Hi All,
I use a ground zone on the top layer of a 4-layer board.
For reasons of defined length/resitivity I need a bunch of complex ground tracks inside that ground zone and i would like to ask if there is a more convenient way to to that without the use of complex keepout zones.
Best Regards,
Paul
Without thinking about it too much . . . I think I’d use a different GND net for the complex ground tracks. The GND zone would flow around it . . .
You could use two different ground nets and tie them together with net-ties at one point.
At first it is hard to understand if you know that zone will simply cover all tracks being drawn inside zone.
You can replace complex keep-out zones with complex ground zone shape 
Margin layer also can help sometimes.
I am not sure what the intention is here.
In general it is not a good Idea to make complex shapes in a GND plane. You are also making a 4-layer PCB, and there is no law that states that all GND tracks should be on a GND layer if you have a GND layer.
Using net ties, as fox suggested may be a good choice, but then combine it with routing the tracks on another layer, so you keep a continuous GND plane. But it’s all pretty generic advise. If you want better advice, then first tell us more about your case.
I’d also be inclined to split into two grounds and use a net-tie.
But, it’s worth pointing out that if you do use keepouts, you can have KiCad build you one by selecting all the tracks, RMB > Create from Selection > Create Rule Area from Selection and select the “Create bounding hull” option with whatever clearance you want.
Can you a bit more specific than that? From where to where do this tracks go? Do you treat them as differential pairs and connect one signal on one end to GND?
How about routing them on a different layer than your GND layers. Maybe use a layer where you don’t make a GND filled zone but a VCC filled zone? (Do your ICs share a common VCC?) This way they have the defined length you want.
Thanks for all the Input. Net-ties seems the way to go.
I’m creating a circuit for meassuring low resistivity. So the tracks from the ADC need to be of identical resistance for compensation reasons. Therefore i want to route them both on the top layer avoiding any vias.
@JeffYoung Thanks for the hint with the Create Rule Area. Is this an KiCad 7 Feature? Haven’t seen it before.
I’m creating a circuit for meassuring low resistivity. So the tracks from the ADC need to be of identical resistance for compensation reasons.
But then, why use GND in the first place? Can’t you use a 4 wire measurement?
The current loop uses the GND on one end, but there the resistance of this wire doesn’t matter (as long as it is still a small impedance) and the voltage sense pins are not connected to GND, there the resistance also doesn’t matter (as long as it is still a small impedance) since only a very tiny amount of current flows through this wires.
I had to didn’t know that when created my GND zone:
Thanks for the hint with the Create Rule Area. Is this an KiCad 7 Feature? Haven’t seen it before.
Yes, I think it is. (Being able to offset the shape of the bounding hull by a specific distance might even be an 8.0 feature.)
The circuit is a little bit more complicated, but net-ties do the job pretty well.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
