Decoupling Capacitors on Schematics - Page 1
Forum section: electronics / projects

author: samsamm777
author_rank: Contributor
timestamp: November 09, 2020, 01:45:29 pm
content: I'm very much a newbie, and learning the ropes thick and fast. I've been watching plenty of PCB design videos, mostly Phil's Lab recently. I've noticed something regarding how decoupling/bypass caps are drawn on schematics, and im really unsure of the rights and wrongs of it.I see many many examples of people drawing decoupling caps as a separate block / grouping with no reference to which IC or component they are supposed to be bridging. I feel this approach misses some vital information in the drawing which states the location required for each capacitor to be optimal. Ie as close as possible to the component.I have seen drawings expressed like the following which I think is much clearer to denote the locality of the cap in relation to the IC. Curious you guys opinion on the matter. I feel like this fashion of drawing circuit diagrams with as little wire connections as possible has a detrimental affect on the intended purpose of the drawing.Bad Examples:Good Examples

author: jfiresto
author_rank: Frequent Contributor
timestamp: November 09, 2020, 02:02:24 pm
content: I would place the decoupling capacitors wherever they make the schematic most clear. The first "bad example" might be a good one if, after glancing at the board layout, the reader will confirm that each IC has a decoupling capacitor (its capacitor) next to it. Why then interrupt and spread out the rest of the schematic with what is obvious and might only distract?

author: Vovk_Z
author_rank: Super Contributor
timestamp: November 09, 2020, 02:05:20 pm
content: Quote from: samsamm777 on November 09, 2020, 01:45:29 pmOf cause you are right. That approach possibly goes from a bit lazy people. Of cause it is much better if drawing is self-explaining as much as possible.

author: TimFox
author_rank: Super Contributor
timestamp: November 09, 2020, 02:16:25 pm
content: One of my schematics drawn that way while I was in grad school (45 years ago) was given to an undergraduate technician, who did not understand the intent and substituted a single large capacitor in one corner of the hand-wired board. If the decoupling connection is important (as it usually is), at least add a note at the capacitor block about how they should connect.

author: Conrad Hoffman
author_rank: Super Contributor
timestamp: November 09, 2020, 02:34:36 pm
content: I've commonly seen them done that way, and rarely any other. Otherwise, they could turn a clear drawing into a cluttered mess. Location of bypass caps is only one layout consideration, so relocating them still leaves the whole rest of the layout to be considered.

author: David Hess
author_rank: Super Contributor
timestamp: November 09, 2020, 04:05:02 pm
content: I would consider the third example bad as well unless it is intended to show that the decoupling capacitors are *not* between the supply and load. Is that what is intended?

author: ataradov
author_rank: Super Contributor
timestamp: November 09, 2020, 06:00:07 pm
content: Quote from: samsamm777 on November 09, 2020, 01:45:29 pmYour "bad" example is pretty much industry standard. You won't see anything else on huge schematics (10+ pages).You are right, it misses the information on layout. That's why there are notes. Real schematic will have a ton of notes to the layout people. Sometimes there are entire essays with requirements and calculations.Also, layout people generally have a good idea of where capacitors should go. And the whole design process is iterative anyway, if something was not placed as schematic designer wanted, it would be corrected after the review.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 09, 2020, 06:32:02 pm
content: Both are good and bad for different reasons.As a layout expert, I like to have the freedom to place things as needed. I loosely model the board in my head and place caps accordingly. I may remove or add some to the schematic, or change their type or size.I tend not to imply too much layout meaning in my schematics, going for readability foremost.The worst of both worlds, is when this process has been done, then not back-annotated to the schematic -- caps that are drawn local to some component or another on the schematic, might end up in random places on the board, grouped in different amounts, interspersed with bulk caps, etc.Novices should probably stick to consistency and locality, using the manufacturers' general recommendations and grouping things on the schematic. As one learns how capacitors work and interact, the groupings can be refined, and layouts improved.Tim

author: phil from seattle
author_rank: Super Contributor
timestamp: November 09, 2020, 06:54:00 pm
content: In a shop where there is specialization (ie. PCB designer and EE) there are always a lot of design notes and often the EE is looking over the PCB designer's shoulder (literally or virtually). So, where the BPCs are located on the schematic is not terribly important. In my "shop", I play both roles plus janitor and CEO. So, I draw it with the BPCs placed near the target IC but never draw lines to connect, instead I use labels. For me the schematic is not meant primarily to communicate to others but rather as a necessary step in getting to a PCB. If I do publish a schematic, I will clean it up but still do not draw all sorts of lines.

author: Gyro
author_rank: Super Contributor
timestamp: November 09, 2020, 07:07:04 pm
content: Even if the decoupling caps are distributed nicely on the schematic, by the time you get to the PCB netlist they are all in a clump again. Even with decent notes and interaction, we often used to have to go searching for the quiet little corner where Our layout guy had placed the 'spares'.

author: tggzzz
author_rank: Super Contributor
timestamp: November 09, 2020, 08:10:07 pm
content: Quote from: samsamm777 on November 09, 2020, 01:45:29 pmGood to see sombody thatthinksabout what they seeTo generalise, there are two situations:where specific decouplers are required for a specific purpose"generic" decoupling required for general principlesThe classic examples of the first type are found in high frequency or sensitive analogue circuits. If you look at data sheets and application notes, you will see specific capacitors shown. IMNSHO you should duplicate that in your schematic.Classic examples of the second type are the distributed decoupling capacitance/capacitors spread across digital boards. Here the location of a capacitor is not critical, and they are placed where convenient during layout. These might as well be crammed together in the corner of a schematic. for faster/denser circuits this is becoming less valid; there is a cottage industry in analysing the impedance of "power distribution networks" on PCBs, where transmission line and RF effects have to be taken into consideration

author: Bud
author_rank: Super Contributor
timestamp: November 09, 2020, 08:26:01 pm
content: Decoupling capacitors symbols take space on a dense schematic and there maybe lots of them. There is rarely a reason to place the in-circuit, it is typically better group them in a corner of the schematic sheet or in a separate schematic sheet with the power supplies. This helps keep schematics clean. Decoupling capacitors are Not needed to understand schematics, they are utilitary. There is nothing technically "bad" with your "bad" example.

author: Benta
author_rank: Super Contributor
timestamp: November 09, 2020, 10:20:39 pm
content: Quote from: Bud on November 09, 2020, 08:26:01 pm+1Schematics are not there for helping PCB layouters, but for explaining and documenting the circuit function. If the PCB artist does not understand this, then hire a monkey instead.

author: Cerebus
author_rank: Super Contributor
timestamp: November 09, 2020, 10:53:29 pm
content: Quote from: Benta on November 09, 2020, 10:20:39 pmBefore I got to this I was working up to a comment like this:Depends, if the schematic is there for a human to understand how the circuit works then I want the decoupling caps to be visible in the part of the circuit that they affect. On the other hand if the schematic is just for the layout monkey then a block in the corner and copious notes is OK.

author: KE5FX
author_rank: Super Contributor
timestamp: November 09, 2020, 11:24:28 pm
content: I like it when the decoupling caps are inside the IC package where they belong. When a board looks like this, fromShahriar'snifty Keysight MXR teardown:.... it means the IC packaging people need to get with the program. Yes, it's more expensive, but so are PCB processes like the one above.

author: vk6zgo
author_rank: Super Contributor
timestamp: November 10, 2020, 12:15:40 am
content: Quote from: Benta on November 09, 2020, 10:20:39 pmSometimes I think they did!

author: drtaylor
author_rank: Regular Contributor
timestamp: November 10, 2020, 01:42:47 am
content: I like to have a "Power Block" section on the schematic. I also use a modified capacitor symbol to indicate that it is a bypass capacitor. The modified capacitor symbol allows clarity on which capacitor is closest to the IC. If you use double or triple bypass caps, then you can place them to clarify how they should be placed on the PCB layout. Having the power block allows the rest of the circuitry to be cleaner without sacrificing signal flow clarity. It is true any competent engineer / layout designer does not need this level of detail, but I find it very helpful. BTW, the angled cap symbol is one I use for PCBs that have ground planes. I use a cap symbol with two angled legs for non-planed boards or for indicating a bypass between two power supplies. For example, sometimes it helps to have a bypass cap between the plus and minus supplies on analog circuitry.I use a lot of not so standard schematic symbols. There are purists that frown on this, but I find so many standard symbols to be antiquated in appearance and too many symbols are duplicated or too similar to often far different functional devices. When I'm working on my own projects, I'm the only one I need to please. This approach does require a Schematic Capture program that allows you to separate pin functions while maintaining package integrity.

author: Siwastaja
author_rank: Super Contributor
timestamp: November 10, 2020, 12:10:39 pm
content: If you place them close to the relevant ICs which all share same voltage bus, they end up in one clump when brought in to layout tool, then you easily mix them up so that even though C1 is next to U1 and C2 next to U2 in schematic, they end up C1&U2 and C2&U1 in layout, and the end result is highly confusing!If you put them in a single block, you kind of give up before even trying, but the end result isn't any worse."Schematic is completely different entity from PCB layout" is also bollocks. Schematic drawnin the PCB EDAis, however unelegant that sounds, doneforlayout, after all. It makes no sense to try todetachit from PCB layoutcompletely, then add dozens of notes to convey information lost in the process. While different people may be responsible for high-level block diagrams, BOM selection, simulation (often done in functional parts, not the whole netlist in spice), the final "PCB EDA schematic" and layout should be, IMHO, done by the same person/team in close cooperation. During that process, both the schematic and the pcb layout changes all the time, in sync, while higher-level specification, simulated analog parts etc. stay put.What I would really want is, when the netlist is first time imported to the PCB, I would like the part placing to loosely match the placement in the schematic! Of course it isn't the right one, but it's a whole lot better starting point than having all the parts in completely random order, in one big clump; or much simpler than running overly complex auto-placement just for initial guess. If you do this thing properly, you use logical grouping (such as "rooms" in Altium) to reduce the size of the clump and have multiple clumps tied to (possibly groups of) schematic page(s), but it's still funny to have a completely random placement as a starting point.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 10, 2020, 12:20:47 pm
content: That would be nice. Hmm, should be reasonable to script that in Altium. Might be hard with channels, but as long as the indices are accessible that should still be doable.Tim

author: langwadt
author_rank: Super Contributor
timestamp: November 10, 2020, 01:17:03 pm
content: Quote from: Siwastaja on November 10, 2020, 12:10:39 pmI sometime cheap and export a net list where the each cap is connected to the right pin but the pin not connected yet to a supply, that way the rastnet help show where the caps go

author: Cerebus
author_rank: Super Contributor
timestamp: November 10, 2020, 02:03:01 pm
content: Quote from: langwadt on November 10, 2020, 01:17:03 pmThe necessity for that work around, and the discussion that led up to it, yet again adds weight to my suspicion that eCAD tools get either produced by programmers who don't do electronics, or electronics people who can't program.Were it my job to design and write the code that deals with this problem in a CAD tool I'd probably do something like this:Either:Add an attribute to every component that allows it to be associated with another component. Then you'd be able to do something like "Right-click on a capacitor", select "associate with" and then click on the IC it decouples. Then you can place the capacitor anywhere on the schematic, but there's an association that tells the PCB layout code that this component should be placed 'near' the associated componentORAdd a specialised "decoupling capacitor" to the components you can place in the schematic (it doesn't have to be necessarily visually different, just logically). When you place one you're asked automatically "What component is this decoupling capacitor decoupling" and then behind the scenes it looks like the previous scenario except that the relationship is "decouples" rather than "is associated with".My preference would be for the more general scheme, regularity has its advantages both for the programmer and for the users of the associated UI. That has the advantage that the components you can make "associated" is arbitrary, and there are more scenarios where it's useful to have components physically 'near' each other than the specialised decoupling case.

author: sandalcandal
author_rank: Unknown
timestamp: November 10, 2020, 02:12:25 pm
content: I have a dual screen setup and when I grab a component in the PCB layout it shows me the component in the schematic automatically so I know which component it is and what it goes with. Useful for not just decoupling caps but all components. No need for additional overhead having to manually associate components other than having them well laid out in the schematic.

author: Cerebus
author_rank: Super Contributor
timestamp: November 10, 2020, 02:21:48 pm
content: Quote from: sandalcandal on November 10, 2020, 02:12:25 pmThat's fine if you have the screen real estate and the man drawing the schematic is also the layout guy. If it isn't the same guy which would you prefer (1) a formalised relationship built into the tool, or (2) a written note that you hope conveys to the layout monkey what you want done?(Substitute guy/gal/monkey as suits your own views on political correctness/speciesism.)

author: langwadt
author_rank: Super Contributor
timestamp: November 10, 2020, 02:31:59 pm
content: Quote from: Cerebus on November 10, 2020, 02:03:01 pmI'm not sure cap to component association is enough, many chip have multiple supply pins

author: tggzzz
author_rank: Super Contributor
timestamp: November 10, 2020, 02:35:15 pm
content: Quote from: Cerebus on November 10, 2020, 02:21:48 pmFor high-speed and/or analogue circuits and/or RF circuits, political correctness has nothing to do with it: getting your stackup and layout working correctly is far from trivial! The designer, EMI/EMC/PDN specialist, and layout specialistneedto have been talking to each otherlongbefore it gets anywhere near layout.Apart from that my attitude to the OP's question is fairly simple:digital circuits: providing not high speed, you might as well stuff the decouplers in a corner of the schematic. You should also indicate balanced lines and impedance (e.g. for USB interfaces)analogue circuits: if the IC's application notes or datasheets show decouplers, then the bias is strongly towards showing them in the correct position on the schematic, next to the IC's pinsRF circuits: mandatory to show everything possible in the schematic

author: SiliconWizard
author_rank: Super Contributor
timestamp: November 10, 2020, 03:39:23 pm
content: As already said above, it really... depends.Generally speaking, I tend to agree with you though. (And yes, as others have said, your "bad" examples are still almost industry-standard.)My approach is to be reasonable and make the schematics look as readable as possible. Obviously on a big IC requiring tens of bypass caps, putting them directly close to the IC, on each power pin they are supposed to decouple, can make the schematic bloated and hard to read (not mentioning it takes longer to do, and you probably have better things to do with your time.) So in this case, the "block" approach is reasonable. OTOH, if only one or two caps are required, I draw them directly tied to the IC pins.One thing that is simple to add (fortunately, often added, but not always...) when using those blocks of caps is a caption of which IC they are supposed to be tied to. When there could be an ambiguity (as if some power pins were not decoupled or if they would need different cap values), just add a list of the corresponding pins to your caption. I wouldn't draw such a block without any caption (as in your "bad" example), even when there is only one IC on the sheet. THAT is IMO bad habit.

author: TimFox
author_rank: Super Contributor
timestamp: November 10, 2020, 07:21:53 pm
content: I like the drawing in DrTaylor’s post above. If I remember correctly, the drawing (hand drawn in ca. 1975) that I discussed above was the same format, with rectangles denoting individual ICs in the corner of the page.