Hi guys, just a quick question. Should the U key highlight also the THT pads ? It works with vias, but not with THT pads. Is there any way how to chek, that the pad is correctly connected to the track(s) ?
Apparently not.
However the functionality you want is the Highlight Net action usually assigned to the ` (backtick) key but this is problematic for some keyboard maps so you may wish to assign another hotkey to it.
U key expand connection. I use it for example when I want to delete whole connection. So vias of course should be also deleted. If pads would be also selected you will have doubts if you can safely press Del key.
1 Like
This is how it looks when I use the Highlight Net from the right click menu on the track. So in this case it looks like the pads are part of the Net. I was bit confused because it is also highlight when there are no tracks and you jsut click the pad to create the track. Anyway I will try to find where to set hotkeys because I mostl yuse CZ keyboard.
Why I was asking. I am working on re-enginnering of a project and when I imported the projects from gerbers (except F.Cu/B.Cu) all the THT pads were imported with vias inside the THT hole.and when I re-make the traks it always connected to the vias. You can see some on the picture.
I don’t know how it happened that the vias were imported inside each THT hole pad. If it was in the orginal project or it was caused by the import… Anyway I asume it doeasn’t make any sense to have the vias there. There is alredy Cu inside the THT pad connected both sides.
I hope I am not wrong.
Yes, it makes sanse with the DEL key.
I have one more question partially related to this topic. I am encountering several errors that state: “Error: Missing connection between items.”
However, the signal does pass through a resistor, but the thin line of the net suggests that the signal should go directly to the next pad or continue along the next trace. When I perform a U check, all the traces seem to connect properly, but the pads are not highlighted. On the other hand, when I use the highlight net function, everything is highlighted as if it were properly connected.
A similar error is occurring with a MOSFET, as shown in the attached images.
Generally this means you have not finished the track routing. For the PCB DRC you should turn on the option Test for parity between PCB and schematic. If you get errors then your PCB doesn’t match the schematic. Remember highlight net indicates which copper is on the same net according to the netlist, and doesn’t imply you have connected them.
It could also be a schematic error. If those Qs are transistors, then you are connecting (I think) the collector and base together, according to the netlist.
1 Like
It is strange for me everything looks OK. When I am updating the PCB I have the following settings (sorry translated from CZ):
YES - Reconnecting footprints to schematic symbols based on their references
NO - Delete footprints without symbols
YES - Replace footprints with those specified in the schematic
If you check my Q6 MOSFET on the schmatic and PCB everything seems to be correct:
Look at each of the bottom 2 MOSFETS, the labels C1 and C2 are each connected to two of the terminals of the MOSFETs. Can this be right? That would be why KiCad thinks you haven’t made those connections yet.
Remember, when you put down a label, it’s like connecting wires to all of the occurences of that label on the schematic. Labels aren’t just for show. If you want descriptive text, then that’s a different tool.
Thank you very much for your help and patience.
Aha, I think I partially get it. The labels are done when connecting the wires to the BUS. SO, you mean if I label the MOSFET GATE connection like C1-IO (connected to the PIC) and the MOSFET DRAIN to C1-R (connected to relay) it should be OK ?
Another thing is with e.g. resistors (see the picures of another part of the project).
I encountered an issue with the FWD and RVS signals when importing the schematic into the PCB editor. KiCad created multiple nets which, when connected in the PCB editor, flagged shorts between the nets. The only solution that worked was adding labels and marking the individual connections with the labels FWD and RVS. Without this, every update resulted in the creation of separate nets like FWD, RVS, D1-A, D1-K, D2-A, and D2-K, etc.
Adding the labels resolved the issue because, in reality, these are just two signals—RVS and FWD—coming from the tandem match and going through diodes, resistors, etc., all the way to the pins of the PIC1938.
If I remove the labels, multiple nets are created again, and I’m not sure how to resolve this.
I think you wanted to label the flow of the signal. But labels are the other connection method to wires, so if you put a label down it is equivalent to connecting together all the places that have the same label. So don’t use labels to document the signal flow, use graphical text if you want to do that. Please understand this documentation on the two ways to make connections or your circuits will not work.
A net is not all the places that have a particular signal. It is the set of places that are directly connected.
Some people go to the other extreme and their schematics have very few wires, labels connect everything. This style makes the schematic hard to read in my opinion.
1 Like
It is standard that one resistor end has separate net than the other end, and you seem to be not liking it.
Both pins of your R3 has the same net (FWD) so you want them being connected = resistor being shorted. The same way you want D1 being shorted and may be other pins and it is why you have connection lines at PCB.
I also noted that you seem to place a lot of importance on the net names on pads, and it seems you are adding labels to make them show what you want. But in truth, many nets don’t need to be explicitly named. Here’s a section of a layout of mine.
KiCad has automatically assigned names to many of the nets, which are of no consequence to me. By placing undue importance on these net names on pads, you are counterproductively wrecking your circuit.
Guys, thank you for you help. I really appreciate it. I think I somehow get what you mean but need to think a bit about it.
But "shortly."when a signal goes through a component like the MOSFET or resistor It must not have the same label on pin 1 and 2 otherwise it is short contact.
I will make a backup and try to test it without the labels on the RVS/FWD nets.and find where I got the error with shorting two different nets.
There is an issue that it is re-engineering and lot of staff was imported from gerbers so it is not as eeasy as first KiCad project.
I will come back. Thanks again.
1 Like
Blimey 
your not kidding, this is an awful first project, I would ‘hit the books’ if I were you. Starting from Gerbers is scary and not a proper workflow in any sense of the word 
may I suggest a nice project next time that starts with a schematic 
Any how I wish you the very best of luck 
If all your connections are by wire, remove all the labels.
Dear Piotr and retiredfeline Thank you for your advice and assistance. Thanks to your help, I managed to resolve all the connection issues, and now I understand how it works. It looks like I’ll soon have this project fully converted into KiCad based on the original schematic and PCB from the Gerber files, and I can finally start working on modifying it. Thank you very much!
BTW, you don’t need to find our profile pages to make links. Just precede the username with @, e.g. @t.konecny. I have notifications turned off (who has all that time to be pinged anyway) but it will make a link in your post.
1 Like