Hello again,
I would like to make “viaducts”, i.e. a way to create space for tracks on the PCB, but without using 2layers. But instead break a track by inserting a kind of “jumper” , 2 through holes, which I can connect on the front with a short wire. (much like the space you get on the PCB by a component like a resistor). The two parts should preferably belong to the same network… And be visible on the schema level, or at least be preserved when imposing the schema onto the PCB anew.
This is a freqiuently asked question, how to add jumpers to a single sided board. Here is one previous discussion with some suggestions. A search will find others.
yes should be a very common issue for us single sided people 
thanks, will check
On the other hand, there seem to be a kind of request for KiCad to provide for this (special symbols ?), and not breaking up into several nets. So in order for the schematics to understand that the network is the same (when generating for the PCB), I think there is a need for a symbol.
Well it seem, (of cause) that this is an ancient theme and has be dismissed way back. So.
My own preference would be to use via’s and tracks on a separate copper layer. To do this, set the via hole and size to something you can drill a hole in, and solder a wire to. This method has a few advantages. It’s very simple and straight forward. You can make the “wire” bridges anywhere, and you don’t have to modify the schematic in any way. And if yo later decide to buy factory made PCB’s, you can send them the extra gerber layer too and you don’t have to make the wire bridges yourself.
For the rest. Sometimes zero Ohm resistors are used. You can insert these in the schematic too if you wish, or modify a (resistor or capacitor) symbol so it looks like a wire.
Thanks for idea. Though I have in mind to make PCB in .cn, which I have done successfully, and at that time not so expensive for a “test batch” of 15 cards. (that was before a serious re-do of KiCad, and I never got the design going again (I had done something that “renumbered” things so I could never get the schema to match the PCB, so now Im from scratch)) However I tend to remember that 2 sided were clearly more expensive… and I need like 4 jumps (just made on the PCB previous time, with pads&thl)
Recently I paid $5 for 10 boards, 2 layer, 64.92mm x 60.7mm
Last week I paid $55 for 5 boards, 4 layer, 132.2mm x 143.1mm
Shipping was the biggest cost, both delivered within 7 days . . . I consider this exceptional value for money.
Many PCB manufacturers do not even have a single layer PCB service anymore. Single layer is mostly used for mass production for relatively simple PCB’s such as power supplies.
4 layers is more expensive, especially in small batches, but when batches become > 100 PCB’s then the cost difference is also not so big anymore.
Also, if you design for more layers, then this allows to have at least one single GND plane, and this is beneficial for nearly all PCB’s.
There is a jumper feature in the next version of KiCAD. It is a bit clunky for this usecase as you can not move the pads independently as they are a single footprint only kind of stuff. But you could make a feature request request for spanning this over footprints.
Although obviously you can use the copper layers you don’t use for documenting the jumpers
Just because 2 layer boards are cheap does not negate the need for this. I do single sided boards with jumpers all the time, I make my own boards when i need a less than a day round trip time*. It would be super useful to be able to do this.
Jumpers also makes multi board layouts sort of possible, being able to move the endpoints would make it even easier. Supported or not.
* Yeah it happens that i may need to do different 4-5 boards on a one day timeline. I could make 2 sided (or more by lamination) but it requires less effort to do single sided as there are less tolerance issues.
KiCad does have: PCB Editor / Preferences / Preferences / PCB Editor / Editing Options / Editing Options / Allow Free pads, and when you enable this, you can move individual pads of a footprint. But I agree it’s a bit clunky. It’s a single setting that works for all footprints, and for most footprints it does not make any sense to make individual pads moveable.
I’ve never understood this request.
Why not just design the board as 2 layers, and throw the back side away?
Just put jumpers in place of the traces on the bottom layer.
Trivial.
go to Preferences > PCB Editor > Editing Options > Allow Free Pads. This can be handy to enable if you mostly do PTH boards where you want to be able to move individual footprint pins around for reasons like this.
ah, one should not “remember” but check. I just discoverd that pcbgogo actually had 30%cheaper for 2 layer than 1 layer !
So I try to put a via (from right side menu), a tiny spec. Well , a track from the via will by no means accept to connect to a pad (thats ground). If i go the other way from the pad, the track refuses the via…
Maybe explain what you are trying to achieve not what you did that didn’t work.
ah, things are not as simple as I thought;
as outlined above, I want to “bridge” over some tracks on the bottom layer, by going via a via to the top layer… and make a connecting track on the top layer between the two vias.
is use the “track routing”, which I guess makes some trouble, since that only wants to connect suggested connections from the schematic. so I guess I should look for some other means to create tracks.
You need to use net tie footprints, not vias. In V10 you will also be able to use jumper footprints (and keep the nets the same) but in V9 and older, you must split the nets in the schematic if you want to have the design “clean” at the end (no unconnected item warnings, etc)
I can’t see any way that this isn’t a mistake.
You won’t know what “jumpers” are needed until you start to route the board. Forcing them to be part of the schematic just locks you into a (potentially) non-optimal layout.
You should just route your board as if it were two layers, and strive to minimize the number of traces on the bottom. When you are happy with your layout, just change the vias to be the size you need for your jumpers, and mark the jumpers with a line on the top silkscreen.
Then, just send the top layer (and soldermask, etc.) to your fab house.
OK thanks all for a while. Will digest this and test. One more thing Im uncertain of is how to make a backup, part-step save. Is it “version control” right click on project, or is it save as… with new-vers name ?
Right, a guess a net tie footprint is a single pad with a net-symbol and a special made symbol for it ?
It has multiple pads, because each pad will join a different net.