What’s the exact area to be respected for a component? Is it the outer edge of the courtyard? The inner edge? Or the “ideal/mathematical” line at the middle of the courtyard rendered lines?
For most cases, this is irrelevant and one can simply leave a little gap beyond the courtyard outer edge; but for, say, 0201 decoupling capacitors that we want as close to the pins as possible, then I wonder: what is the closest possible?
As an example, graphically — which of the options would be the closest acceptable placement?
Or can I still go to option 4, where I would make the inner edges match?
In my case (and I’d guess in most cases), the more relevant part is: how close can the capacitors be to each other (since I have several of them connecting to consecutive pins, so any tiny differences add up and I have to space them out or the traces won’t fit).
IIRC v5 has an option to check courtyard violations with DRC, so try that with different placements.
But the real question - how close to each other components can actually be - is more difficult. The first question is what the courtyard means: does it mean that other component’s body shouldn’t cross the courdyard, or that two courtyards shouldn’t cross? Courtyard is meant for assembly phase to make sure that the components can be physically handled and placed next to each other and then soldered. Requirements for manual soldering can be very different than with machine assembly. In my personal opinion it’s OK to violate courtyards selectively if you know it works and can be assembled and soldered. In general it’s good to obey them if you know they have been designed well. Use your common sense and experience.
I’m pretty sure the board can be assembled if you place the components like in your third picture.
Assuming that you are designing a board for manufacture and just doing a paper exercise, then the answer is : it depends on your fabricator capabilities. We can’t answer that.
The official libs use IPC guidelines which I believe are based on conservative values that should be completely reliable using current technology.
That’s why I thought of asking on this forum — my question referred to how the libs are designed: with the intended effective courtyard being the outer edge, center, or inner edge?
Anyway, I just sent a query to the manufacturer, to see whether they have specific guidelines/specs about minimum distances between components.
Interesting — and interesting that I didn’t think of that; for the clearances, it was more or less obvious to me that the clearances of two adjacent traces could overlap (i.e., that clearance means no other trace can get in, and not that no other clearance zone can get in). But it didn’t occur to me to consider the same principle for the courtyards.
The courtyard line is 0.05mm, so the distinction is insignificant.
But you are still missing the point, the courtyard is a guideline. Even if you meet the IPC paper spec, it is not a guarantee that the fabber can build it with 100% success : you need to verify with the fabber. Equally, if you violate the line by 0.05mm does not mean you will get 100% failure, you need to verify with the fabber.
Too many engineers regard the spec as black of white, the reality is there a sliding scale, the tighter you design, the lower the yield and the higher the cost. Some components might have a waiver to violate the guidelines, others might require much more conservative specs.
The IPC have several options, I think KLC uses “nominal” option. In practice, you will probably always be able to violate the guidelines by a little bit, but don’t if you don’t need to. The same applies to all the other PCB specs.
I also think fabs are too conservative if you ask them.
Overlapping edges is alright, and depending on the components, even tighter placements can be done.
Another way to see the mechanical clearances is the 3D viewer. Optical, and subjective analysis can be done. Testing from a top view that components aren’t overlapped or “too close”.
I would maybe contest your view that the distinction is insignificant; it’s always relative: when you see it against a 0201 part, the thickness of that line ends up being 5% of the component’s width. 5% is a reasonable “within tolerance” figure, but I would say not insignificant. But no, this does not contradict your more general point, with which I agree!
I would say that the libs are designed with the center of the line being the effective courtyard.
For example, if the KLC tells me I need a 0.5mm courtyard for my part, then I draw the courtyard so that the center of the courtyard line is 0.5mm from the center of the fab line. (The lines are essentially “ideal” lines, and the width is just to make them visible.)
But as others have pointed out, the courtyard isn’t really that precise of a quantity, so it doesn’t really matter.
P&P accuracy could be +/- 0.03mm, or worse… there is a trade off between speed and accuracy.
If you consider rework, how wide is your solder iron tip? etc
Theoretically, it is the centerline. But the width of the line represents the fuzziness of practical application. Mathematicians can create lines of zero width, we engineers can’t
Whoa! Soldering-iron-rework for a 0201 part is waaaaaay beyond my skills level !!!
But yeah, I know, I’m again missing your point
That was a very nice way to put it — the courtyard is defined as the ideal/mathematical line, but the rendered line with a non-zero width represents the reality (the tolerances/inaccuracies of all aspects involved in assembling a board)
If you are good enough with your hands to do normal soldering with bigger SMD components you would quickly learn to handle 0201 with a microscope and a good iron. But I wouldn’t try that without a microscope.
To stay on topic, I routinely handle 0402 manually. For manual work, too, it’s true what has been said: courtyards are only guidelines. It depends on all the surrounding components whether you can violate courtyards or should leave even more extra room around the component. A pick and place machine can drop 0402 between, say, two mini usb connectors, and they will solder well with a machine, but trying to rework it with an iron may be impossible.
That’s the one that is save to use - any tighter and you’re essentially on your own (which is no problem if you know what you’re doing).
KiCAD expects such distances to count to the CENTER of lines like those (except for zone fill vs edge.cut lines, there the algorithm has a bug that takes the edge of the line, which leads to the thickness of the edge.cuts line influencing the zone fill).
But yeah, otherwise the thickness of marking lines should be no influence on the underlying meaning.
So you can go to the center.
PS: if you’re hand soldering, consider lining the SMDs up in rows, with the pads along the long sides of that row, so that you can easily access them with a soldering iron from the side and don’t waste too much space (screenshot depicts mostly 0805 in a convenient tightness for handsoldering without a microscope ).
PPS: if you’re doing prototypes or hobby work and not scientific/medical/space stuff, don’t go as tight as you can, go the opposite direction, make it as loose as you can bear. Especially when you’re starting out. Once you need to rework or modify you’ll be happy that you left some space to operate in.
Once something works and you’re getting it made in the hundreds you want to optimize, but not before.
PPS’s … always the most useful pieces of information
In my case, the situation is tricky; yes, for most of my personal/hobby projects, I try not to go below 0805 (and that’s already aggressive; originally, I figured, no reason to go below 1206). But then, when my hobby projects start to use DSP chips that only come in 0.5-mm pitch and where the (presumably noticeable) performance depends on proper decoupling, then I figure: might as well forget about soldering myself and get it done quite inexpensively from manufacturers in Asia. Yes, of course, I’m sacrificing the ability to rework to fix bugs/glitches in my design (bound/likely to happen in the first iterations of the design). Maybe at some point in time I will get a set of really good tools for soldering (both reflow and rework), including a good stereoscopic microscope. For now, it is probably more cost-effective to just get it done, which then allows me to go as tiny and as close (roughly speaking) as necessary.
I can manage 0805, and sometimes 0603, using a moderate-cost swing-arm desk magnifier (“MAG Lamp XL”, model UN1030, about US$125) and a small soldering iron tip (Hakko FX-888 with T18-C05). A microscope certainly helps, and extends my capabilities to 0402. At work I have a wide-field binocular toolmaker’s microscope that cost my employer a bit less than US$200 at AMScope .
For board assembly I use solder paste and an electric skillet (about US$10 at the second-hand store). The cost of plastic stencils has followed the price of circuit boards. Some of the quick-turn board houses will add a stencil to your order for a few dollars, making them economically viable for even one-off projects. After a practice run or two I could turn out boards that were much more consistent in their soldering than if I hand-soldered them, even under the microscope - and do it in a fraction of the time.
Use parts in 0201 pitch? Forget it! There is no advantage to the small size - the courtyard necessary for positioning components with tweezers, toothpicks, or dental probes is 5 to 10 times larger than the part itself!
I’m also using a binocular microscope exceedingly similar to the Amscope SE400-Z with 10x widefield. Currently handle 0603 with ease, recently been trying 0402. No specials tools, just regular iron with fine tip, tweezers, copper solder wick, fine solder.
Solder paste is horribly messy, difficult to apply, and goes off quickly.
I’ve also tried some DIY techniques: toaster oven (not enough, difficult to control), electric hob (too hot, difficult to control), hot air gun (difficult to get right). I guess like everything practice makes perfect, so I need more practice…
One day I might get a cheap reflow oven package, plus stencils for solder paste, but it’s hardly worth it for occasional use.
).