7400 multi gate ICs with a solid fill power unit. Tsk, you guys calling them parts.

I mentioned this deliberate design detail way back in the second post. I’m just amused by the thought that some KiCad veteran dev is chuckling over the things we young uns rediscover.

19

I called them parts to avoid confusion for our new member.
That’s my excuse and I’m sticking with it. However, I have edited my above post to avoid the expected avalanche of complaints when those North Americans and Europeans awake.

Hence the use of the word “should” and not “would”. :stuck_out_tongue_closed_eyes:

20

For my future reference, I would like to know the process for creating a subsheet. This idea of putting all the power/decoupling there is a good decluttering idea for densely populated digital logic circuits.