How can I make sure that the mask is not on the place where I want to solder pins to?
See photo
It looks like you are using vias as the connector. Share a screenshot of your pcb editor and schematic Also: what is your KiCad Version Info? Help > About KiCad > Copy Version Info.
Version Application: KiCad PCB Editor x64 on x64
Version: 8.0.0, release build
Libraries:
wxWidgets 3.2.4
FreeType 2.12.1
HarfBuzz 8.3.0
FontConfig 2.14.2
libcurl/8.5.0-DEV Schannel zlib/1.3
Platform: Windows 11 (build 22631), 64-bit editie, 64 bit, Little endian, wxMSW
Build Info:
Date: Feb 23 2024 02:24:15
wxWidgets: 3.2.4 (wchar_t,wx containers)
Boost: 1.83.0
OCC: 7.7.1
Curl: 8.5.0-DEV
ngspice: 42
Compiler: Visual C++ 1936 without C++ ABI
Build settings:
Are there any simple ways to change it instantly to the good connectors?
From the looks of it, you probably made this without a schematic.
All your via’s also have arrows from DRC violations on them.
In KiCad, working without a schematic is a bad idea. You will be fighting KiCad all the way to the end result, in a (false) attempt to save yourself 5 minutes of work.
To fix this, I would just start over from scratch, or maybe re-use the tracks.
Try this:
- Backup your project.
- Create a schematic, put a single row 32 pin header on it.
- Hover over the header, press [Ctrl + D] to duplicate it, press either X or Y to mirror the duplicate, and then put the pins on top of the first header.
- Select the header with a single mouse click, then drag it away from the other. KiCad will add 32 wires between the two connectors.
- Assign a 32 pin DIP socket to one connector, and a QFP footprint to the other.
- Schematic Editor / Tools / Update PCB from Schematic [F8] to put both the netlist and the footprints into the PCB Editor. (Just place them somewhere).
- Detelte the footprint that is already on the PCB.
- Draw a box from left to right over a row of via’s. Make sure the box is so narrow that none of the PCB tracks are fully enclosed, then delete the row.
- Draw a box from right to left over the other row of via’s. This time make sure that the via’s are only touched by a sliver of the box, and does not even reach the center of the via’s, as anything crossing the box boundary will also get selected. Then press [Del] to delete the other row of via’s.
- You could also have done this with the selection filter in the bottom right corner. Just uncheck all boxes except Vias.
- Move the DIP footprint to the right location.
- Move the QFP footprint to the right location.
Those steps would fix your project. If you have some experience with KiCad, you can do them all in 5 to 10 minutes, but if you’re still learning KiCad, it will take longer.
Next item on the list is the red rectangle. I assume this is the outline of the PCB, and the outside of the PCB is a very important feature of a PCB, and it has it’s own layer. You can select it, then press e to edit it’s properties, and then set the layer of it to Edge.Cuts.
Some other improvements:
A. Draw a copper zone on B.Cu, and attach it to GND (You can use test pin schematic symbols and footprint for the extra GND pins). You get the 2nd layer for free from nearly any PCB manufacturer, and having a GND plane is always good on any PCB.
B. Add some decoupling capacitors. Connect one side to GND, and leave the other open (Use the “No Connect” cross schematic symbol). Use a footprint of your choosing. (I prefer SMT either 0603 or 0805).
C. Update KiCad. V8.0.1 has been released a month ago. Increments in the third digit are bug fix releases, and in general they should always be installed. V8.0.2 is now in it’s testing phase, so it’s a bit (one or two weeks) to early for that. In general, a bug fix release is made about once a month.
4 Likes
@paulvdh has written a fantastic list of operations for you to follow 
here to help you visualise better are a couple of shots of a breakout board I made many years ago for the ATmega 328pAU
It is not the usual way to use vias as connectors.
Anyway, if you want to do your layout this way choose the desired MASK layer first (!) and then create an area in this layer. The silkscreen will be removed on all copper !
Modifying the current project in this way is slightly less work then what I proposed, but doing it “the proper way” has a lot more advantages.
- It’s not only about “getting this project fixed”, but also about learning how to use KiCad effectively.
- For the next project, doing it “the proper way” the first time is quicker (compare placing a single footprint, to aligning all those via’s).
- With a schematic (and thus a netlist) routing can be done much quicker. You can use x to start a track, and then immediately press f to finish the track to the nearest open pad of the same net.
- With a schematic (and netlist) DRC works properly, and this is a HUGE difference.
I did this on a project where I needed very small holes and pads.
(It was a 1 mm x 1mm LED matrix display).
I chose 0.15 mm vias with 0.3 mm pad.
Set track width to 0.15 mm and drew a circle with 0.075 mm radius on top and bottom mask. Quick and easy.
If I had to do it again, I’d probably define a suitable pad, but this was a one-off.
Couldn’t agree more, the first project I made with Kicad was a breakout board like the one I posted and I learned there and then a decent workflow is essential. I worked my way through the schematic then the board and then got 10 of them made and it felt good to have done that its a great starter project especially if your getting up to speed with MCUs.
Thank you for this, I will try this step by step.
I did all the steps except the GND pins, also I still have 1 fault when I do the DCR test. (See 3th picture attached). The fault is saying that 2 footprints overlap each other.
Yup, the smaller square footprint is inside the larger rectangular footprint, hence they overlap . . . I would ignore this error.
1 Like
I did thanks, now I wanted to make the PCB at PCBway but it says my drill layer is not showing up or something. How can I fix that the holes I made in Kicad are also shown in the gerber file?
Did you produce the Drill files ?
or here:
Thank you that was what I was looking for!
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.