Joining upper and lower copper zones

Layout
1

Hi All,

I have two layers board as shown below

Screenshot 2024-11-12 at 6.20.43 PM
Screenshot 2024-11-12 at 6.20.43 PM1049Ă—1072 145 KB

I created a ground zones on the upper and lower copper layers. it works great.

I see that there is an island with no copper filling in the middle. I highlight it in green.
is there a way to connect the red area with the upper area to avoid this empty island ?

2

Simply place vias in the empty space. They will connect to GND and lead to copper zones on the other side. So you can e.g. connect the upper red zone to the lower one. This would give smaller loop areas and lower EMI. With respect to EMI, I would also suggest to reduce the clearance of the pours such that they create copper between the IC pins.

3

I did add via and re-fill and it started to create copper on the other side. Many thanks.

regarding the clearance, I have to keep it like this because of my poor soldiering skills :frowning:

4

If you get your board properly manufactured (with appropriate solder resist), don’t care about it. If you etch or mill it manually, you’re right. I am no Old Surehand myself but I never had trouble soldering. Trust in yourself!

5

when you say “appropriate solder resist” you mean the soldermask ?
I manufacture my boards in JLCPCB in china. would that count as good quality boards?

6

Adding stitching via’s is not the proper way to do this. The proper way is to put all the tracks on a single layer, and reserve the other layer for the GND plane. Only when the PCB becomes too dense using stitching via’s becomes a last resort. Your PCB looks like it’s made with freerouter, or at least by just drawing the tracks without paying any regard to proper track layout. It’s a big mess at the moment and needs cleanup. It is OK to use vias in tracks to create “hop overs” to get past crossing tracks. You already did this at least once in:
image

With an PCB that is as easy as this, it is also quite easy to reserve one full layer for a GND plane. Randomly placing some via’s to get copper to fill more area’s of the PCB does not make a proper GND plane.

Some other remarks:

  • The default TO-92 is a nuisance to solder (or home etch) But KiCad also has some TO-92 footprints in which the pads are spread more apart. Those are much more fit for DIY projects.
  • You can easily make rectangles of zone edges by drawing them on a coarse grid.
  • Draw the PCB outline on the Edge.Cuts layer. This is pretty much mandatory before you order a PCB. KiCad’s 3D viewer also can not show the PCB properly without a valid outline on Edge.Cuts.
  • When you have a proper Edge.Cuts, you can draw the zone outline as something irregular. KiCad will then clip it at the edge of the PCB, and it will keep a clearance that can be defined in: PCB Editor / File / Board Setup / Design Rules / Constraints / Copper to edge clearance
1 Like
7

Thx Thx for the hints.

Highly appreciated.

I am using freerouter since it is a hobby project and long time is required to finish this job. I don’t know if there exists better routing applications. do you know ?

I also don’t want to use cracked Altium Designer for routing so I stick with what is free.

8

It’s a simple board.
You could hand-route it in an hour or so.

9

You have it between your ears.