[solved] Ratsnest not updating correctly (reason: symbol, same pin number, different pin name)

Schematic
1

Hi, I’m a student who is new to both PCB design and KiCad, I’ve spent a good while looking through some tutorials and been doing fine in my work so far. Now I’ve got a new mini-project going and my goal is to produce a prototype PCB for some testing of a couple of resistors. I want to use the method of 4-terminal sensing, and have therefore drawn a schematic with 2 N-type PCB mounts.

Now, the problem I’m having is that, when I start PCBnew and read my netlist, all the footprints load in correctly but not all connections are drawn. One of the coaxial connectors gets left haning in the air. Like this. (Not sure how to attach pictures)

Also, here is a picture over the schematic in Eeschema. I’ve already tried moving around the joints with “G” to check that everything is indeed connected.

Any help would be appreciated!

2

You should be able to drag and drop pictures into the reply box. (As a new user you can only post one picture per post.)

Now to your real problem:
I noticed that sometimes pcbnew does not update the view correctly. In this cases it helps to restart pcbnew.
You can also try to switch between opengl and legacy canvas. And run drc.

If this does not help we might need more information.
Especially: What kicad version are you using. What operating system.

2 Likes
3

Did you try to switch to OpenGL yet? [F11] (back to Legacy via F9]
It shows the ratsnest a little bit better.

Also, post the netlist file if this doesn’t help you.
We can check if the net is correct or not… it’s just 4 devices, shouldn’t be big.

PS:
pictures can be attached by either using [Ctrl]+[v] in the reply window (if you got one in the clipboard) or there is a little button for uploading things and last but not least you can drag+drop images from your computers explorer into the editor box as well…

2 Likes
4

Have you tried to generate a new netlist? The schematic looks fine, but in the layout it seems E1 and I1 are connected, and the same for E2 and I2.

2 Likes
5

If the legacy view doesn’t update correctly I found it helps to just use [M] on a device and then abort the operation by hitting [ESC]

1 Like
6

Thanks for the quick reply! I’ve now tried restarting pcbnew saving/loading the netlist again and it doesnt seem to help :confused:

1154×1080 92.6 KB

If I run drc and check the unconnected pads, it seems there is no net including any of the resistors and the component “J2”. Would this suggest the problem does lie in the .net file?

Here is the .net file as Joan suggested! shunt_prototyp.net (2.9 KB)

7

In the netlist you can see that J2 is not connected to the shunt.

You might want to do an new annotation before generating the netlist. I had similar situations when I erased a part, copied a new one and edited the reference designator manually (‘U’) to reflect the original reference designator.

8

I tried this too, but as you are saying E1 and I1 are connected, wich is how it should be (at least in my head, maybe this is not how you do things in pcb design though?).
For reference here is the resistor I want to place. And as the internal schematic suggest both of the legs are connected from “inside” the resistor.

9

I’ve noticed that this can indeed help in some situations, but it would seem that in this case the component isn’t actually connected to the rest of the schematic, right?

10

Can you please grab this corner [G] and try to move it around - what happens?

1 Like
11

I tried moving all of the corners around for you here.

378×510 3.77 KB

Also I made a zip with all the project related files if you would want to have a look prototypproblem.7z (4.4 KB)

Oh and also I’m running the 4.0.6 windows 64-bit version of KiCad…

12

That’s how a 4 wire connection is supposed to look like.
This way one has 2 wires that have a high current on them but the wires for measuring the voltage drop has only a low current on them.
https://www.cirris.com/learning-center/general-testing/special-topics/40-4-wire-kelvin-testing

Back to your problem.
Did you run an electrical rule check on your schematic? If not: run it and show what it says. (If @Joan_Sparky is correct, then you will get a message about unconnected pins.)

13

The netlist generated looks like this (straight loading of the project, done nothing else than hitting the netlist generator button):

  (nets
    (net (code 1) (name "Net-(J2-Pad1)")
      (node (ref R1) (pin 1))
      (node (ref R2) (pin 1))
      (node (ref J2) (pin 1)))
    (net (code 2) (name "Net-(J2-Pad2)")
      (node (ref R1) (pin 2))
      (node (ref R2) (pin 2))
      (node (ref J2) (pin 2)))
    (net (code 3) (name "Net-(J1-Pad1)")
      (node (ref J1) (pin 1))
      (node (ref R1) (pin 1))
      (node (ref R2) (pin 1)))
    (net (code 4) (name "Net-(J1-Pad2)")
      (node (ref R1) (pin 2))
      (node (ref R2) (pin 2))
      (node (ref J1) (pin 2)))))

shunt_prototyp_3.net (3.1 KB)

PS: I assumed that the corner would have been not connected properly and some visual glitch didn’t make it obvious, but moving everything and it keeping together ruled that one out.

PPS: I’m running a nightly from 12th May on Win7 64bit though which I can’t fail at the moment… Version: (2017-05-12 revision b823d0b78)

14

Hm the one i get with version 4.0.2 looks very different.

(nets
    (net (code 1) (name "Net-(J2-Pad1)")
      (node (ref J2) (pin 1)))
    (net (code 2) (name "Net-(J2-Pad2)")
      (node (ref J2) (pin 2)))
    (net (code 3) (name "Net-(J1-Pad1)")
      (node (ref J1) (pin 1))
      (node (ref R1) (pin 1))
      (node (ref R2) (pin 1)))
    (net (code 4) (name "Net-(J1-Pad2)")
      (node (ref R1) (pin 2))
      (node (ref R2) (pin 2))
      (node (ref J1) (pin 2)))))
2 Likes
15

Cool, now we got a bug.
The 4.0.2 and 4.0.6 netlist look alike, but are not correct, the nightly version from 12th May is correct.

How do we nail that one?

1 Like
16

Yes, I did run an erc with default settings and got no errors or warnings.
Could the problem have something to do with the fact that the component “CONN_COAXIAL” only has 2 pins and the footrpint I made for the PCB-mount has 5 pads?

17

No, the netlist is wrong… PCBnew is not at fault. This is some error in EEschema related code that makes the netlist.

PS: if you download the netlist file in that post up there with the _3 in the name… can you load that in PCBnew and look if it solves the problem for you?

18

I think the problem might be that two pins of the symbol have the same pin number. This should not be done. (E1 and I1 currently have the pin number 1. E2 and I2 have pin number 2)
The correct way would be to give the symbol one pin number per pin. (Or to only have two pins in the symbol.)
If @EJones decides to go the road of 4 pin numbers in the symbol, he also needs to change the footprint accordingly.

Edit:
output of the erc check of the symbol:

Duplicate pin 1 "I1" at location (-0.200, 0.000) conflicts with pin 1 "E1" at location (-0.100, 0.150).
Duplicate pin 2 "I2" at location (0.200, 0.000) conflicts with pin 2 "E2" at location (0.100, 0.150).
1 Like
19

Again: try an extra annotation, or did you?

20

I did try that, I’m going to edit the component as @Rene_Poschl just suggested and see if that solves anything.