OK, I’m new at this KiCAD, but I kn ow that if the schematic doesn’t show two terminals shorted together, the PCB rubber bands shouldn’t either.
The V+ out and the V- out of the PFE-700S switching power supply symbol I made aren;t shorted together on the schematic, but pcbNew shorts them together. Does this have something to do with the pin names or ???
Here are some screen shots, if I can upload them OK
Anyone get what’s going wrong?
Thanks
Correct
There is more than just those 2 pins in variance - Generate a new NET file, from the SCH, then open in a Text editor and check the net connections. It is a simple ASCII file you can search.
Then, ensure you import that NET file into PcbNew
Try dragging the four capacitors above the IC to check their connectivity. A common mistake is connect the wires to the wrong pin and fail to see the wire under the capacitor symbol or to rotate the capacitor symbol 180 degrees. Either is shorting the nets out and we wouldn’t be able to see it at that level of zoom
Carefully check your drafting on the schematic, generate a new *.net list, and import it to PCBNew.
If that doesn’t help, studying the *.net list in a text editor probably CAN point you toward the error . . . . but diving into the netlist like that probably isn’t the most efficient way for a new user to work. Instead, review both the symbol and the footprint for the PFE-700S in the symbol and footprint editors, respectively.
If nothing seems to be amiss, post the symbol and footprint here.
Dale
The expectation is not that a new user works by editing net lists, but they should know what a NET file looks like, and when it is generated, and how to scan one, when there appear to be net-divergence issues.
Given there is a lot more wrong that just 2 pins shorted, I’d guess the OP is working with an old/incorrect NET file.
Thanks for replies.
I redid the schematic and added in a couple components so I could be sure I knew I was reading the correct netlist. Corrected other errors while I was at it. KiCAD just doesn’t seem to want to stop shorting the output pins of the module together. The capacitor rubber bands are fine. It’s just the PFE700s-48 module -V and +V pins that are scewy.
Here are the schematic and footprint symbols.
pfe700s-48.lib (849 Bytes)
PFE700S-xx.mod.kicad_mod (3.8 KB)
Really appreciate your looking at it. I’m baffled.
Bart
Beware of the rats nest display -it can be misleading where there are overlapping lines.
Use the “highlight net” tool in pcbnew to discover which pads are on a net.
This has got to be a bug in KiCAD. When I highlight the net - it shows the correct connectivity for both +V and -V, the capacitor bank, and +VM and -VM.
Interestingly enough, the connection between C23 positive terminal and +V doesn’t show up as a rubber band, but the" highlight net" shows them as connected, along with the bogus rubber band connections between +V and -V, and between +VM and -VM.
Check out the pics
Sorry about the wierd space before the “highlight net” shots - I don’t seem to be able to remove it from the post.
Bart
Here’s the overall schematic and pcbnew rubberband view, in case that helps.
Should I be posting this somewhere else?
Thanks for being kind to a newbie.
Bart
I think @bobc is correct, this is likely a render artifact/bug.
Try routing short traces from +V, -V and see if issue is maybe overlapped rats XORs back to black.
Try different View Canvas settings, as they do render differently.
Your problem is that rats nest lines of different nets drawn over each other in Legacy canvas will disappear.
The ratsnest line between pin 3 & 5 and the other between pin 2 & 4 overlap in the area between 3 & 4. That’s where they become ‘invisible’ in that canvas.
Switch the canvas to OpenGL and you will see them all the time.
It’s a bit irritating, but if you route with DRC enabled it won’t actually let you connect wrong nets together, so there is nothing buggy here, besides the rendering.
And as it’s the legacy canvas there won’t be any work on that as the effort is on the OpenGL one.
Why are both canvases still active?
The OpenGL misses some stuff still that the Legacy has and makes it useful to keep around.
Thanks for all the helpful feedback. Especially the explanation of lines becoming invisible when they overlap in some way. Understanding that really helps.
Buggy rendering I can learn to ignore. I will try using the OpenGL rendering - I had chosen the one with the KiCAD name thinking the OpenGL was for people porting designs to other layout programs - I probably skipped something in the documentation on it figuring I didn’t need it.
BTW, I like the interface so far !
Bart
As I said, currently the new standard canvas (OpenGL) lacks some features that the Legacy canvas has… you will be switching between them for the time being to get the best of both worlds (there was a thread about it a couple of days ago: Pcbnew canvas differences).
Personally I use legacy 95% of the time.
