Hello!
I would like to create small GND plane close to boost converter. It shouldn’t be connected to big GND top plane, but should be connected using vias to internal GND plane.
How can I do it?
When I create small plane with the same signal it is connected to top GND plane. When I create separated signal (GND1) then I can’t make add viad properly…
Regards!
Teo
The internal Gnd plane needs to be the same name as the small Gnd plane.
If lines at Margin layer could have defined for what layer they define margin…
I think using narrow Rule areas you can define walls around your small GND.
I have no practice with net-tie. May be it is possible to have this small GND being GND1 and close to the same size net-tie placed on it may be will allow to place GND vias there connecting to internal GND layer.
See Below Screenshots
Not True!
RESULT’s You can see the inner GND-Plane below the Outer GND-Plane and the connected Via
ADDED Screenshot showing Different Nets
I understood this ‘internal’ as ‘internal layer’.
Ok.
Do I correctly understood what you said:
You can connect (with vias) copper with different net names provided that you will not refill zones since that moment.
Correct?
If yes then from my point of view it is not a good solution.
Yes, you understood correctly.
But, user’s can right-click a Zone and select to fill it so, other Zones can be filled as needed. Just don’t want to blindly/automatically fill all Zones.
It may not be a solution/approach for your but, it is for me and perhaps other’s…
ADDED: Oh, if you fill Zones as needed or automatically, you can Right-Click and ‘Unfill the selected Zones’
It is not a good idea to rely on any solution that has “don’t forget to never refill zones again” as part of it.
Any proper design should be able to blindly fill all zones at any time, and get the correct result.
If you want to connect two different nets in this way, you should use a net tie footprint.
If you want to have an outer and inner zone on the same net but isolated (meaning, connected on a different layer, because they can’t be electrically isolated or else it won’t pass DRC), you probably don’t even need two different zone objects. You just need to draw keepouts around the area you want to isolate. You can draw these with lines and then use Create from Selection to create the keepouts.
Step 1: Single Zone object, set to fill on multiple layers:
Step 2: Draw a Rule Area (set to keep out copper fill) on the outside of the area you want to isolate
Step 3: With the rule area selected, right click at the point you want to start the inner cutout (to set the width of the isolation barrier) and choose Zones > Add Zone Cutout
Now fill zones:
Note: you need to either have pads or vias on both sides of the cutout connecting together on another layer, or else there will be DRC errors and/or the zone will not completely fill.
Possibly similar to what I do for crystals?
The plane under the crystals is GND1, and there are three net ties between GND and GND1.
The GND1 is connected to the nearest GND pin of the micro, along with its decoupling cap on the bottom side.
It’s all done with net ties in the schematic:
I have never used net-ties.
At the schematic I see 2 of them (you write three).
What are these vias at GND1. Do there are other GND1 zone?
This is exacly what I need! Thank you 
I can’t use net tie because then it is not possible to make stitching.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
