Hello,
Is it possible to create a PCB directly under Pcbnew without going through a schematic (therefore without routing) ?
This is an experimental stage where there will only be pre-wired sockets and connectors and power tracks. I have placed my components but when I want to trace a track between 2 pads, I have the message “ErrType (4) - Track near a pad:” and the track cannot be placed. Is there a solution ?
Thank you in advance.
AFAIK the PCB board will electrically be the same as the schematic. So no you can’t easily force a new connection in PCBnew.
You might (not sure), however add be able to add un-associated copper areas. Assuming you are copying a board of some sort you should try to get a schematic. Most breakout boards have their schematics somewhat on the internet.
- Stop being stubborn for the sake of it, and read on.
- Make it a KiCad project. not a loose .kicad-pcb file.
- Make a schematic. Put generic connectors on it with the correct pin count.
- Give the connectors the same Refdes names as the Footprints you put on the PCB.
- Pcbnew / File / Export / Footprint Association File…
- Eeschema / File / Import / Footprint Association File…
- Lay out the wires in the Eeschema.
- F8 to put the netlist in Pcbnew again.
- Lay your tracks.
From a distance it may seem “straigt forward” and “simple” to make your PCB without a schematic. In practice however you’re rowing against the workflow.
If you’re having trouble with this and If this project is not a state secret, then post your project here and I’ll have a look at it.
If your current workflow does not even put footprints from the Footprint libraries on your PCB you’re even rowing against a much stronger flow. Sort of rowing up a waterfall.
Also, any extra information of what you want to make is a plus. STEP models are the best, then you can draw a real footprint around them. Even a photograph from hand drawn graphics (with pen and paper) is useful.
Depending on the amount of work involved I may do most of it, or just enough to give you an idea of how it works and explain some things here on the forum, so you can do the next board yourself.
1 Like
Or, if you prefer to be stubborn:
In Pcbnew new you can easily add pads of Footprints to existing nets, but creating new nets is a *&^%$#@! as far as I know.
You could make a very simple generic schematic just to get some nets into Pcbnew. something like:
( you NEED to add footprints to the connectors for the nets to end up in Pcbnew.)
Then after [F8] to get the netlist into Pcbnew you can click on any pad to highlight it, then click with the right mouse button on the pad and select “Propierties…” from the context menu, or just press the shortcut key e for edit.
Then in the “pad properties” window you can add one of the nets to that pad.
(This 2nd screenshot is from a different project with different net names as the first screenshot from the schematic).
Yes, it is possible.
Disable DRC, first icon on the left sidebar.
But you’ll have to deal with the lack of a netlist, a ratsnest and netnames. Any pad can be connected to any other pad.
I had been experimenting a few times with that and I could not get it to work.
Today I read the tooltip text which made it all clear:
The Legacy Toolset is getting ever more obsolete and will completely disapear some time in the future. On my Linux machine it already has disapeared. The new Toolset is also already much better.
So the way forward is with the modern Toolset and the (absolutely wonderfull) interactive router. And I experimented a bit untill I got it to work.
In this window:
Pcbnew / Route / Interactive Router Settings
Use these settings:
The Key settings is first to set it to " Highlight collisions".
This will turn the option for: “Allow DRC violations” from grey to black so you can turn it on. You can experiment with the other settings according to your needs and personal preferences.
After that you are on your own and can lay tracks anywhere you like. Proof in screenshot:
1 Like
Try avoiding sharp corners in your design >90°, it has some disadvantages … 
disclamer: this is a joke. (one never knows)
Thanks Paul.
As I always use a schematic I didn’t notice the icon was intended only for the legacy canvas. I use kubuntu. The legacy canvas is gone too.
Hi @paulvdh and @pedro, I too have just changed to Kubuntu on a really fast Lenovo from an old , tired, PC running Windows XP and there seems to be quite a few changes from the KiCad Windows version I was using compared to the latest download. Paul, many thanks for those tips - I only make my PCBs for hobby use now (having spent 50+ years designing PCBs without being able to transfer the schematic across in the software package) so I tend to quickly runoff a PCB design without inputting the schematic, through habit, (although it would probably take me forever to input the schematic) but mainly because there are probably only a handful of components on the PCB and I will be etching it myself so don’t have to please a board manufacturer with the things that I do. Really grateful for the hints.
Sounds for me impossible.
In 1988, I spend few days to make it possible for me to run at my PC the software to allow me designing PCB based on transfered schematic. My PC had only 640k RAM and no HDD. My self made monitor was 14" B&W (rather black&green).
Hi @Piotr, I had to do it from a drawn (or printed) schematic on paper and design the PCB from that. It was good fun when dealing with valves (tubes) and 300+ volts to consider and avoid flash-over. Those were the days ! The very early designs were pre-computer and hand drawn with drawing pens onto clear film after primary design on squared paper. Much simpler now when even 5V is considered a high voltage although currents can now be in Amps rather than mA.
My first PCBs I designed (being a teenager) on squared paper and then printing it directly on PCB (using the pen refill with the ball removed), but whenever I was able to use a computer for this I used it.
Then I plotted it (borrowed plotter) at the back side of sheet from the wall calendar (2:1) and went with it to a photo shop to get the photographic film with my PCB 1:1. PCB manufacturer (just started that business those time) needed that as input. Not the gerber file 
Yes, see also this plug-in, which allows add-connection, split net etc nice features.
Thank you all for all your answers ! They are very interesting and informative. I will think about the most optimal solution for me. I think I will create a proper diagram with dummy components and proceed as it should for the PCB.
Greetings.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.