I am following a course in Udemy about how to use KiCad and I am starting to get familiar with the pcbnew, the problem is that I am currently unable to make work the copper fill zones. I’ve attached the issue in a link to show more graphically my situation.
The circuit is very simple. I am trying to do a copper fill zone for +5v in my circuit and there is only one wire that is related to this fill zone, but the software is not showing me the copper field and is also unavailable when I look the 3D viewer.
I can’t see the left-hand tool bar in your screen capture anigif, but it looks to me like you have “Do not show filled areas in zones” turned on. Instead you want “Show filled areas in zones” turned on. On the left-hand tool bar you should see these three icons:
The active one is highlighted in blue, in my screen shot I have the top one active and that is the one you want. It looks like you have the middle one active.
I dont know if this fits your situation:
In the beginning I had difficulties with fill zones that would never fill though definition and priority and surroundings were OK.
I read that zones must touch related tracks or pads - but still they would not fill.
Finally I recognised that the zone must touch a REFERENCE point of another Element not just its outline.
I enlarged the zones to include at least one track or pad nearly completely and everything was fine.
I checked the project from your link and the issue is the terminal block you have added that is not in the schematic and therefore it’s pads are not assigned nets. Because you connected no net pad to 5v pad it creates a conflict that the zone does not know how to deal with. To fix this you can
remove terminal block
add terminal block to schematic
assign 5v net to the pad 2 of terminal block manually in pad properties
Either of these will fix the zone, I recommend adding all your components to schematic (at least ones with electrical connections).
Ok, I found the problem with your LED Resistor board. You forced something that broke the zone filling algorithm. Obviously, you placed the terminal block manually on the PCB since it doesn’t exist on the schematic. Then you set the interactive router to “Highlight collisions” and turned on “Allow DRC violations”. Otherwise KiCad wouldn’t have let you connect the terminal block pin that has no net to any other pin that does have a net. You then started drawing the trace from the terminal to the resistor. When drawing traces, what is drawn inherits the net from where you started drawing. In this case, a pin. Then when you finished the trace over the resistor’s pin that has the “+ 5V” net, the end of the trace covered the attachment point of the pad. This keeps the fill from attaching to the pin.
There are a couple of different ways of avoiding this issue:
Put the connector on the schematic and attach the connector pins to their appropriate nets.
If you don’t want the connector on the schematic and insist on placing the connector manually on the PCB, select the pins of the connector and assign them to the (pre-existing) nets.
If you really don’t want to do any of the above and insist on routing with “Allow DRC violations” on (this is like tight rope walking without a net), get in the habit of starting to draw traces from pins that have nets assigned.
I was able to confirm all of the above (and experiment to verify my suggestions) using the same version as you, 5.1.6. This is the current latest stable version, so there is nothing to upgrade to at the moment.
I would NOT suggest using the 5.99 nightlies for any real work. These are development builds for the devs and any volunteers to play with to test out new features. Some features may stay and others may be found a bad idea and dropped. It is expected that the nightlies have bugs. It is also known that the current 5.99 nightlies save files that cannot be opened in 5.1.6 as some of the new file format features are being implemented. I wouldn’t even trust 100% that something saved in tonight’s (or last week’s) 5.99 nightly build will be able to be opened in next week’s (or next month’s) 5.99 nightly build. The file format may evolve over time as bugs are found and squashed.
Wow, I totally get it. After doing it, it is more obvious why there is an issue in the copper fill zone generation.
I think that getting familiar with this tool is also getting into this kind of “bugs” because that way you understand better how everything works and what is the workflow.
I will have in mind to keep connections of terminals in the schematic to avoid issues in pcbnew. That is the most important tip of this thread.
Thank you so much to all the people who helped with this issue.
Google keywords: Peter Dalmaris , KiCad like a Pro second Edition , Udemy , Course
(I add this so that hopefully other course users of the following course will find this topic faster via Google).
FYI. This example from topic starter is coming from the 17 hours (Udemy) Video course “Kicad like a Pro” of Peter Dalmaris.
I also ran into this issue. In the Udemy course in section 39 Peter is adding the terminal block in the PCB directly. I do not know why he is doing this (maybe to show that it is possible to add adhoc components). This is causing issues in section 42 (copper fill as showed by topic starter). I am not sure what the whole idea is of showing this because in KiCad 5.1 this is suddenly more difficult. It requires selecting the legacy mode, turn off DRC. Then drawing the lines ‘are difficult’ (there also seems to be some rendering bugs in KiCad around this e.g. if you do the first mouse click, then this looks like the second point).
For the rest this is a relatively OK course for USD 10. It starts a bit slow with this LED/resistor starter, and later a more real world project around a breadboard supply. The information outlines that the course is upgraded to 5.1, but the actual recordings are in 5 so that is a bit misleading info.
I’m the author of KiCad Like a Pro and the course instructor.
After looking at this lecture again (section 39), I now see what is happening.
Specifically in relation to the screw terminal, before I add it to the PCB, I do say that this is not the right way to do it. I inserted a new footprint “ad-hock”, without adding it to the schematic, and after turning off the design rules checker.
I did this to demonstrate a few KiCad features:
How to drop a footprint on the PCB.
What is the role of the DRC.
That PCBNew and Eeschema are really two seperate programs.
I should probably emphasise that this is now how to do things, and that this is simply a warm-up exercise that makes it possible to demonstrate many KiCad features, quickly.
Would you recommend something else?
For anyone reading this, please note that there are 3 additional project of increasing difficulty that demonstrate proper PCB design process and principles.
The one discussed here is like a “Hello World” program. Quick to write and demonstrate that it works, but you would probably not want to write your next “proper” program base on this.
Hey there, I know this is coming kind of late. Another way of filling the zone with copper is for you to select modern toolset (fallback) option. This can be found on the preference tab. Once this is enable, then your filled zone can work properly.
Filling doesn’t depend on the accelerated(default)/fallback. If something behaves differently between accelerated and fallback, sans small visual differences, it’s a bug.
