Hello everyone, this is my first post here. I am in the process of migrating from Eagle to KiCad and I started importing schematics and related footprints without any routing. The import was successful (I did it only once!), I started slowly with the routing on the KiCad side and in that process it was necessary to correct the wiring of some components. This was done in the Schematics editor and âUpdate PCB from schematicâ (F8 option) was used. In several iterations it worked correctly until yesterday at some point I started getting cryptic messages and it seems I lost sync between schematics and PCB layout. I donât know what to do next, I tried to go back several versions from the backup folder, there I can find older versions with which I could possibly continue to work, but I donât dare if I will face a similar problem in the future that I will not understand how it happened. Thanks in advance for any assistance.
First, welcome to KiCad, (and this forum) 
I tinkered a bit with your screenshot:
Those Updated messages with the UUIDâs are informal. Errors and warnings start with Error: and Warning:, and they are probably higher on the list. Scroll upwards, or save the ERC report in a file and paste the text here.
This forum software also has some automated anti-spam measures in which rights are gradually granted as you gain more âexperienceâ on this forum. More details in:
Also posted on:
Thank you so much for prompt reply. It seems that as a new user I cannot attach file. Here is the screenshot of the bottom:
I would also like to share with you the consequences of these messages that I found suspicious. First, when trying to add a new RN symbol, it offered me the designation RN8, although I only have 5 on the schematics, so it turns out that there are two âphantomâ (invisible), RN6 and RN7.
Additionally, when unrouting previous lines, it looks as if some of them no longer exist at all.
It seems that as a new user I cannot attach file
read and follow the ânew memberâ link provided by paul. You need to read at least Thirty different posts in at least Five different Topics for at least Ten minutes to get the next basic user level. (you have not read the â30â posts yet).
so it turns out that there are two âphantomâ (invisible), RN6 and RN7.
You could use the âFindâ function to search for RN6/RN7. Or use âToolsâ>Edit symbol fieldsâ to open the symbol fields table which shows all used symbols in the schematic.
Additionally, when unrouting previous lines, it looks as if some of them no longer exist at all
Board and schematic are not as tight coupled as in your previous EAGLE version. It will need some time to get used to this different concept and to avoid the disadvantages, but to make use of the advantages.
Some things you have to get used to:
- if you delete a wire in the schematic then the board is not affected, all tracks remain on the board.
- Wires (in schematic) and tracks (in the board) are syncronized by their netnames. The netnames itself are:
- either given explicitly by you (with local+global labels or with power symbols).
- or the netnames are given automatically (if you donât place a label on the wires). These automatic netnames are created by a combination of connected symbols + pin/pad-names.
- If you delete and redraw wires in the schematic and they get different netnames then sometimes the tracks in the board either remain their old netnames or get a âno netâ name or get a netname from the remaining pad which they are connected to. Such tracks must be manually deleted (or renamed to the new netnames).
a remark to your âupdate pcb from schematicâ window: I would recommend to normally enable the checkboxes for:
- delete footprints with no symbols (otherwise you could end up with a bunch of orphan footprints on the board)
- replace footprints with those specified in the schematic (consequently a change of the used footprint should occur on the schematic side)
Thanks for your inputs. Iâm still struggling with those UUIDs that seem to appear in a completely random fashion. For example, if I donât touch anything on the Schematics editor page and do an F8 update, I get this:
https://i.imgur.com/MQCcDdA.png
⌠then I close the project and open it again and try to update the PCB layout from the schematics again and then I get this:
https://i.imgur.com/RByYiFg.png
Attached is the latest report.txt (now I can also upload files :)âŚ
report.txt (23.3 KB)
I donât know if the appearance of those warnings is the reason why some routes when unrouted disappears completely (see the video in the previous post), which is my main concern.
now I can also upload files
congratulations.
Try to produce a zipped archive from your project (Kicad main managerâ>Fileâ>Archive project) and attach in this thread. Maybe we can investigate better then.
Are you sure they follow the connection from schematic. If you look closer you should see net names at pads and tracks. May be these were âNo netâ tracks so KiCad didnât miss them when they were removed.
I updated post with your screenshot, to clearly show you have turned off the warnings in the ERC dialog. If you change those checkboxes, you will see the warnings:
Warning: No net found for symbol B1 pin PS1.
Warning: No net found for symbol Y1 pin NC.3.
Warning: No net found for symbol Y1 pin NC.2.
Warning: No net found for symbol X6 pin SH2.
Warning: No net found for symbol X6 pin SH1.
Warning: No net found for symbol X4 pin SH2.
Warning: No net found for symbol X4 pin SH1.
Warning: No net found for symbol FM1 pin T.
Warning: No net found for symbol FM2 pin T.
Warning: No net found for symbol FM3 pin T.
Warning: No net found for symbol FM4 pin T.
Warning: No net found for symbol IC10 pin 7.
Warning: No net found for symbol IC10 pin 8.
Warning: No net found for symbol IC10 pin 9.
Warning: No net found for symbol IC10 pin 15.
Warning: No net found for symbol J1 pin P$2.
All the warnings are about No net found. KiCad relies on the pin numbers (which are actually 4 character alpha numeric strings) to match the pins in schematic symbols with the pads on the footprints. You have to modify either the schematic symbols, or the footprints so the pin numbers match the footprint pads.
I donât know what the video with the disappearing tracks when you move your mouse over it means. Without further context it has no meaning to me.
Thank you all for your attention and answers! It seems to me that after all the problem with the âdisappearanceâ of the lines after unroute is due to the fact that in Net Classes (2) it was necessary to do hide/show in order to show the line again (1). I donât know if itâs a feature or a bug, either way itâs confusing for a beginner like me.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.