Hi guys. I’ve only been using KiCad for a few days and boy, am I impressed. It’s a thoroughly amazing piece of software compared to what I was using before, around 1990 vintage. Hats off to all who helped produce it.
I’m trying to produce a PCB with differing ground planes on both sides each having some isolated areas. I need to keep some of the signal ground lines on the board separated from absorption into the ground plane so I have to set them as a separate net. I basically have the zones working as I want with zone cutout areas working too. However, as soon as I set each plane to have a net, i.e. not as “no net”, they don’t fill and remain clear of copper and I can’t figure out why. That’s problem number 1.
In order to try out another apsect of zones I then removed all of the zone cutouts for simplicity. My intention was to try to connect between planes through the board with vias to join all areas together. I’m finding that, with both zones set as “no net” and the vias also as “no net”, the vias get swept around and isolated and don’t do their job of linking both ground planes. Is there a better strategy for this or am I missing something obvious which would make it work as I intended?
Probably the zone cannot reach a component pad of the same net. A zone needs to reach at least one pad to be considered non-isolated, and isolated copper fills with a net are removed by default. You can also disable the removal of isolated islands in the zone properties, but be sure this is actually what you want.
You will need to set the zones to the same net (not “no net”) and place vias that are also on that net. If you want two different nets (one on each side) you will need to use some kind of through-hole net tie footprint instead of a regular via if you want to link the two different nets together with “vias” – but if this is your intention, I have to say it is a very strange request, can you say more about why you want it?
Thanks for the good thoughts Craftyjon. Your first point seems to be fairly obvious to me now, it wasn’t something that occurred to me before. That’s always the way isn’t it? Things are always easy when someone who knows tells you how. I’ll try that out and report back.
As to the second point, I thought I had actually set up the net choices so the two zones and the vias were all on the same net. That seemed an obvious requirement. I think a simpler test layout for just these two points is called for.
Thanks again for the advice, it’s much appreciated. I’ll try these approaches and get back to you with the results.
You can have these tracks to have the same net as zone but surround them with area with forbidden zone filling (I’m not sure of names as I can’t run KiCad here to check).
I didn’t understood OPs as you did, but I am not English expert
– but if this is your intention, I have to say it is a very strange request, can you say more about why you want it?
I hadn’t anticipated that this would be considered “odd” . I was exploring the idea of tying up all isolated areas of both planes by linking them through the board into one single running ground area. It seemed kind of a natural way to do it, and “natural” is where I have gained my experience with PCB design rather than formal training. I’m really a circuit designer who has to also double in laying out the PCBs for the work I do in a small company. (In the country of the blind the one eyed man is king! )
I know I can exclude small isolated areas but when there are larger ones spread around which really should be included and which have no way of working tracks between them, this seemed to be a simple approach to me. How would you better PCB educated guys achieve this?
OK, I misunderstood you. If you want them all on the same net, you just can make a single zone, assign it to that net and to both layers, and then add a bunch of vias to stitch them together.
Ahhhh! A single zone? I hadn’t even thought of that. I assumed each side would have to be defined separately. So does that mean that it will be automatically differently shaped on each side but will still be effectively the “same zone”? If so that is where I am going wrong.
If you want to have copper filled on both sides but in the same net (like, a ground net for example) and across the same area in the XY plane (for example, across the entire board) you can draw a single zone and assign that zone to multiple layers (in its properties). The zone outline (the hatched border that you draw as a polygon) has to be the same on all layers, but then the actual copper that is created will be filled differently on each layer, depending on what other things exist that the zone has to keep clearance from.
Excellent! That seems to be just the ticket Craftyjon! That’s pretty much a description of what I want to achieve in a nutshell. Tickety boo and absolute mustard!!! (Apologies, the Brit in me is coming out now.)
I’ll give it a go as soon as I can but I really think you have pointed me to the solution I wanted. It may be pretty obvious with hindsight but that would have taken me a fair bit of time to come up with myself, if I ever did. Thanks to both of you for helping. I’ll be back with the results asap.
Additionally, Zones also keep their distance from the edge of a PCB automatically every time you let them regenerate their internal geometry with the b key. Unfortunately this clearance is set to zero by default. The setting is in: PCB Editor / File / Board Setup / Design Rules / Constraints / Copper to edge clearance.
Some people do not want to rely on the zones keeping their distance from the edge, but it is reliable in KiCad. Additionally, I draw the outline of the zone usually like a big pentagon around the PCB, because then it will be immediately clear when the zone fill does not work properly.
Thanks Paul. One of the worst things about a new piece of software is that you often know something is there having just used it but, you get that “where was it now?” and lose so much time trying to locate things you have already used. It’s all part of the joy of software I suppose!
Thanks to both of you, I did pick up on the “B” for regenerating the zones early on. I’m astounded how quickly it works over a fair sized PCB.
I’ve actually got a simple layout working exactly how I want it to now using the info you have all given. In particular Craftyjon’s instructions were spot on, (am I allowed to use the English “spot boIIock” here), and easy to follow. I’m flying from here on in. Problems solved and thanks to all.
For software I am planning to use I make my cheat-sheet in a form of spreadsheet.
For KiCad I have there tabs for all 4 applications I use containing menu hierarchy with comments were needed and important for me functions marked by green background color.
For example I recently read here about genius hotkey ‘P’ used after first time updating PCB from schematic and then selecting at schematic a block and using P at PCB (both windows opened and you have to have some setting set for focus going automatically with mouse between KiCad windows).
And separate tabs for:
what is my intended use of layers,
what are my limits in footprints (example - local mask clearance in 0.4mm raster footprints)
how to make 3D models with FreeCAD,
step by step from beginning schematic to production files with pointing important things (like this P) that can be forgotten,
and some others.
Me too.
Recently I have seen here at forum - there is currently some bug in zone filling. As I understood it will be fixed in 7.0.8.
. I was exploring the idea of tying up all isolated areas of both planes by linking them through the board into one single running ground area. It seemed kind of a natural way to do it, and “natural” is where I have gained my experience with PCB design rather than formal training. I’m really a circuit designer who has to also double in laying out the PCBs for the work I do in a small company. (In the country of the blind the one eyed man is king! 
)