I have an odd problem. I am using the latest nightly (April 8) and one of my nets seems to disappear when generating the netlist. I have a net labelled +13V8_F:
These are not connected anywhere that I can find. When I generate a netlist, the +13V8_F net is simply not in there- I did a search after opening it with Notepad++. It appears that +13V8_F has been assigned to +10V. I opened all the schematic files and searched, everything looks okay as far as I can tell. There was no hint of this in the DRC either. I added the net label explicitly (twice) to make sure it was in there, but it does not appear in the netlist.
I did a search for each of these and examined every instance, they look correct.
Is there any way to find if two nets are inadvertently connected? (I am sure it must be something I have done, but I am drawing a blank right now).
You are using a schematic symbol for +13V8_F.
My guess is that you copied this symbol from the 10V power symbol, but forgot to remove the link that KiCad uses to connect all the +10V power symbols together.
So your _13V8_F symbol is actually a +10V symbol with a misleading name.
I am a little confused here. I have a bunch of power symbols- +5V, -5V, +3.3V etc. These were all created from the same symbol and re-labeled. All of these seem fine except for the +13V8_F. I have opened these one at a time in the Symbol Editor and I cannot find the “link that Kicad uses” to connect them together.
All of them have a Reference of “#pwr” and they seem to be distinct on the schematic ("#pwr0178" and so on).
If I go into my power symbols library with a text editor, what would I be looking for? Presumably something I cannot access in the Symbol Editor?
Quick response:
Rene wrote that the “Link” is made via the name of the pin itself.
I opened up the default +3V3 power symbol in the Part Library Editor.
The string +3V3 appears twice in that symbol.
The horizontal string is a “Field Value”.
The Vertical, hidden, string is the “Pin Name”.
I think that the “Pin Name” is used to make the “Link”, and you only changed the “Field Value”.
I wanted to readup in the EEschem Reference manual on how this works exactly, but your post seemed to warrant a “premature reply” from my side.
I think it is a combination of the #pwr? and/or the “Pin Type” set to the Electrical type “Power input”.
It seems a bit weird to me that a “virtual” symbol has an actual pin.
Edit:
You can make the invisible pins visible with:
EEschem -> Preferences -> Schematic Editor Options -> [ ] Show hidden pins.
Yes, I have found a solution. Using Notepad++, I found that in the +13V8_F symbol definition in the library file, two fields do not agree:
+13V8_F
DEF +13V8_F #PWR 0 40 Y Y 1 F P
F0 “#PWR” 0 90 30 H I C CNN
F1 “+13V8_F” 0 150 50 H V C CNN
F2 “” 0 0 60 H V C CNN
F3 “” 0 0 60 H V C CNN
DRAW
X +10V 1 0 0 0 U 20 20 0 0 W N
C 0 50 20 0 1 0 N
P 4 0 1 0 0 0 0 30 0 30 0 30 N
ENDDRAW
ENDDEF
I am not sure what the X field refers to, but apparently it has to agree with the F0 field. Once I edited that to X +13V8_F …, the problem went away. It would be nice to know if this could be done in the Symbol Editor. But as always, a good text editor is essential with Kicad.
For all my other power symbols, when I created them the X field was filled in correctly, and hence no problems.
Thanks for the pointers- it made me hunt around until I found it.
We are talking about exactly the same here.
The lines starting with “X” in the library are the definitions of the “pins”.
So, although your immediate problem is solved now, I think you should read a bit on how this actually works in KiCad.
