I am trying to finish up my first pcb with KICad. I am having a problem gettting the GND pin from one component to connect to a pin on my connector.
The GND pin is listed as a pwr output but I have also tried just output. No matter what I do I cannot find a way to connect the GND pin from my Arduino component to my connector component. The connection is made in the schematic but does not carry over to the pcb.
Any ideas what I am doing wrong?
Press E for edit when you have the mouse over a pad. Look at the net name in the dialog that opens.
Make sure the net name is exactly the same on the pads you want connected.
On the schematic side if the power/GND pins are hidden they might be named something non-obvious (like VEE/VSS or whatever)
you might also look at the netlist file (.net) of that project and search for entries starting with:
(net (code ...
One of those entries will be for the net of either the connector pin or the components ‘GND’ pin… they should be both listed under the same net there.
For examle:
(net (code x) (name GND)
(node (ref C1) (pin 2))
(node (ref U1) (pin 6))
(node (ref C2) (pin 2))
(node (ref SW1) (pin 1))
...Thanks for the responses.
I will check the netlist file.
The net names are not the same which is the problem. What I don’t understand is why this particular connection is not being made. Perhaps some pictures will help show the issue. Of course I am having issues posting images since this is my first time on the forum.
What is up with pad/pin numbers for those symbols?
The pin numbers (be they letters or numbers) need to match the pins in symbols AND in the footprints.
If you got a connector with 3 pins and the symbol has got ‘GND’ as pin number the footprint will also need a pin with that number. But this will cause havoc and proprietary among your footprints… stick with numbers for pin numbers, so you can REUSE footprints and symbols.
I think (with what little I know of this) you’re treating the system wrong.
If you want nets with names like ‘GND’ you either have to use the pin/pad name field or add labels (local, global or hierarchical) to the nets (wires) in eeschema…
The way you do it now is wrong IMHO.
Who made those symbols?
Here is the part in question:
(net (code 32) (name “Net-(P3-Pad2)”)
(node (ref P3) (pin 2))
(node (ref U1) (pin VCC)))
(net (code 33) (name “Net-(P3-PadGND)”)
(node (ref U1) (pin GND))
(node (ref P3) (pin GND)))
The U1 part has 3 GND pads. Would having 3 pads with the same name be the issue? What would the solution be?
Thanks
I do not doubt it is wrong. This is the first board I have ever made. I labeled the pins according to what they were on the spec sheet as it seemed to make more sense than just using numbers and alpha numeric codes were allowed.
Is this a bad practice? Is 1,2,3,4, etc better?
I made the symbol for U1 and change P3 to include the GND pin when things were not working correctly.
I will try changing all pins to numbers.
Check the footprint of that IC you’re using… those will be numbered with 1,2,3, this is universal among all ICs or devices (I know BGAs will have A1, A2, A3… B1, B2, etc. pp).
So for example if you got an ATtiny with a SOIC20 housing and a MAX323 with a SOIC20 housing, the numbering of the pins on those housings will be the same.
KiCAD only has to know one SOIC20 housing to be able to make this work…
The symbols in eeschema will need to match that numbering scheme as the logical wiring you do in eeschema shall translate into tracks that will work with what you want.
If you do create symbols you use the name field for the function of those pins…
And if you need a label that you can ‘understand’ later and will be visible in pcbnew, you place a local or global label on one of those nets/wires.
So yeah, get used to pin numbering with 1,2,3,4 and use the name field for the information that hints at the function of a pin.
I made the footprint, so everything matched. I think the problem was that there were more than 1 pin numbered GND. I changed all the pins in the component and footprint to numbers 1-24 and now the connection works.
I think it would have worked if I had changed the GND pins to GND1, GND2, GND3, etc. But since plain numbers seems to be the more common way to do it I went that route.
Thanks for the help.
Well, using plane numbers (1, 2, 3 etc) or alphanumerics (A1, A2, … B1, B2, … etc) is not a more common way, it’s the only right way and all components I’ve used had their pins numbered that way in datasheet.
Just curious, what is the component you had troubles with?
Whether pins are numbered or named shouldn’t matter, although conventionally people use numbers. Kicad can also handle multiple pins with the same name.
I am sure I have used footprints with odd pin names in the past without problems, but Kicad has changed the way nets are named. Possibly there is confusion if you have the same name as power nets, as they are handled specially.
