I’m attempting to connect two different grounds together at a single point. I’ve done the method suggested elsewhere of creating a “jumper part” that is a mere two pads with copper between them, but I can’t seem to draw the copper between the pads. Kicad doesn’t allow me to draw on the copper layer in the footprint editor.
What is the current way of doing this?
You could add a third pin to your jumper, bridging the two pads you’ve already drawn. You can also draw a line of whatever desired thickness, then change its layer to F.Cu (and/or B.Cu if it’s a two-sided part). It’ll warn you about something something dangerous.
So, I’m currently just using two overlapping pads. Is adding a third pad between them going to get rid of the DRC error?
Probably not very helpful insight: proper support for this function is planned.
Work has started, see https://www.mail-archive.com/kicad-developers@lists.launchpad.net/msg19199.html
But that will wait until January at least: https://www.mail-archive.com/kicad-developers%40lists.launchpad.net/msg20198.html
Thanks! I’ll live with the DRC check now.
I do star grounding by braking up grounds into separate ground-legs that i connect via “0 ohm” resistors.
But to make things simpler, after im done with a board and before i make gerbers (last DRC check) i save that board then i replace all the 0ohm resistors with one footpint i made and that one is shorting resistor (quick and simple in my case i make SMD0402S which i modified version of SMD0402, so when i click on the resistor footprint i want to “replace footprint” i just add S in lower box at the and of footprint name and click to replace all of them (to make your life easyer I suggest that for this purpose you use a footprint that you do not use anywhere else in the design, so when prompetd to replace that footprint, it will replace only those footprints and not other ones that you would not want to replace).
Then i make gerbers, do not save the board when asked and close the PCB program.
That gives me have nice star ground but i have to repeat the proces every time i make a change and generate new gerbers…
It works fine untill better solution is introduced, even in schematic because i create separate node with bunch of these resistors on one spot there that is pretty self explanatory, and grounds are other labels share the same gnd just add numbers 8-).
The problem is if you run DRC AFTER you replace the resistors with jumpers, then error report propagate the error pointers up the trace which can be very annoying and misleading…so beware!
The 0R/jumper component solution doesn’t seem to work for me when connecting A and D ground planes together. Instead I place a copper fill with no-net affiliation overlapping the two planes I want connected. The no-net plane has a 0mm clearance.
This is the last step of the layout as after that the DRC is wonky. If I do need to do some work afterwards, I move the plane out of the way, make my changes, hit DRC until all is well and move the plane back in place. A bit tricky but not too nasty although a built-in feature for star point grounding would be far preferable of course.
1). Make a schematic symbol with 2 pins.
2). Switch to the Footprint Editor.
3). Make a Footprint with 2 SMD pads.
4). Draw a line on the silk screen between the 2 pads.
5). Right Mouse Button and change the layer of the line to the right copper layer.
This is quite dirty hack because PcbNew does not know about lines on the copper layer and it can not use it for DRC checkecking. This problem can be mitigated a bit by placing the 2 smd pads close together.
You also have to adjust the solder mask etc of the pads.
More info with screenshot & link to a youtube video/tutorial below.
I know there might be a good reason to create a star ground in your specific case (none of you have stated why you want to use a star ground design), but in most designs it is better to have an uninterrupted ground plane.
(Best option is to have one layer only for the ground plane. Would require at least a 4 layer board though.)
A uninterupted plane makes it a lot easier to ensure the current return path with the lowest impedance. (lowest area between signal and signal return path.) As soon as there is an interruption in your plane you need to ensure that no signal trace ever crosses this interruption.
For more details have a look at this post over at the contextual electronic forum. (Yes it is a bit simplified but it is still a good introduction.)
@Rene_Poschl: Star point grounding (SPG) is used for mix digital and analog designs. Additionally, designs where safety ground, signal ground/shielding and instrumentation ground all can be polluted differently (long cables, nearby radiators etc.) you need to use a SPG.
The reference you provided is interesting but only concerns itself with digital only signals. For mixed designs, in particular with analog circuitry that handles a large dynamic range (e.g. 24bit ADC) one must use a SPD (or have very quiet digital logic 
). Take a look at some of the Power Modules out there that provide buck converters and LDO’s all in one chip - buck converter for the rough digital stuff, LDO for all that needs to be quiet. Each with their own ground/return.
Disclaimer: Everything below is very simplified. There are lots of books out there that handle this stuff in detail. (Sadly i don’t know good books in english. I learned this stuff in german)
For mixed signals it is especially important to be careful when splitting the plane. You have digital signals crossing over from the analog plane to the digital plane. Which creates quite efficient slot antennas if you are not careful.
Just assume the right ic in the following scetch is your analog ic and the left ic is your uc. The signal might be the clock of a bus (example i2c) which means it is for sure > 10kHz (for signal > 10kHz the return current wants to flow below the normal current.)
In this case we already create a slot antenna.
One can place capacitors to give the current a path back that does not require it to flow around this slot, but why even break up the plane? (If one breaks up the GND plane, one should connect the two planes via a ferrit bead and not directly via copper) In most applications there is no real benefit.
It does not matter where the main supply connector is placed here. The return current always flows back to the ic that send out the signal.
@Rene_Poschl
I think you have a bit of tunnel vision here.
You are looking at star / plane from a digital designer point of view.
With the picture of the long signal return path you also create a false / incomplete image.
Considerations here without also adding the decoupling caps in the equation are at the least useless, or even worse, misleading.
The “Signal Return Path” should be near DC and mosty irrelevant.
From an analog designers point of view the situation can also be quite different.
Take for example and audio power amplifier.
The last power stage can handle high currents. Peak currents of 10A or bigger are no exception. On the same pcb you also have delicate / sensitive input stages and intermediate power stages (100mA base current to the power transistors?)
In a digital design you want big planes to make the overal impedance low and planes are very good there. In a digital design noise in the ground plane also is irrelevant as long as it is below a certain treshold. The influence of 50mV noise means very little to 3V3 logic.
In the power amplifier a lot of the intermeadiate stages are fed from a constant current supply and a little voltagedrop over a pcb trace is completely irrelavant, but fast transients may be coupled into the signal and therefore you want to make very sure that all the different stages do not pick up any noise from the other stages. Therefore everything is referenced from a single star point and from that point the whole GND net is split into individual traces as fast as possible.
This technique is also very common in SMPS circuits. The PCB layout must be carefully designed to avoid any of the big switching transients being coupled back into the voltage sense feedback circuit.
Reference: http://cache.freescale.com/files/microcontrollers/doc/app_note/AN3898.pdf
