First Design with KiCad (8.0)

RE: First Design with KiCad (8.0)

Andrew J — Wed, 04 Sep 2024 10:43:23 GMT

I started with v5 and the frustrations you felt were the same as mine, particularly the drawing tools. Trying to create an edge cut for a DB-9 (or whatever the letter is) was the Devil’s own job to get a neat curve that actually joined up and didn’t flag board errors. At the time the on-line help was typically YouTube videos for earlier versions and I think v5 was a major interface change so there was a lot of translating. What I’ve found is that over the versions I’ve worked out what works for me and then I, essentially, started again with libraries, footprints, paths, settings etc. I didn’t have to struggle with coming from a different CAD software though, as KiCad was the first I used. There’s some good tips in here: the only one I would add is that you MUST check library parts, esp. footprints. I’ve found that there are often errors and it occurs in a high percentage - say circa 30% of parts. At least creating symbols and footprints is easy.

RE: First Design with KiCad (8.0)

Jan Cumps — Mon, 02 Sep 2024 12:01:28 GMT

For the Vias, you can use "create array from selection". This is useful if you want to place a decent set of vias.

put one via
select it, then right-click -> create from selection -> create array

RE: First Design with KiCad (8.0)

shabaz — Mon, 02 Sep 2024 02:48:16 GMT

Hi Michael,

I was going to point you toward my 50-minute quick-start video https://www.youtube.com/watch?v=5Be7XOMmPQE , but from that PCB screenshot is seems you don't need it. But maybe worth scanning bits of it (e.g. from the contents list there) in case there's anything you spot that you've not tried yet. It is for version 6 but the UI has not changed significantly in version 8. Version 8 has some extra features of course.

Nice idea to make the board TO-3 shaped! I found KiCad to be a bit weak in the area of making curved board outlines (i.e. Edge.Cuts layer) like that, it is harder sometimes than it ought to be.

Regarding the Board Setup, a neat thing is that now for all future projects, you can import the settings; there is a place to click that at the bottom of the Board Setup window.

Regarding grids, the single most useful thing is to go to Preferences->Preferences and under PCB Editor->Origins&Axes,ensure that the Display Origin is set to Drill/place file origin. I have no idea why it should ever be set to anything else, but I believe the default is something different.

Once that preference is set up, each time I create a new board, what I do is go to Place->Drill/Place File Origin, and then click on (say) the bottom-left position of where I want my board corner, or, for symmetrical boards, I may click on the center of the board. It is effectively my "board origin". Now the X and Y co-ordinates displayed at the bottom of the screen will start from that origin point, and that's handy when positioning connectors etc., since I can precisely type the co-ordinates for them.

The next very key thing is to go to Place->Grid Origin and then click on the same exact location where you put your Drill/Place File Origin. If you don't do that, then things get crazy when changing grids, because they won't align with your board origin (i.e. the Drill/Place File Origin).

Now that that is sorted, when laying down copper using the X button, you can set the copper to snap to the grid at any angle, by going to Route->Interactive Router Settings and enabling Highlight collisions->Free angle mode.

It's a bit tedious, but if say you want the initial leg of copper to be at precisely 90 degrees (e.g. so it comes off an IC pad squarely) for a short distance, and then have the complete free angle, then the only method I know is to start off with the Free angle mode box unchecked in the Interactive Router Settings, and draw the first part of the trace, which will inevitably have the 90 degree line followed by a 45-degree line often. Once the mouse left-button has been clicked to place those two lines, then hit ESC twice to exit the trace drawing mode, and then click on the unwanted 45-degree like, press DEL to delete it, then, hover over the end of the 90-degree trace, press X again and hopefully it will connect to the end, and then right-click the mouse and in the pop-up menu, select Interactive Router Settings, and then enable Free angle mode. Now you can continue the trace, drawing at any angle.
The 45-degree mode does have an advantage in that the 'Shove' mode can be selected in the Interactive Router Settings, which might be useful when trying to route wires close to each other. Personally I don't use the Shove mode often, but it's interesting to try it out in case the need arises.

The many ground pins stacked on each other thing is really bizarre to me too. I don't use that technique in my own component symbols.

RE: First Design with KiCad (8.0)

battlecoder — Sun, 01 Sep 2024 21:33:51 GMT

Thanks for sharing your experience with KiCad. I experienced something similar when I switched from my previous software (Eagle) to KiCad, but it gets easier with time.

Btw, I can 100% relate to this:
"I don’t like the manual routing - the software still keeps trying to coerce the track into silly shapes."

Some tools that I've found that help with this: With / you can toggle between a couple of "approaches" to the track you are drawing, although it's a "posture" change and will not change the angle or the track at all, especially with shorter segments. With Ctrl+/ you can switch between 90° corners, arc corners, and 45° corners while you are routing, so you can switch at every segment to a different approach to get what you want. Finally, once you are done with the track and it goes approximately where you want it, you can use G to drag any point from the track without angle restrictions.

I'm by no means an expert, and there might be a better way of doing arbitrary angles or getting a better manual routing out of KiCad. But that's what I've used in the past. If you are following a book (which btw is something I should've done when I switched to KiCad) they might have better suggestions than this.

RE: First Design with KiCad (8.0)

DAB — Sun, 01 Sep 2024 18:46:01 GMT

Nice blog on your experience.

I took a quick look at KiCad several years ago, but I just do not design PC boards, so it was not something I wanted to invest any time learning.

I look forward to your future blogs as you do the next round of learning.

RE: First Design with KiCad (8.0)

genebren — Sun, 01 Sep 2024 15:30:41 GMT

Great intro to KiCad blog! I started to learn KiCad when I lost my license to Eagle during a hard-drive swap (license locked to the hard-drive). I imported most of a design from Eagle which went pretty smoothly, but I was crawling through the learning process, doing a lot of stumbling. I gave up when I realized that the vast majority of my designs (likely more that 100 PCB) were such that they would work with the Eagle Freeware version, so I just switched back to eagle and left KiCad behind. Is that going to be the end of story for KiCad, nut likely, but if I do try again, I'll do when I am not up against deadlines.

Thanks for sharing your journey!