technically i don’t see one.
How can I best approach this?
use vias and connect to bottom gnd, redesign the footprint with smaller pads, or use a pcb technology that enables you to connect between pads ($$).
Choice is yours.
btw, if you are using a castellated pad module and you want to mount it ‘smd style’ i don’t think placing plated holes on the pad is a good strategy.
Which is the isolated island? The one in the middle? If so - it’s connected via pin 2.
Either way I’d add some vias if you have GND zones underneath.
And you have 5V pin 1 not connected.
If you do not want the big ‘island’ under the foot print, you can add a ‘no-copper-zone’ there.
I feel daft not to mention what the isolated island is. Yes, it’s the big zone beneath the ESP32. May I ask why you say you’re not seeing the isolated island? The one below the ESP32 connects to the outer ground plane only through the 2 GND pin. I assumed that this is the reason DRC was complaining. DRC errors:
Now that I’m reading the errors again, I see that it’s not complaining about the isolated ground plane. It’s complaining about a minimum number of spokes count. Sorry for this. I’ve been trying different things and it toggles between these two errors. The isolated island error is there, but for a different place on the board:
I must say that I don’t understand the difference. For both I see a ground pad connected in two places, one to the (lets say) outer ground plane and one to an isolated one.
I have big THT holes for connecting the ESP32 because I want to keep my option open to use pins, maybe even removable pins. But yes, I want to solder them using the castellations. Here’s a picture of my previous version of the PCB:
It’s functional but I’m redesigning it because if I push the strength of the WiFi signal beyond 50% I get noise in the audio being recorded. (I’m making quite a few changes; the ground plane is just one of them.)
Long story short. I can switch to SMD pads and use the castellations to solder the chips. Then if I do have an isolated island, I can use vias to connect it in a second place, right? Or should I rather then use the bottom of my PCB as the ground plane and use vias everywhere to connect the GND pads to the ground plane?
(Sorry for the imgur links. The forum doesn’t allow me to embed more than one image.)
May I ask why you say you’re not seeing the isolated island?
as greg_m pointed out, the copper area is indeed connected (with 1 spoke per side) to gnd.
The DRC is complaining that just 1 of the minimum 2 spokes required per side is possible to draw.
Similar issue here today:
With castellated modules SMD mounted (or smd pads in general), if you plan to automate the manufacturing of the board is not good practice to have a open plated hole on the smd pad, it tends to ‘wick’ out the solder, leaving problematic joints.
For manual soldering of small batches there is no problem.
No, hand soldering. No more than 10 boards.
I’ve made a few changes. Ground plane is at both sides now, which allows me to use vias to connect up some islands. I’m designing two boards, and on the other board I could fix one min spokes DRC error by changing the angle of the spokes to 45 degrees (was in the linked post; thank you!). I fixed a few other ones by adding GND tracks. I did decide to remove the island below the ESP32. I don’t understand the trade offs to make a decision about e.g. clearance around the pads, and I did want to keep the THT holes for now.
Thanks for the help!
I agree with you. Both situations look the same.
Which version do you use? If V9 than you should expect it still being buggy.
I see one difference that can, may be explain DRC.
One error says that there is only one spoke while two are needed. The question is why KiCad sees one while we see two. It is possible that when this will be solved than DRC will report another Error - the same like in second case.
In second case I understand error as saying you have to have 2 spoke connections and you have two, but one connects to copper area that has no other connection so if not this one connection it will be isolated island. Such connection really not gives you two spoke connections to general GND zone.
I supposed that if pad has two spoke connections from which one goes to island DRC will be satisfied. I am surprised it is not. May be it is something new in DRC.
I have never had such situation and don’t expect will have. I’m using full/continuous GND at one side so all ‘islands’ at the other side have many via connections to this so they are not islands.
I’m using 9, so that may be the cause. I ended up switching the pins around to get rid of the island on the second print screen. I’m pretty happy with what I’ve ended up with.
Is it advisable to not use 9 yet?
Your footprint is all wrong. It makes perfect sense for modules such as this to have THT holes, because this is needed to create the cancellations on the perimeter of the PCB. But for soldering such a module onto a project, normally SMT pads are used. This is also much easier for you, as it keeps the whole backside (blue) side of the PCB empty.
GND planes are important in PCB design. flooding all unused areas with GND is not a good design practice, and it does not give the expected result. With some bad luck, areas of a GND plane that are only weakly coupled to the rest of the PCB can start to act as antennas, both for radiating and picking up noise.
For good design practice. Keep the whole bottom side of the PCB reserved for the GND plane (but do keep track of cutouts needed for antenna’s and such) and then put all tracks (Except GND, but including power) on the front side of the PCB. Any cutout in the GND plane should be as small as possible. Don’t put ANY long tracks though the GND plane, do not place rows of via’s in the GND pane, but spread the via’s around so the GND plane connects in between the via’s. Connect all SMT GND pads with via’s directly to the GND zone on the backside. If you want to know more theory behind this simple and practical rule, then I highly recommend to watch the “how to design a proper GND plane” video from Rick Hartley. It is 2 hours and 19 minutes long, but it’s worth watching. It’s an excellent reference on GND plane design, and it’s length is an ode to the importance of proper GND plane desing. It’s not a waste of time. (Rick Hartley is also a pleasant speaker to listen to. I guess he can make almost any subject appear to be interesting.
Edit / addition
You may want to revisit that statement after reading my post. You were less then a minute quicker then me in your last post.
Choice is yours. Reading KiCad forum you can see if people write about problems still existing in new version. Based on it you can decide how risky it is to move to new version. I don’t remember if first V8 version I have installed was 8.0.3 or 8.0.4. Fortunately now I’m not designing PCB for some time so don’t have to make decision.
I’d say “don’t scare off the newbies” but since I’m the newbie in question, I won’t.
I will take your advise and I will redesign the board according to your advise and what I learn from the video but I will not revisit my statement because I’m still happy what I’ve ended up with! It’s a lot better than what I had. Every step in the right direction is a good one 
!
depends on your ‘risk propension’.
I have even designed ‘production’ boards using nightlies 
some people around here is still on 7.x, sometimes somone drops in from 5.x.
Personally i could not use something prior to 8.x due to the lack of DBLibs, but you do you.
My example you can see here:
My strategy is to go with VCC under uC and then distribute from there through corners and VCC pads. That way VCC connections don’t block other signal connections. I am also using 0R from time to time.
Any advise for working with SMD components on both sides of the board? The second board I’m designing has that, although I realize now I can change that. I will. I’m just curious. Do you just accept that you’ll have holes in the ground plane, or does it force you to go to a board with inner layers?
that is inevitable even if you go with blind vias, and unless the plane becomes completely disconnected, is still better than no plane.
If you mount by hand smt both side is not a problem, (unles we are talking about 0201 and fine pitch bga) if you have good eyesight and steady hands.
It was not my intention to scare you away. I just wanted to give some advise about a direction towards a path you can use to improve your knowledge / design. It’s up to you what you do with it.
Single sided SMT placement is common. Especially when size constraints are not severe. When PCB’s become more dense, routing becomes exponentially more difficult, until at some point there is simply no physical room for routing the tracks, and you’re forced to go to multi layer. Single sided SMT placement is also easier to manufacture, so a slightly larger PCB can result in cheaper production.
Overall, having a bunch of SMT parts on the bottom is not such a problem for integrity of the GND plane. Especially if you keep them of 0603 size or smaller, and space them apart. It is however becoming more common to switch to a 4 layer PCB, because the increase of cost is offset by the time saved by the designer. Routing a project on 4 layers is a lot easier for the designer.
Even for DIY it makes assembly more difficult. For very simple projects, you can hand paste the pads with a syringe (there are projects for electric powered syringes that put out just enough paste for a single pad when you press a button or foot switch). But pasting with a cencil is much quicker. Single sided with a soldering stencil is easy, by taping some left over PCB pieces to a flat surface such as a table, and also taping the stencil into position. If you have parts on both sides, then you’d need a “stencil printer” which is mostly a mechanical device that can hold the PCB into place while the bottom of the PCB is not touched.
With parts on one side, you can solder a PCB on a hot plate, which is the easiest way to do the whole PCB in one go. With parts on both sides you need another soldering method. a modified toaster oven is popular, but just a heat gun is possible as well. A PCB with wet paste and SMT parts on both sides is also delicate to handle, and likely to result in more rework.
If you look here in your layout …
… it gets obvious that you can route between two pins. The same is true for a filled zone.
You have to reduce clearance for the front zone. I mostly use 0.2 mm, ask your PCB-manufacturer.
I gathered as much. You were just a bit blunt and direct, but all advise is greatly appreciated. I’m 30 minutes into the video and it helps a lot. I’m working with I2S so if I’m not mistaken, the signal is already into the MHz range so the things Rick’s saying about how the fields form absolutely apply. Thank you for your help.
