I’m trying to have the schematic talk to the PCB and I’m not getting them to get along very well (see enclosed pics). Pin 11 of the IC should connect with the other leg of C7 than pin 10, and yet C7 reports the net of that leg as “unconnected.” What’s going on here?
Thank you for your help.
The little green square implies that the pin 11 is not connected
And yet, it is. The schematic clearly connects it to pin 1 of C7.
Oh, I think I know what you mean. I have connected it, but the same issue applies, schematic and PCB don’t want to talk to each other.
Is version 8 really this buggy?! I worked many PCBs in v5 (which I was told was very “buggy…”) and I feel it was a dream of smooth sailing compared to this.
Did you do an update (F8) after editing the schematic? It’s not automatic. And did the sync go through error-free? According to your first screenshot that leg of C7 is already connected to something else, J3-Pin2, according to the pad annotation, wihch I guess is in part of the schematic you didn’t show.
I thought you meant in the middle of the tracks which is normal behaviour but there are no examples of this in the screenshots anyway then I realised you meant to write schematic wires.
OP subsequently fixed your second point but I suspect they didn’t do a F8.
No more green squares, but an incorrectly drawn symbol
Note: Pin 1 & 8 are not connected to wires, so the pin has a circle and the wire has a square
Pins 2 & 7 are correctly connected so no circles and squares.
Pin 3 and pin 9 are both attached to the rectangle incorrectly. They both need to be rotated 180 degrees.
This is why both your pin name is outside the symbol and your wire covers the entire pin.
You have apparently already learned the red circle (open pin) and green square (open wire end) thing.
But there is a problem here with your symbol. The red circles (attachment points) are supposed to be on the outside of the pins. To fix it properly, open the symbol in the symbol editor, and change the Left / Right properties of those pins (Can also be Up / Down)
This is not a “signal name” (label) but they are the pin names and this is actually normal behavior. The problem here is that the pin itself is mirrored (Left / Right), and as a result the pin name is outside of the symbol instead of inside it.
(Yes, KiCad uses a confusing “Left / Right / Up / Down” naming of the pin orientation. If a pin is on the right side of an IC, you have to set the pin orientation to “Left”).
You write you are having problems with the transition from KiCad V5 to V8, but most of your problems you mention would be the same either in V5 or in V8. I guess you have learned some bad habits in V5 (I am guessing probably self study with little input from external sources) and these bad habits are being pointed out, now you are communicating with others over this forum. However, the GUI has also changed quite a bit between V5 and V8, and this will also take some time to get used to. For example, in KiCad V6 all icons were re-designed. ERC and DRC have been extended, and they flag more issues (and also some false positives). DRC now complains about a lot of things that went undetected in KiCad V5.
Thank you all very much.
Indeed, v5 to v8 is a bit of a jump, and not in the most obvious ways. And definitely, a lot of v5 was figured out “trial and error.” In a large part, I’m trying to do it differently this time, requesting help here, so that I’d learn this in a way closer to how it’s intended.
The symbol is indeed a custom IC symbol. 'll have to take a second look at it with your feedback in mind. Hopefully, it won’t be difficult to revise.
On updating from schematic to PCB - in my environment, it seems trying to “push” the schematic into the PCB doesn’t work, but if I save the schematic, and then try to “pull” it from the PCB Editor, that works OK.
It’s entirely possible I’m using the wrong command to do it, I’ll take a closer look.
Make sure you are starting every component of KiCad from the project manager. If any of the components are running standalone the sync will not work.
The normal method is: … / Tools / Update PCB from Schematic [F8] and it does (should?) not matter whether you stat this from the PCB or Schematic editor.
But you do have to be careful with the checkboxes.
The Re-link footprints to schematic symbols based on their reference designators should normally be off. It is only used when the normal connection between the schematic and PCB (by using invisible UUID’s) is broken. The other two checkboxes can be set according to your wishes.
And indeed, as retiredfeline mentions. This updating does not work when KiCad is in “standalone” mode.
“Does not work” is not a helpful description. Always add error messages you get to your post. They are needed to find out why something does not work. And without knowing the why a problem can not be diagnosed / fixed.
When I attempt to update the PCB from the schematic from the schematic editor in standalone mode, I get this message:
paulvdh - there was no error whatsoever. The PCB would simply not update. I’d never post a potential bug (or apparent dysfunctionality) without attaching all the pertinent information (to the best of my judgement), and an error message would have been an obvious must.
It’s entirely possible my workflow was incorrect.
Fix errors and misconceptions as you progress. Like the symbol pins. Cleaning off the dust will make it easier to see the error you are looking for later.
Yes, I’ve been doing that, I just don’t post back here on that progress.
As much as I can help it, none of the input on here is wasted on me and others that run into similar issues and may read these threads.
