I am new to KiCad. I have a small schematic (a voltage boost converter) and have begun my pcb. So far so good. But the netnames are all baloney and I would like to change some of them to meaningful netnames which will get to the pcb. I cannot figure out how to do that. I see the button on the right “place netname local label” but aside from putting a label on the schematic this does not seem to do anything. As an experiment I just now placed two different labels on the same net. I have seen some instructions on how to do this but I do not fully understand those. Can someone please advise? Thanks.
I am using a version:
Application: kicad
Version: (after 2015-may-25 BZR unknown)-product release build
wxWidgets: Version 3.0.2 (debug,wchar_t,compiler with C++ ABI 1002,GCC 4.9.2,wx containers,compatible with 2.8)
Platform: Windows 7 (build 7601, Service Pack 1), 64-bit edition, 64 bit, Little endian, wxMSW
Boost version: 1.57.0
USE_WX_GRAPHICS_CONTEXT=OFF
USE_WX_OVERLAY=OFF
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_WXPYTHON=ON
USE_FP_LIB_TABLE=HARD_CODED_ON
BUILD_GITHUB_PLUGIN=ON
I am guessing that you are meaning to do it from with in the schematic editor not after. There is a button on the right side just below Junction button. It is called “Place net name - local label”.
As you can see in my post, I have tried that. That only seems to place a label on the schematic. Very useless. I can even place two different labels on the same net. It does not get through to the pcb.
All the same I am looking at a schematic and layout that I just did where that did work. Here is a small screen shot to show that I am not BSing. I wish I could show you the hole thing, but I think my boss would have a problem with that.
Could it be something as simple as just how the you place the label? Sorry, I hate to break this down to that low level.
The 2 different labels sounds like KICAD does not check for this. I have not really had a need to even try this. This does seem like checking for this is a bug/feature that should addressed.
My hunch is that my labels are just labels in “space” and for some reason are not being associated with the net. I can use the same tool (place net name - local label) to place local labels in a white area away from “wires” or components and I get the same result. It seems like I am just placing dumb text on the schematic. I wonder whether I should try loading a newer version of the software?
Thanks to anyone who can shed some light on this as I do not know how this particular button is supposed to work…
After placing the label you have to generate a new netlist in eeschema and read the netlist in pcbnew. I have forgot this more than once…
If that doesn’t work, you can open the project’s netlist file (.net) with a text editor (e.g. gedit) and check that the correct label is there. Towards the end of the file you see multiple entries that look like:
…I think you also need to place the netname ON the “wire”. The text has a small black square which I guess needs to be placed on the net to name it. How would KiCAD otherwise know which of the netnames should be associated to just this net?
You could also use global netnames if nothing else is working.
And I guess Andrew’s tip with exporting the net-list and re-importing it into pcbnew is a good one as well
It seems that when learning different software, there is huge variation in the basic functionality of identifying clicking dragging etc. Airic’s comment mostly nailed it. I was clicking the local net label button then clicking on the wire and assuming that would associate the label with the wire. But in fact it seems to be necessary to drag the small square to the wire and place it there. Without carefully placing the small black square on the wire, it seems that the schematic capture portion of the software will happily allow the label to float. I saw nothing in the documentation to describe how this should be done. Anyway NOW I can re-save the schematic netlist and re-load it in pcbnew and it seems to work properly.
I can still seem to put two netnames on the same wire and it seems strange that the software allows this. But this is my experiment and is not a problem as I should be able to limit myself to one label per net.
Glad to hear there was some resolution with this problem. It can definitely be confusing at first.
As for the multiple names on the same net…the software really doesn’t care as long as it has one unique name. This is up to the user to ensure there aren’t multiple nets converging, but it can throw you through loops when trying to work out which net is which when you get to layout. If you have a dual screen (or split screen) setup, you can always click on a net in layout and it will highlight that net in the schematic (and vice versa). This can help troubleshooting. However, my rule is to use net names sparingly and only explicitly label important nets.
Hopefully this is deemed close enough to be the same topic.
I am looking for some clue regarding the forward slash “/” which seems to get placed as a leading character on any of those netnames which I have assigned. It does not appear on the schematic where I put it, but it does appear in the netlist. And when I go to connect stitched vias in PCBNew, I need to include that slash in order for PCBNew to recognize the name. So this seems to be a little bit of inconsistency. Am I missing something? Perhaps some way to pull up the list of available netnames when I go to assign the via connectivity (rather than needing to type it)? I do not see that option…
And it seems that even a capitalization mismatch will cause PCBNew to not recognize the netname; it appears to be case sensitive. Am I missing something else?
Thanks a lot for your detailed explanation. I have now found View-> Net List. This is all working OK and now I have a better understanding.
Just an idea/comment (probably number 4,809 or so on the list) but when stitching vias it would be nice if I could select one or more vias at a time, and then edit the properties of all of them simultaneously, including selecting the net name from a list without having to type it in.
I suppose that if you have a bunch of them to change, it might be better to change one first, delete the others, and then duplicate or make an array of the one which has the correct net name. By the way now with August 01 2015 software I seem to be able to select a block of vias (such as 4-6 at a time) and duplicate them easily.
I guess that another possibility would be to include the vias as components (probably on a seperate sheet?) of the schematic, and let the software assign reference designations to all of them. The disadvantage of this would be that it is difficult to anticipate how many you may want to place on the pcb so some sort of back editing may be necessary?
I have been doing your (“uglier workaround”) and had not thought of your last point. I may try again with the vias in the schematic. I have a hunch that this might be the most “solid” solution. Sometimes whatever seems quicker at first can be more of a problem by the time you are done…
FYI I am engaged in an exercise to learn the software so whatever happens to this particular design is unimportant. But this has been a pleasant and enlightening experience.
Airic, thank you. I had the same issue. I saw that black box but it didn’t occur to me that I needed to drag that on the wire.
Here is a label that is not connected:
And here is a label that is connected.
Note that the black rectangle disappears. You then have to export the netlist and import it in PcbNew. As usual, PcbNew doesn’t know about the changes you made. So for instance if your track was linked to a copper field then the copper field loses that association and you have to redo it.
Another trick to help with schematic documentation. If you precede your net name with the tilde character “~” EESchema will put a line above the label text. Like what I did to “NET2” here:
This is done to indicate a low active signal, and makes it easier to know what to expect when troubleshooting your circuit (or remind you how to drive your µC pins in your programs).
