I have problems creating a PCB with 0R bridges. I added the 0R bridges in
Pcbnew, not in Eeschema because they have no other use than to allow routing.
The net name for the pads had to be adjusted, otherwise it wasn’t possible to
connect the pads. This works until the PCB is updated from the schematic. Then
the net is changed and the connection breaks. How can I fix this so the 0R
resistors survive updating the PCB from the schematic?
KiCAD 5.1.6
Here is an example to illustrate the issue:
This is a horrible way of doing things.
The ratsnest line over your 0R resistor still wants it connected, which means you end up with DRC errors.
An easy and quick solution is to put those components on the schematic.
They do not have to look like resistors in the schematic. You can make a very small schematic symbol with just 2 pins next to each other.
You can probably go as far as also hiding all text for that schematic symbol and reduce the visuals to a piece of wire of a different color.
By having the 0 ohm resistor in the schematic in the same manner as you want it to be connected. After all the goal of a CAD system is to ensure the documentation (schematic) agrees with the product (the layout).
OK, fair enough.
I assumed a component only required as a routing artefact has no reason to be in the schematic. But I seem to be mistaken.
One more question: I added the 0R to the schematic, but both sides are in different nets. It that intended? Logically they are the same net.
And thanks for the quick response. Much appreciated.
Yes, of course this separates the net in 2 parts.
It’s the only way to keep the parts o the left and on the right sides of the vertical track without DRC errors.
For an example of representing these on the schematic, you can start with the “net tie” symbol.
Even with a net tie there will be two individual nets? The net tie is just an alternative symbol, right?
The idea of a net tie is to explicitly connect 2 “different” nets with a (small) piece of copper on the PCB.
One of it’s intended uses is for example when you have a high current track to a current shunt, and a sense line back to some measurement circuit.
Physically it is one net. All the copper is connected. but you want different track widths for the high current track and the sense line. And you want to connect those 2 at the current shunt, to avoid measuring voltage drop over the high current PCB track.
So you split the net in 2 sections in the schematic, and in Pcbnew you can assign different track widths to the 2 sections.
I just wanted to point out that Footprint assignment to schematic symbols is flexible. you can use any footprint for any schematic symbol. Even if it’s a physical resistor on the PCB does not mean it has to look like a resistor on the schematic.
Thanks for elaborating.
I tried to include 0R as net ties in the schematics. But now ERC throws an error. It works without the net ties. Here’s a quick example. What am I doing wrong?
You need the Power_flag at pin1 of U1.
Anyway it is not a connection error. See ErrType(3): Pin connected to some others pins but no pin to drive it
Your power flag is connected to the +5V signal, the other side of the net-tie is not the same net, therefore you have not power flag at the VCC of your component.
OK, then I’ll place a 2nd the power flag directly at the component’s pin if that’s the way to go. Thanks for your support.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
