Hi, and excuse me for my newbies questions.
I draw a schematic. This is a single layer with several jumpers wires,
I traced it with Eeschema, it’s OK.
But i want to register fingerprints with CvPcb, i can not find the jumper’s footprint in the list, where is it?
Hi, and excuse me for my newbies questions.
OpenGL pad clearance when moving or globaly
Using Kicad’s default libraries if you look in the Connect Library there is a part named ‘TESTPOINT’. You could use that I guess.
@cyril Well I guess you’re laying out a single-sided board, right? In this case the easiest way to emulate jumpers is to set up the board as double-sided, parameter vias and their drills the same size as regular pads. Whenever you need a jumper, place the via (“V” key), route the track on the front side and press V again to end it. You’ll have your “jumper” presented as a copper track on the front side. The advantage of this method is in flexibility: you won’t be limited by the size of the “jumper” component, it could cross other footprints too like real jumper wire could, contrary to a dedicated component which couldn’t.
Single layer, through hole, zone fill + jumpers, how to make it work?
The above answer by @dolganoff is good. I did that and another plus is, that you can print the front layer separately, which then shows how the jumpers are to be mounted.
Yes thanks, here there’s explanations, but it in french:
Right, this is it.
For the “jumper-compatible” PCB design you’ll have to increase via size though, go to Design Rules > Design Rules Menu and increase “Via Dia” and “Via Drill” values or else the holes will be too small for the jumpers to be soldered.
Good, I am doing my single-side PCBs with this via technique to emulate jumpers, but how can I workaround if I have 2 (or more) jumpers that should cross the same point? I mean, this technique uses the top metal as “manually placed” wired but. Can I have 2 (or more) top layers to workaround my problem?
You can have up to 32 copper layers.
go under [design rules]->[layer setup]
There is a drop down menu called copper layers.
You can even give them your own names.
Good, but how to change from B.Cu to In1.Cu using ‘v’ command? There is a way to do that?
I know of 2 options:
option 1 (quick and dirty):
place your via with “v” and [left click]
press “ESC” and choose your desired layer in the layers tap.
(The active layer is indicated with the blue triangle. to change this selection just left click on the layer name)
before you start your track you can select your layer pairing.
This can be found under “tools”->“layer pair”
You can also press V and then with + and - change the layer. It works in new canvas.
Hi. Just to add my thoughts.
If you are doing a professional single sided PCB with solder mask etc, vias are masked and so are un-solderable without cleaning the mask off first. My solution is to use a resistor body, or several for different lengths if needed, and edit the footprint. Delete the outline and draw a new line between the pads. Call it LK? in its reference field and 0R0 in its value. It is simple to construct a number of length links by moving the pads, and assigning the foot print as Link_4 say for 0.4". Link_5 for 0.5" etc.
If it is in a single signal path leave it as it is in the circuit but for ground lines or supply line it is easier to connect both ends to the same point, especially if there are many on the same net. This makes bug checking easier as otherwise the ground or supply line will be fragmented and will not be a single net.
This is a problem if you use connections to VDD VSS VCC GND etc by flags rather than by drawn connections. For example if the VDD supply needs a link to a pin and the link is shown on the circuit between the pin and the VDD flag, the end becomes a different net and the bug checker will throw an error that the pin is not connected to VDD.
If the link is connected at both ends to VDD this is not a problem, it just looks odd on the circuit. I have used a similar idea for cuttable tracks where the resistor is bridged by a thin track and cutting the track puts the resistor / capacitor / switch in circuit. Not cutting it leaves it bridged out. Can be useful for one -time address settings etc.
If the final circuit has to look better, save it as _V2 version and remove the parallel links. Issue that as the circuit, but keep the original for reference.
I have exactly the same issue. I have a double sided PCB with copper layers but on one side the copper layers is divided into several big parts due to some tracks. I was looking for a solution, hoping they have something like “jumper wire” in the library. I was thinking of just drawing some resistors but was looking for a neater solution. Your suggestion of using a transistor with 0R0 and then create your own footprint is exactly what I will be doing. Thanks for the suggestion.
These days, jumpers come in increasing choices…
“Zero” Ohm resistors are common, from (0.40mm x 0.20mm) to (6.35mm x 3.10mm)
but there are also larger SMD jumpers like