You can right click on an error in DRC and choose Exclude this violation and it won’t complain about that particular problem any more.
Or you can go (in the PCB editor) File → Board setup → Violation Severity and make Thermal relief connection to zone incomplete a “warning” (and it’ll tell you about thermal reliefs but not call it an error) or “ignore” (and it won’t say a word about thermal reliefs).
If you create new projects from a custom template — for instance I have a template for Kosmo modules — you can change the Board setup in the template and then it’ll have that setting for all future PCBs you make from that template.
I have it set to “warning” because I figure it’s best to try to fix it if I can, but any I can’t fix I just exclude.
I also have silkscreen errors set to “ignore” because I don’t want to hear about them until I’m close to done with the layout. Then I set them to “warning” and proceed to fix them.
1 Like
Thanks. I too have a ton of silkscreen-related notifications that I just scroll past. Good to know that there’s a way to ignore them.
I have a circuit-related question: I see in the schematic that the frequency selection potentiometer (RV1) which is B50K, is designed to cover a frequency range between 1kHz to 11kHz.
What component needs to change in order for it to go down to 20Hz?
When I have courtyard issues i tend to edit this specific instance of that component to remove the courtyard itself (i prefer courtyard violations to ring alarm bells). Your PCB project basically embeds a copy of every single footprint you use, so it’s possible to make one-off customizations.
(If you look up the .sch and .pcb files in a text editor, they’re basically Lisp dialects - that makes it easy to process them automatically, or with search and replace! I sometimes do it to use my signature font family on the PCB)
Looking through the project:
first, without the .sch, it’s impossible to run the full DRC, but none of the errors i saw matter.
The 10µF caps use a 8mm footprint, much bigger than necessary, though better to have a bigger than necessary footprint than the other way around. It’s easy to find 5mm ones rated 50V, a prime candidate to shrink if it’s necessary to reclaim space!
You’ll probably want to either move the reference designators somewhere readable or remove them altogether. Leaving silkscreen that clips the copper is harmless (the fab will clean it up for you) but we be aware that when you have silkscreen like this:
One you send it to print it will actually look like this:
Anyway this is looking great, from no prior experience to a module very likely to work in two weeks 
1 Like
Check your pots to make sure of their orientation. It’s a bit of a mess because with some footprints pin 1 is the counterclockwise end and with others it’s the clockwise end. I always use one of the former kind. Then usually for an attenuator ground or the lower voltage connecting to pin1 is what you want, but for a variable resistor it, uh, varies. (In an op amp feedback path higher resistance means higher gain, at an op amp inverting input higher resistance means lower gain.) So you have to think about it to figure out which way around makes more sense, and inevitably you get it wrong once in a while.
1 Like
It’s all thanks to you two! Plus I can’t say that I really know what I’m doing yet. Especially in the schematic domain. But it’s a real privilege to know people who are so generous with their time and energy to help out a newbie.
I saved the silkscreen concerns for last (might delete all designators and just generate an interactive BOM)
If the board seems fine as it is, I guess that the next step would be to design a panel.
What’s a good way to do so, getting the holes aligned to the components etc.?
I just copied over the footprint from the original design’s interactive BOM. But I’ll see if I can confirm it just in case. Thanks.
