Hello,
I am currently building my first “real” project, and I am not sure if what I did is okay:
I placed my components as close as possible so the filter will work as intended, but I ignored the courtyard marks. How can I know if it will work when the manufacturer assembles the PCB ? I believe I will use PCBWay for the fabrication and assembly. I reached out to them, but it’s Sunday, and they don’t work today. If any of you can shed some light on the matter, I would appreciate it.
Thanks
Yes, I read it, so the take-home message is:
You need to know the limits of the assembly process and the interplay between that component and surrounding components.
So, I will need to get an answer from PCBWay. But what I didn’t understand is how the courtyard is determined. For example, most of my components came from SamacSys Engine. How do they decide on the courtyard size?
I guess that the assembly machines push the components vertically from a long distance above and practically speaking a courtyard isn’t even needed. As I wrote in the FAQ, “In my personal experience I have seen that, for example, with 0402 components, the copper clearances limit placement more than the suggested courtyards”. Which means the courtyards can virtually be ignored when you have low components side by side.
THT components are often taller and larger (e.g. connectors and elcaps) and may require more room around them, but not necessarily for themselves. You have to take the space needed for manual work into consideration. If you need to manually solder or repair smaller components near larger ones, the space is needed for the small components and the area may be larger than the small component’s own courtyard. You should try to visualize or test somehow what you can and need to do when you use the soldering iron, tweezers, microscope etc.
By guessing, I guess. Maybe they have people there who have some experience. I don’t know about any standards or other fixed rules. Even professional experience can give only a rule of thumb which may be about as good as a less educated guess.
got it, thank you !
i will wait for pcbway to see which restriction their assembly machine imposes 
Please tell us their answer, it may benefit other people.
Actually the KLC refers to IPC-7351C, but that seems to be non-existent and superseded by https://www.ipc.org/TOC/IPC-7352-TOC.pdf. If someone has access to it they could tell us what it says about courtyards. It probably gives some kind of parameters for standard component packages. But it can be only a recommendation which guarantees it works well in most cases, i.e. “large enough for almost any situation”. It couldn’t tell anything about optimized minimal distance or what you actually need. KiCad’s KLC already uses existing standards where possible, so you could follow that and not overlap the courtyards in the design. It doesn’t hurt if there’s enough space on the board.
that is what i intended to do, i believe tomorrow i will have the answers
What is going on with your biggest SMT capactitor?
The courtyard of those three big resistors look out of proportion. Where do they come from?
And why are your pads rectangular?
For comparison, I placed a SOT-23-5, a 2010 and an 1206 sized resistor from KiCad’s default libraries (V8.0.3) next to each other for comparison. I put them on the front of the PCB, so the text is readable.
| yageo | RC0603FR-0720KL |
|---|---|
| yageo | RC0603FR-0741K2P |
| yageo | RC0603FR-1340K2L |
| TI | TPL7407LDR |
| Panasonic | ECH-U1C333GX5 |
| panasonic | ECH-U1C153GX5 |
| yageo | CC0603JRX7R9BB104 |
you can see here the components (without the TPL) and i took the symbols and their footprints from mouser for example here : panasonic ECH-U1C333GX5.
now because of your comment i went and checked - i put 1206 components on top of the ones that supposed to be 1206 and they match in size but the courtyard is massive compared to Ki-cad’s parts. and also i did it for the 0603 parts and they match. i think because they are so different in size it looks like this.
what do you think?
I use KiCad’s native footprints if they are present and only use alternative sources (or make my own) when it’s really needed. When I first saw the rounded corners in pads (and thus also solder stencil) in KiCad’s libraries I thought it was a bit strange or a gimmick. But after reading a bit, I learned it’s actually useful.
For the rest, I already mentioned he courtyard from that footprint you fond from mouser was unusually big. But in the end, it depends on where the SMT placement gets done. Neither KiCad nor Mouser can now in advance you plan to use PCBway.
hello,
i got a replay from PCBWAY :
Pls ensure the min spacing between two components at least 0.5mm
Interesting. I’m pretty sure they can do tighter. According to this, in KiCad footprints 0402 and smaller would have too little space between two parallel resistors when the courtyards are obeyed (and they most probably obey the IPC standard recommendations if possible). I believe the manufacturer/assembly factory wanted to give only one easy number for you. I can understand that, it would be too complicated to advice customers with a detailed answer and actually any exact answer and numbers don’t exist, even for them.
A 0402 resistor has a size of 1.0 by 0.5mm, and in KiCad the courtyard is 1.86 * 0.94mm. If you place two of these next to each other (with touching courtyards) the clearance is indeed only 0.44mm.
Ans as Eelik already mentioned, things like this are not simple numbers. If you look at Calculator Tools / Memo / Board Classes you see a bunch of standardized numbers for different manufacturing capabilities. There may be something similar for SMT placement machines. There are a lot of different machines out there with different accuracies and capabilities. PCBway is one of the big board houses. They probably can go finer, but I guess they give you some conservative numbers. If they had to fine tune each small batch of 10 PCB’s they would be assembling PCB’s at a loss.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
