At the risk of incurring the wrath of the moderators, I have some fabrication questions that are not exactly “how to use KiCad” related. However, there is a wealth of experience and knowledge in the KiCad community that would greatly benefit newbies using KiCad to create their first pcbs. So, I through myself on your mercy and ask that you let the forum experts answer my questions.
The KiCad default for min hole size is 0.5 mm. PCBWay offers 0.15, 0.2, 0.25, 0.3, 0.8, 1.0 mm options. What should I use? I ran into an error in the DRC for the pcb as I am using a vertical microUSB connector on the board, and the holes in the footprint are 0.4444 and KiCad complained.
What are some good rules of thumb for all of the options presented by PCBWay? I am a bit overwhelmed by all the choices. The fastest signal on my board is the 2.34 MHz clock for an SPI interface to a Raspberry Pi. The rest is just switching some high current lines with relays.
I am considering PCBWay to make my 4 layer board. Any pros or cons I should be aware of? Are there other manufacturers that you have used that you prefer?
Was hindert dich daran die KiCad-Leiterplattenregeln so einzustellen wie du diese für richtig siehst? Die 500 µm ist nur der Standardwert. Generell gilt: Je kleiner der Minimaldurchmesser je teurer und schwieriger ein Hersteller zu finden der deine Leiterplatte herstellen kann. Wenn du die Minimalgrösse auf PCBWay umstellst ändert sich möglicherweise der Preis. Ein kleinerer Minimaldurchmesser bedeutet das es eventuell einfacher ist die Leiterplatte zu entflechten oder macht dieses vielleicht erst möglich.
I ran into an error in the DRC for the pcb as I am using a vertical microUSB connector on the board, and the holes in the footprint are 0.4444 and KiCad complained.
Dann musst du den Minimaldurchmesser wohl auf etwa 301 µm - 440 µm verkleinern und 300 µm bei PCBWay wählen (oder einfach der nächst kleinere als in den KiCad-Leiterplattenregeln).
The fastest signal on my board is the 2.34 MHz clock for an SPI interface to a Raspberry Pi.
Ich glaube du verwechselst die Datenrate mit der Signalfrequenz (nicht sicher was das Korrekte Fachwort ist, auch nicht im englischen). Der Clock ist 2.34 MHz, aber das ist ein Rechtecksignal und hat deswegen noch Oberwellen die > 100 MHz sein können. Relevant ist die Flankensteilheit und nicht die Datenrate.
Hast du bei jeder Signalleiterbahn eine nahegelegene Rückleitung? (Entweder durch eine Massefläche unten, oben oder nebenan oder eine Leiterbahn und durch Durchkontaktierung).
The rest is just switching some high current lines with relays.
Hast du Freilaufdioden eingebaut? Was meinst du mit »high current«? Wieviel in Ampere?
I am considering PCBWay to make my 4 layer board
4 Kupferlagen ist natürlich teurer als 2 Kupferlagen. Eventuell könntest du es mit 2 Lagen schaffen. Wie komplex ist die Leiterplatte und wie gross darf sie sein?
What prevents you from adjusting the KICAD conductor record rules as you see them right? The 500 µm is only the standard value. In general, the smaller the minimal diameter the more expensive and difficult to find a manufacturer that can make your circuit board. If you convert the minimum size to PCBway, the price may change. A smaller minimal diameter means that it may be easier to unklown the circuit board or maybe make it possible.
I ran into error in the DRC for the pcb as i am using a vertical microUSB connector on the board, and the holes in the footprint are 0.4444 and kicad complained.
Then you have to reduce the minimum diameter to about 301 µm - 440 µm and choose 300 µm for PCBway (or simply the next one smaller than in the Kicad conductor plate rules).
The Fastest Signal on My Board is the 2.34 MHz Clock for an Spi Interface to a Raspberry Pi.
I think you confuse the data rate with the signal frequency (not sure what the correct technical word is, also not in English). The clock is 2.34 MHz, but this is a rectangular signal and therefore still has upper waves that can be> 100 MHz. The flanking and not the data rate is relevant.
Do you have a nearby return line with every signal conductor track? (Either through a mass surface below, top or next door or a conductor track and through the overtacting).
The rest is just switching some high current lines with relays.
Did you install free -running diodes? What do you mean by “High Current”? How much in ampere?
I at Considering PCBway to make my 4 layer board
4 copper layers is of course more expensive than 2 copper layers. You could possibly make it with 2 layers. How complex is the circuit board and how big can it be?
Nothing prevents me from changing the KiCad default except lack of experience regarding pcb design. I changed it to 0.3 mm and the DRC signed off on the design.
I understand the issue of upper frequency harmonics. What I meant is that there are only 2 traces with the SPI clock for two chips. There is no high speed switching on the board. And yes, the relays all have fly back diodes (thanks for the heads up). The current is 1-4 A for around 100 msec - 500 msec. Basically, the board is used to ignite rocket motors remotely.
I tried with just 2 layers and the layout was too big. I went to four layers and the board is 145 mm x 108 mm with 116 parts, 365 pads and 29 vias. Again, my first pcb design, so probably could use a lot of improvement. The 40 pin connector is for a Raspberry Pi that sits over the two chips under the connector. The screw block connectors are for external LEDs and switches. It could be a lot smaller with SMDs, but I am really bad at soldering SMD by hand. lol
PCBWay has defaults for all the pcb options (se picture above). Do I adjust KiCad options to match, or are there options I should adjust on the PCBWay side. I just don’t have the experience to make those selections.
BTW, in another forum, it was recommended to use JLCPCB, and their price is about 1/2 of PCBWay’s price ($48.36 vs $104.88) with a few days faster delivery. Again, a set of options for the board that I have to choose, and I don’t really know which ones I should choose.
I have done quite a few boards with pcbway and liked the quality, but price seemed to creep up a few years ago. Then I found jlcpcb and they have been great. You can request a production check (forget what the call it) which pauses production until you approve. For the pcb this lets you look at their version of the gerbers (and they do get changed when the layout gets tight). For assembly you really must check this so you can approve part rotation.
I realize you are doing a through-hole design here but you can someday go smt and spec jlcpcb parts for many of the parts and have them assemble a bunch of it for cheap. Then you just solder on the connectors and special bits jlc didn’t have and Bob’s your uncle.
Four layer is not that much more expensive than 2, and really speeds up your design and gives you a much better board in regards to power distribution, EMI/EMC…
Nice job on the rocket launcher. I did one when I was a cub scout leader years ago that fired six rockets together or sequentially, with a 3" red 7-segment display for a countdown. We launched at night and had flashing nosecones to find them.
This is my current Board Setup – note 0.3mm is smallest hole which works well with a 0.6mm via and gives an annular ring of 0.15mm. This is a nice minimum for a cost-effective board. I have gone down to smaller stuff when needed but the boards can get more expensive.
I’m working with PCBWay for more than 7 years and never had an issue with them. The quality is good and the price si decent. To optimize the price you can use for via a minimum hole of 0.3mm with a ring of 0.6mm and 6/6 mils minimum track and clearance, on silkscreen I use 20x20mils characters for designators with 4mils thickness and HASL if is manual soldered and prototype (modify the KiCAD constrains accordingly). More than that as general track width I use 6mils, 8mils, 10mils, 12mils, 24mils, 50mils as bigger as possible where it fits if you don’t need a specific impedance.
nothing special with your PCB so the setting you’ve captured are ok.
PCBWay should be fine; they will told you after auditing if it’s something wrong with your board. I sent them Gerbers (see details here: Generate Gerber file from Kicad - Help Center - PCBway) but they also have a plugin now to extract the files they need (I prefer gerbers).
I have never used uvias so no idea what that does. Also never used net classes, as I sizes traces an vias as I go from the drop-down menus. Here is a constraints snip that I used when I dropped Min-Track-Width to 0.125mm (my normal min is 0.2) and min hole size to 0.2mm (my normal min is 0.3) which is no problem for jlc and I don’t think it even cost extra. I also set min via to 0.5mm which still leaves a .15mm annular ring with a 0.2 hole.
I like my silk text height/width at 0.8mm and 0.15mm thick and bulk edited my library parts to make that the default.
Just for balance I am a JLCPCB customer and have been for many years and never had a problem. I have always used the defaults that Kicad ships with ! I have some reasonably complex stuff but I adjust tracks and things as I need too and never been told by JLCPCB that my demands are unreasonable. They also have a plugin that I used for the first time last week and that worked fine. From what I read I don’t think you need to think about speed and current beyond make the high current tracks the appropriate width (fat as space permits ) Thats my two pence worth, I hope it helps.
I’ll toss in another vote for JLCPCB–not against PCBWay (I haven’t used them, but I’ve heard generally good things about them), but I’ve also been happy with JLCPCB, including their assembly service. And if it’s their pick-and-place machine placing the parts, SMD assembly gets a whole lot easier. They also do THT assembly, but I haven’t used that service and understand it’s a good bit more expensive.
I have some reasonably complex stuff but I adjust tracks and things as I need too and never been told by JLCPCB that my demands are unreasonable. They also have a plugin that I used for the first time last week and that worked fine. From what I read I don’t think you need to think about speed and current beyond make the high current tracks the appropriate width (fat as space permits 
) Thats my two pence worth, I hope it helps.