Hi everybody, I can add the shape ok and it shows up but I cannot route a signal to it (track disappears after routing).
I tried editing the pad to include the net name I am connecting too but it says “unknown netname”.
This is a pcbnew generated from a schematic netlist and I have already partly routed it with no problems.
I am sorry if this has been answered elsewhere, I have looked but not found so far, any help much appreciated 
Check spellings and use of special characters like “-” (dash) and “_” (underbar). I don’t know if KiCAD netnames are case sensitive or not.
Dale
1 Like
My first thought would be to run the DRC on the schematic. It souns like something is not connected. Either that or the DRC on the layout is set so you are going to close to another pad or via. There is sometimes a short message on the lower left of the screen.
Thanks for the replies, sorry I was slow to notice!
I ran DRC and its fine except all the incomplete routing.
This item only appears in the pretty library, it has no corresponding schematic shape so it cannot be included in the netlist and it’s got me wondering if this is the source of the problem ?
I am trying to do two things, add some wire links to the pcb to get past a large heatsink and also make some connection pads for a wire ended transformer, in both cases I dont see any schematic way of representing these so I am trying to add pads directly to the layout, so far without success!!
The message at the bottom of the screen when drawing a track from the new pad into an open area is “error type 4, track near pad” so my guess is it doesnt like me connecting anything to this wire_pad in pretty
Well make your own symbol and connect it in the schematic as needed?
Yes I think that’s gonna be the solution and thank you. I did try turning off DRC in preferences/general and that does let me attach a track to the pad but I think this will store up problems for later. Guess I thought as I found them in the pretty libraries along with wire links that have the same problem and there were no corresponding schematic components there was some clever bit of trickery for directly using them on the pcb, ohh well!!
Another option would be to edit your pad and give it the correct net name.
Yes I tried that but unfortunately it always gives “unknown netname” even though I tried several different ones that appear on pads on the pcb. I think I am going to have to start at the schematic even though it will make it messy!!
The answer to the net name conundrum is for some crazy reason it must be preceded by / so net fred has to be entered as /fred (in the pad properties)
No idea why but then it works!!
The / has to do with hierarchical sheet.
You can think of the hierarchy similar to a file-system. (linux file system.)
The first / is the root directory. (In kicad root sheet)
every further name between two / is similar to a directory. (hierarchical sheet)
The netname (text after the last /) can be seen in our analogy as being the file in a directory.
Well that’s good to know and it makes sense except I am confused as to why the guy didn’t do it in your tutorial video ?
Edit a pad that already belongs to the net. Copy the net field. Paste into the new pad net field.
There’s no need of / then.
Version 4.0.5 stable.
Gotcha! thank you everybody
That seems to be the general consensus among experienced users.
In my mind, the only valid reason for disabling DRC happens in the very early stages of a layout task. You may want to plop some components onto a board, then run a few traces simply to define your general approach to the task. Something like, “If I put the power supply in this corner, and the amplifier stages over there, I can run the input signals along this edge, and the outputs go to that other corner . . . .”, etc. After you have a mental image of how the physical layout will look, you enable the DRC and start placing parts or running tracks “for real”.
Dale
- If the transformer is physically part of the PCB Assembly, see my comment above, about associating footprints with schematic symbols. It means I can (for example) plunk a transformer symbol onto my schematic, and assign ANY footprint to it, e.g.:
- a 6-pin DIP IC footprint,
- the footprint for a 5-pin DIN socket,
- the footprint for an octal tube socket,
- a footprint I create from 6 pads,
- a modified version of one of the wire_pad footprints,
- etc.
- If the transformer is mounted off-board, your approach depends on the documentation standards applying to your organization, and how strictly they are enforced. Get help from your Configuration Control folks, or other designers with more experience dealing with your local bureaucracy.
In a strict environment the transformer will appear in the documentation for the next-higher level assembly, or another assembly at the same level as your board. In either case the next-higher documents will show connections to your board, and the points where the transformer leads connect will have designators starting with “J”. Your schematic will show each of these connections as a connector (with a “Jxx” designation), and it might be associated with one of the footprints from “wire_pads”.
In a lax environment, I would put the transformer onto the board schematic and treat it like my Case 1, above. I would draw a dashed (graphic) box around the transformer and add a text reference to “Note n.”. The body of “Note n.” would say something like, “Not a part of this assembly. Component located on main chassis.”, or “Typical interface to power input module. Power input module selection based on specified line voltage.”, etc.
Dale
Hello Dale,
Thank you very much for your fulsome answers/comments, actually I like KiCad very much, like all CAD systems it has it’s own library management and once you learn it there’s no problem, one of the good features is being able to very rapidly produce a schematic without worrying about footprints and being able to share shapes and footprints freely.
To me wire links are a construction feature and I had no desire to show them on the schematic, I place them directly on the pcb from the pretty library, change the net name and unlock the pads, I can move them wherever, label them with a bit of silk screen and problem solved except the rats nest remains, but hey I cannot have everything
I am doing some high voltage stuff at the moment so in the case of this particular transformer its primary is to pcb pins at the physical footprint where it is mounted but secondaries fly to different pcb locations, I found a solution, create a footprint with all the pins on the schematic as normal and then unlock the pads, then they can simply be moved to the location where the flying leads terminate on the pcb.
A wonderful package and many thanks for the good work
Best regards
Roger