Rat's Nest won't go even after routing

Even after manual routing the rat’s nest won’t go between few pads. And when I went for auto routing , it didn’t route those specific pads. Hence it is showing under unconnected section. What could be done?

Zoom in on those pads and be certain that the tracks actually go to the center of the pad. (Some users like to put the display into “Outline Mode” for tracks and pads when they do this.) It is possible to lay down a track that almost-but-not-quite connects to a pad, especially if the footprint is not aligned with the grid in PCBNew.

[quote] . . . . And when I went for auto routing , it didn’t route those specific pads . . . .
This sounds like an error in the schematic. Could be the connection lines are almost-but-not-quite touching the pins of the schematic symbol, or the netlist is being fooled by an “invisible pin” on a schematic symbol.


1 Like

I spaced the components a little and removed all my manual routing, then went for auto routing and it could route it all. So any thoughts on this? because had it been a schematic error then it shouldn’t have routed no matter what.

moreover routing done by auto routing confuses me…because it seems its allowing tracks to crossover on the same layer.Any thoughts on this?

thank you

screenshots would be nice to understand what you see and don’t understand :wink:

this is after spacing …the latest…here all routing done by auto routing …but if you look carefully it has tracks overlapping on the same layer.especially between seven segment and the resistors.

I am a novice at this, so if anyone would like to suggest better routing or placement of components, you’re most welcome.

OK, that helps.

Uhm, that’s what the ratsnest is there for to help you with and what your job is :wink:
You move, rotate the devices until the ratsnest (or better sub-groups of it) become easy peasy.
You stick to one side of the board F.Cu or B.Cu and arrange them so that the tracks between them are simple.

And if you do hand soldering you put them in a line mostly to get to them with the soldering iron easily.

If there are electrical/mechanical conditions which put constraints on placements/distances they rule over all else naturally - like high vs. low voltages, EMI, displays, buttons, connectors, high speed buses, RF, thermal islands with big copper planes for heat dissipation, etc. pp.

It takes some time to do a layout - always.
Auto routing only helps if it’s dead simple and you worked on the low hanging fruit.

This took me 3 rounds of optimizing:

Now to that dogs breakfast of yours :scream:

I tried to increase the visibility, but I can’t see tracks on the same layer overlapping.
Red is F.Cu and green is B.Cu I assume… lot’s of vias and criss-crossing, but no errors afai-can-see.
Also the auto router seems to use other angles than 0/45/90 degrees, which makes it hard to follow.
And you putting the transistors up there to the right and the resistors down there doesn’t help things - it makes it more complicated.
Starting as a beginner and using an auto router is as bad as it get’s.
You’ll never learn what is needed to do it properly and which of the results of an auto router you have to rework.

Here is what I would do:
Delete the autorouted tracks.
Look at the ratsnest.
Move/rotate transistors and resistors for as long as it takes to make it look like the first example I posted up there (with the tracks all in green).
Once you got that you can drag the display and the connector into it as well and move it around and see if you need to make any changes to the transistor/resistor groups.

Can you assemble from both sides?
The display and the connector look like through hole components and the other stuff like SMD?
Any chance you want to place the SMD stuff on the other side from the display/connector to make the pcb smaller (costs less - can probably have 2 pcbs in the space that now uses your 1 design).

Is that a student project where the pcb will be milled?
Or is this going to be a real 2-sided pcb from a fab with silkscreen/soldermask?


First of all, thank you very much for such a detailed and insightful reply. I am very keen to learn and improve.

No, its not a student project , we are new to pcb designing. Well, I just confirmed that its better to have all tracks on one side.

I did two sided to make the size small .But still keeping the size small, better tracks can be put I guess.

Yes, connector and display will be used as through hole and rest as SMD.

It will be sent for fabrication.[quote=“Joan_Sparky, post:7, topic:5190”]
Look at the ratsnest.Move/rotate transistors and resistors for as long as it takes to make it look like the first example I posted up there (with the tracks all in green).Once you got that you can drag the display and the connector into it as well and move it around and see if you need to make any changes to the transistor/resistor groups.

Please elaborate on this too.

and you say you can have two pcbs in the space I have used for one, please if you can elaborate on it too.

thanks !

above images for in case.

the schematic, in case it helps in explaining.

is this anything better as a layout?

Again, delete the auto routed tracks - they’re useless.
You tried to run before you could walk or even crawl.

Fabrication means, they do 2 layer routinely and 1 layer will cost more.
You will be doing 2 layer then.

display + connector = through hole, so manual mounting.
This means to get the smallest real estate possible (with most amount of freedom) you want the SMD stuff on the back.

Is the pin order on that connector fixed yet or can it be rearranged?

There is not much more elaboration possible, I’m afraid.
You have to walk through that door - I can only show it to you. :wink:

Back up the project so you can revert to your current status if something goes wrong (hit the [zip] button in the project manager).
And if you can attach the zip here.

Here is the door:

  1. delete the tracks - all of them (in legacy canvas you can draw a selection bracket over all and select the tracks only and thus delete them)
  2. hover with your mouse over each transistor and resistor and flip it to the backside (hit [F])
  3. move the display and the connector out of the way
  4. move + rotate the resistors and transistors until the ratsnest between them is simple

I think your schematic needs some work first. And it would be a good idea to label the pins of your connector according to function.


I agree with @1.21Gigawatts.

But i would like to give you a bit more guidance what specifically could be done better.
First of all, why labels:
If you label a wire, the net gets this name. This makes it easier for you when you layout your board.
(net names are shown in the pads/traces.)
It also makes your intentions more clear. (Example: where the ■■■■ is your ground connection?)

How to add labels:
In kicad there are 3 types of labels.
Global labels: labels that are valid across all hierarchies. (Power symbols are global labels)
Hierarchical labels: Labels to define the “interface” of the current hirachical sheet. (To connect to the parent hierarchy)
Local labels: These labels are valid only in this hierarchy (=sheet)

I would suggest you use local labels for adding more information to your schematic.

I would also use power labels for the connection of your transistor emitters. (would make it a bit more readable.)
Maybe also add one for your gnd pin.
I would also strongly advice you move the wire connecting R6 to Q6 in such a way that it does not cross over the ends of the resistor symbols. Kicad sometimes thinks stuff like that should be connected.

Otherwise i think not a lot can be done to make it more readable. (without changing symbols)

1 Like

There’s also the fact that it probably won’t work as drawn. It would appear you are using a Common Anode display and the PNP transistors are likely intended to source to each digit yet only one transistor is connected to a digit’s common anode while the others are connected to segment cathodes.

560R is a bit low for the base drive of those transistors but then again we don’t know what your supply voltage is.

There’s no need for a ground.


You have a wonderfully patient, organized, clear and concise teaching style. :heart_eyes::kissing:


1 Like

Yes, in general, the schematic is ALWAYS helpful to me. The schematic is the language you use for communicating your intentions and the ideas arising from those intentions. (But then, I have been looking at schematics - often holding them in one hand, while holding the corresponding physical assembly in the other - since I started to learn electronics well over half a century ago. Others may use a different form of communication.)

If the schematic is drawn well it usually gives a reasonable first-guess at an effective board layout. Spending a little time to un-jumble the schematic will typically save several times as much time in creating an efficient board layout.

This particular schematic raises several questions even before we begin to consider a board layout. Others have already noted the questions so I won’t repeat them. You seem to be teachable :smile: and there are many on this Forum who are quite willing to share their knowledge and experience. Most of us won’t live long enough to create optimal solutions to every problem on our own, so it is efficient to learn from the solutions developed by others.



Well, I am not allowed to upload attachments(.zip file) since I am a new user on this forum. Could anything be done about it? or do you wish to share your email id or anything else?

And ! Wow ! I being a novice am having a problem in India and people from all around of different ages are willing to help. Grateful. I shall go through all what you guys have suggested and report in a while. Thank You.