LibrePCB
librepcb.org
librepcb.org
- How comprehensive is the part library?
- Is there auto-routing? How good is it?
- "Import formats: DXF". For what, the board outline? DXF is for mechanical CAD. You can't import a board layout or schematic that way.
- "Export formats: PDF, SVG, pixmap, BOM, pick&place, Gerber/Excellon". None of which have enough info for import into another EDA program. This thing is very self-contained, which is unusual for an open source program.
This seems to be is a marketing tool for some board maker. "At this time, you can choose either AISLER or PCBWay as the PCB manufacturer. With every order you start with LibrePCB Fab (or direct .lppz upload on the AISLER website), they will make a 'donation' to the LibrePCB project."
Why do people always ask for this? It's a feature only newbies use, and once a project becomes even slightly less than trivial, the best auto-routing tools fall face down. There's an awful lot more to PCB design than just physically fitting the components on the board.
It has no comprehension of the actual components it's placing, or the nets it's routing. So it'll find a physical layout that matches your schematic in a logical sense, but the actual circuit may not work when it's finally assembled (ADC placed next to a switching power supply, for example). Some components have strict tolerances or needs, and some types of designs require special considerations.
So, a newbie will click the button to auto-route and then have the board fabricated and then do the final assembly - then wonder why it doesn't work, or it sometimes works, etc. If you don't have the skills and knowledge to do the layout the "right" way, you likely don't have the skills or knowledge to debug a bad board layout.
PCB layout is not trivial. Some folks spend an entire career doing just PCB layout. For low-speed trivial designs, you can get away with a lot of bad practices, but it's best to invest some small amount of time learning the craft.
However, general rule of thumb, if your design works on a breadboard then you can probably make it work on a PCB... probably.
The issue with PCB-design is that:
1. Even the slowest ~4MHz microcontrollers have 1ns rise/fall times, or 1GHz+ of high-frequency noise all over the place. Faster chips have even faster rise/fall times.
2. ~1GHz wavelength is ~30cm, meaning that a 7.5cm trace is an effective antenna for 1GHz noise. As it turns out, 7.5cm is well within the scope of typical PCB design. A faster rise/fall time (ex: 0.2ns rise/fall time is 5GHz noise instead) could have "antennas" as small as 2.5cm or 25mm.
3. Vias have non-negligible inductance and resistance. Modern signal design also requires the designer to think of "the return path", so a 2nd nearby via to serve as a capacitively-coupled via (IE: "Route a ground-via next to any signal-via"), and other such rules, are rarely followed by autorouters.
------------
It looks like the professional tools are fixing this problem by performing FEA of signals / coupling / electronic flux, and helping the engineer visualize the magnetic and electrical fields of the designed PCB-layout.
However, if you are a conservative human, you can get such a feel for your circuit by thinking about return-paths and mentally thinking about microstrips (ex: wire + ground-plane return), or striplines (ex: ground-wire-ground plane for internal layers). The return path is always on the nearby ground plane, so it makes it very easy to think about.
On a long-enough timeline, ML tools will become a natural fit for placement and routing. It is a rather dumb thing for humans to have to deal with, at the end of the day, but the existing tools are just not good enough to take over the job. At least not the tools that most of us have access to.
Lets say you have a trace that's 4mm wide that skips across a slot in the ground-plane. Is this good or bad?
1. Why is it 4mm? Is this a high-current line / power line of some kind? A crude power-plane that's just oversized for a trace? Is this a switching regulator with a bit of switching noise? Or is it a "quiet" power line, like a battery or LDO-line?
2. Is this trace actually ground? And the 4mm is to "jump" across the gnd-slot to provide a controlled return-path for some other line? What is the relationship of this trace vs another trace?
----------
If its a fat line on a switching power supply with a ton of current, maybe its a bad idea. If its a fat gnd, maybe its a good idea. Its all contextual. Its not very clear how a hypothetical ML tool would figure out this context, outside of like learning to read data-sheets and/or the EE writing down the purpose (very precisely) on each net... which probably is slower than just routing the trace manually to begin with.
Eventually.
Or hell, that PinC1 is an input vs output.
Modern chips have very flexible pins. Many microprocessors (and MCUs) can configure any pin to be input, output, tri-state output, pull-up output, or pull-down output, for example, with different properties in each state. Some pins can be analog (on-board op-amps), others can be digital and high frequency, still others can be digital but rarely-changing / effectively DC for the lifetime of the application.
Each scenario changes how you'd route a trace.
Tools to help with high speed are much much more important
Because when you market a tool as "Easy to learn", "from beginners to experts", and "For everyone", then I would expect some decent newbie-friendly features.
Honestly as a non-professional who makes PCBs that are almost exclusively "connect this pin to this other pin over here", this kind of comment comes of as a bit unnecessarily condescending in a "I don't need this feature, so nobody else should need it either" type way.
Take software for example - newbies can and do write code, but it's rarely good or error-free. Codeless solutions have appeared - but there's good reasons even those aren't used often.
Any auto-routing feature is going to appeal to absolute beginners, and few if anyone else. So, we're asking a FOSS project to spend a tremendous amount of time building in a good-enough auto-routing feature that only a small portion of their audience will ever actually use, or use more than once.
If your board is simple enough for auto-routing to provide value to you - then I would assert your board is simple enough for you to spend 30 minutes doing the layout yourself.
I would have thought that autorouting would have improved in all that time, but from this conversation, it sounds like it has become worse. What gives?
More focus on hybrid routing tools where there is some automation going on while a user routes things is typically were you get much more useful help in modern ECAD.
Maybe you could encode all of them in the schematic and then let a modern algorithm suggest a board layout, but in practice nobody seems to do it that way (note that I am just a hobbyist with limited experience).
I worked with an RF engineer who'd been in the field since the 70s, and he'd always use the auto-router for anything "slow". If it was "digital dc" or digital logic or under a MHz then it was auto-routed because he didn't have time for that. Anything critical that carried RF or drove a reference was hand-routed first then anything left would get the auto-routing treatment. And this was in a radio astronomy observatory!
If you cannot commit a few minutes to learn how to route correctly, then you really are just "hoping" for something magical to work.
Would you take the same position in software? Almost certainly not - because it is complex.
Sure, there's plenty of no-code or low-code platforms out there - but why are they not more popular? Because they universally suck and their target user quickly "graduates" into real coding.
People asking/demanding auto-routers are asking a FOSS project to commit a lot of time and resources (because it's not trivial to implement!) to a feature a very small subset of their userbase will ever use, and will also be the most negatively impacted by said tool when it fails them without them realizing.
Seriously, if your board layout can be done by an auto-router then it is a trivial board and you should spend a few minutes learning the basics. There is nothing but upside in doing so.
Unlike software, all the "features" of a component are not readily available to a tool like that. Maybe one day they will be, but we're very far away from that. No two component manufacturers do anything the same...
Its the random creation of antenna that suddenly throws your electrons off the board and suddenly causing nearby traces (to also turn into antenna) to get crosstalk leading to failure. Or throwing your electrons off the board and failing EMI regulations.
With 1ns rise/fall times on typical microcontrollers (even a 4MHz ATMega328 / Arduino), an antenna can be inadvertently created with just a 75mm trace. With a faster chip, you could have antenna at 25mm or even shorter traces.
-----------
PCB board design today is about understanding the physical attributes of the PCB: how the stackup causes your board to act like a capacitor (and therefore a source of voltage when the bulk / decoupling capacitors run out of energy). Seriously, this is called "PDN" or power-distribution network. You turn Layer2 into a ground-plane and add a plane to Layer3, calculate the dielectric thickness and estimate the amount of latent capacitance you get between a 30mm^2 ground vs power plane seperated by 0.1mm of dielectric.
And not only do you calculate this, you *take advantage of it* to reduce high-frequency (ie: 1GHz+) power-delivery issues.
Which could happen as low as ~100MHz in practice, because its more about rise/fall times than it is about the actual clock speeds.
--------
There are two kinds of PCB designers. Those who know that they're designing an antenna... and those who do not know they're designing an antenna. The PCB itself is an antenna and you need to design it in a very peculiar manner to minimize radiation. You can't just guess-and-check this (I mean, I guess with enough time/money you can guess/check... but ideally you lay things out with a mental simulation of inductances, eddy currents, an idea of electric fields and return paths of your signals across low-through-high frequencies)
If ~20MHz is the highest speed signal on your entire design (ie: ~20ns rise time, which STM32G0 or PIC or AVR beginner-friendly chips are around), then your wavelength is 15-meters, meaning the quarter-wave antenna would be (at a minimum) 3.75 meters (12 feet long), which is just far larger than any PCB-circuit a beginner will ever come across. (And will only in practice, be an issue on cables running off-board).
Why not?
> Sure, there's plenty of no-code or low-code platforms out there - but why are they not more popular?
I would compare software with auto routing and without more to Python with C situation. Auto routing is more like garbage collector to me. Should we discourage people from programming in Python just because for hobbyist C or C++ might too hardcore? It's not that they have to be professional developers - why not let them learn how to write even simple python script that help them processing some text and do simple automation? It's not that everyone need or want to write operating system.
After all today python is the most popular programming language even though it mostly started being used in education or basic scripting. Should we also forbid people using ChatGPT to help with programming for doing some creative coding? Let them have some fun.
Your example perfectly illustrates that autorouting is a catch 22: in order to get something useful out of autorouters you either have to (a) provide them with a enough information on signal, DRC, and fab parameters OR (b) have a design so simple that it doesn't really matter. (a) requires subject matter expertise that beginners won't have and (b) really is such simple point and click that beginners don't gain anything from an autorouter. The beginner already has to learn enough to place components on the board before routing, which IMO is where 80% of the leverage of expertise comes in anyway.
The calculation changes if you're all bought in on an EDA package like Altium and you know all about modular schematics and PCB docs on with standardized PCB layering. Then maybe you can start cobbling together quick designs that are largely autorouted but again, catch 22: you have to know enough Altium to know how to do that and enough electronics to know how to select open source modules and parts.
And I mean *learned* because it was not as simple as clicking a button.
Using it right means dropping down keepouts over sensitive areas so that the autorouter knows to stay away -- you know it, but it has no way to. It means placing vias to a ground plane next to every ground pin so that it doesn't try to deal with top layer ground planes breaking. It means telling it how much to penalize a trace for being routed on the power plane layer or the ground plane layer. [and on]
It's a super useful tool -- if you are careful with it like you should be with, well, chatgpt. Give it all the information you know it needs to know, patiently and quantitatively, and sure it'll find a reasonably optimal solution. You just have to tune it as well as you tuned yourself.
[edit: and you can do it in the reverse order for nasty piles of spaghetti nets that you can't smooth out with part placement, to get hints on where you'll have to run busses later so that you leave room -- but always route the sensitive traces first]
The newbie doesn't know that yet, and believes there could be any other approach, but that doesn't matter. They are wrong.
* The very best most costly, fall over and fail
* If your design is simple enough for the autorouter to work at all, then it's simple enough to do yourself.
These two points are true and unavoidable.
The "subject matter expert", actually, all of them not just any paryicular one, is in fact a subject matter expert, and is giving you the useful information that you lack. It is the most useful info and the shortest most convenient path from idea to working board.
I'm a hobbyist, and when I started out I used autorouting a lot initially to give me a starting point, and inevitably I would adjust everything manually. Autorouting wasn't magic, or even particularly good, but I found it helpful. My PCBs weren't particularly complex, but not dumb either.
I totally get that autorouting is almost certainly a waste of time anything serious, but writing off autorouting entirely, even for hobbyists, comes off as more of a meme than a position resulting from actual experience.
Hell, if autorouting really sucks that bad, then maybe that's a good way for some people to learn how not to route your circuit paths.
Don't you think it'd be possible to create such a thing, which would also create labeled solder points for jumpers where traces needed to cross?
Maybe "rat's nest" already does this; I don't know what that is.
Without that knowledge, it's impossible to create a good auto-router/layout tool. The tools often just stack components as close together as physically allowed by the necessary traces.
For very trivial stuff, it might work ok. Anything else, no chance unfortunately.
You start out the board deisgn by orienting your parts in a way that there are as few intersections as possible. Then you draw the connections, and the ratsnest lines disappear one by one. If you have intersections, you need to route around the part, or work with multiple PCB layers to get rid of them.
At that point "as few intersections as possible" becomes a bit of a lark and to maintain any semblence of sanity you have to prioritize connections, hiding all other nets.
It’s not meant to be condescending. Virtually everyone who starts doing PCBs goes through a phase where they think that it must be “easy” to press a button and get everything laid out and connected. Countless developers have tried to create software to do that over the years.
Maybe some day it will come to fruition, but the reality is that autorouting just isn’t very useful for setting up entire boards.
I think beginners get confused because they think the schematic connections contain all of the information needed to properly route a real board. Then you get into the real world and realize that you need to select connector locations in a way that make sense, place capacitors to minimize loop area, orient components to keep parasitics minimized on important nodes, make traces bigger where you need high current or better heat dissipation, and so on.
Which is why it’s not condescending to say that autorouting/autoplacement isn’t useful. It’s just a reality of making PCBs. You have to do a lot of manual decision making at layout time that isn’t easily automated away.
I have used autorouters for certain buses, but I have to set up the constraints in detail and steer the routing myself still. There is no autorouting/autoplacement that will make good boards for you, even though everyone goes through a phase where they assume it must exist.
I hope they add autorouting, but I would much rather have more parts libraries, access to the part supply house APIs, more 3D models, better tools for verifying that your design will be pick and placed the way you think it will and there isn't something inexplicably upside down because of a bad footprint file, etc.
Hobbyists often like to do more analog stuff with discrete parts than I do, so SPICE simulation in a way that's as easy as the Falstad sim may be important.
I don't think there's any true beginner friendly open sims out there, ideally you'd have a one-click way to fuzz all the components and see how everything behaves with noise in every wire, bad connections everywhere, 60Hz buzz getting in, etc, so you could verify it still works in the worst case of crappy counterfeit parts and loose connections.
My experience with the Altium auto-router (which is pretty good, as these things go) was that it took quite a bit more time to setup and tune than to just bite the bullet and manually route the board. Eagle's auto-router was easier to use, but it was also attached to Eagle.
At the end of the day, the difference between getting an autorouter to the point that it can autoroute a simple 2-layer board with lots of through hole parts, getting it to the point that its useful to the average professional, is monstrous. There's so much more to routing that just widths and clearances. It will probably someday be the case that most PCBs are laid out and routed entirely by computers. But for now, there's too much subtlety in PCB design. I'd lose my mind if I had AI-designed boards failing QC because of tombstoning, for instance. I'm not sure that anyone is trying to simulate board heating in detail enough to predict its occurrence, let alone evaluate solutions prior to board fab. And yet, the solution is pretty easy once you see that its happening in the first place.
I would consider it absolutely unnecessary, and invariably results in something that is unreliable at best.
Do you have examples that show how it is essential?
I can't see how it would cost me money to do so, on the other hand if I was to blindly autoroute my designs i'd spend more time troubleshooting and way more money doing several revisions before I got something stable.
It can't trivially tell which areas of your board you have intended for analog signals, or where high speed things are. When you autoroute a 2 layer board (in particular) if you don't drop vias next to ground pins it goes nuts trying to connect ground pins with a ground pour constantly changing. It tries to keep traces as close as possible to edges where a human would really just give it "breathing room". If you want to make a prototype that can be reworked, you need to be super careful (you always do, but it's easier to miss a lack of accessibility if it's automatic). It orients traces in ways that are in accordance with a score metric rather than geometric elegance, legibility, or crosstalk because it doesn't know what signals are where.
None of these are unsolvable, but they are the kinds of problems I expect when I use it. That said, if I have 1000 traces to route I will do 970 of them manually and be grateful for the autorouter doing the last 30 that would take me a half day to figure out a clean path for.
The problem comes when people think an autorouter is a computer program written by people who know about their PCB and that the results will approximate an expert doing an okay job. Then they realize that's not the case and decide the autorouter cannot do a decent job ever. Much later they realize that if they actually learn how the autorouter works they can use it as a tool to do... what the autorouter is programmed to do. But it can't read the designer's mind.
In the future I certainly hope that the integration of ECAD and Spice works transparently, I think it's closer every year.
I also hope that EMI simulations of PCBs become straightforward as well. I think if Spice worked, that would be a pretty clear second step and it would be a gamechanger.
As soon as the autorouter is aware of all of these constraints and is trying to keep signals that you manually specify to constraints you specify (say, from spice or from you reading the datasheet -- or an language system trying its best I guess, I've had terrible luck extracting data from datasheets).
That would be genuinely game changing. You could tell the autorouter not just "go diagonal or add 4 points" or "a via costs 3 points" or "stay away from this area" but instead "keep EMI spread spectrum and give me a spectrum for the noise as measured in a solid surface one meter away" so that you can actually simulate your FCC test. And make the autorouter minimize the spikes with filters of various kinds. And since Spice might know how fast you are operating different traces, and knows rise-fall times, the autorouter can simulate how much cross talk there is.
None of this puts the designer off the hook, it just changes the nature of the work. For more than a trivial board I think it's unlikely a human could do better than an EMI aware autorouter with Spice level knowledge of what every single net is doing -- and on top of that knows all about the capacitance between planes...
Basically, I see this as a huge opportunity for growth, and dismissing autorouting out of hand is something a senior professional might well do because autorouters have sucked for so long. They may continue to suck, if you don't use them like algorithms and instead pretend they are an expert. But I see a heck of a lot of people trying very hard to create an EMI and Spice aware ECAD system, even KiCAD has Spice integrated (albeit I have no clue how to use it). Eagle does too, so Autodesk will.
I assume Altium has Spice and I sure hope it has EMI since what else is the thousand dollars per year per head for... Okay, no, I know their parts management system is second to none I've ever seen, god I wish I could specify alternate parts and automatically generate BOMs based on alibaba real-time availability in KiCAD. But again... soon.
In any case, kudos to this project either way. I will never, ever use a proprietary PCB tool again in my life, I still struggle to get OrCAD 16.2 running and regret learning Eagle instead of just jumping to KiCAD and recognizing that nothing that can be bought will stay available.
It is too much to ask someone who does professional PCB designs to change tools for reasons that only are about the business that makes the tools. It's just a waste of so much billable productivity... that I don't want to do. KiCAD will hopefully be my last, I've learned my lesson.
That said... I am still trying to understand how this is better for a beginner than KiCAD, which does have an autorouter, has a pile of paired extremely useful tools (calculator, geber viewer, image importer), a pile of excellent add-ins, an excellent footprint library (I've rarely had to manually do it), a shockingly complete symbol library, a 3D viewer that I can use to check footprints against manually downloaded packages, excellent DRC, and for little things it can round traces and make teardrops which is just aesthetically pretty compared to sharp corners.
A few thousand parts total, so: Still quite small.
> Is there auto-routing?
No, just ratsnest. The utility of autorouting was already discussed in sibling comments.
> "Import formats: DXF". For what, the board outline?
It's mostly useful for the documentation layer or the Board outline. For example when creating a Raspberry Pi HAT, or an Arduino shield. It can also be used to import logos for silkscreen, or the like.
> None of which have enough info for import into another EDA program.
Can you give a concrete example of the use case you have in mind?
> This seems to be is a marketing tool for some board maker.
It is not, and it becomes obvious if you spend even just a few minutes reading through the website. It's mostly one developer, who spent almost 10 years developing the software in his free time, and who now tries to work on it full-time. Source of income are donations, some EU funds and revenue sharing of some fabs.
I will go to extra effort to avoid fees being imposed on the recipient of the money.
There have been times I have wished that I could import DXF as footprints in Kicad because it was easier to draw complex shapes in QCad or Inkscape. I think it could also be useful to import object placement/orientation data from a DXF file and snap to those when placing components.
For the latter use-case, I have instead written placements by hand as code in a Python script and made that output both DXF and Kicad files.
The CAD tools inside KiCAD could be a lot better (esp since it’s using FreeCAD under the hood and the tools should be there) but it’s OKAY as is.
Also, beginners shouldn't even autoroute. I can't think of a single valid reason to support it, honestly. The algorithms and compute power needed to actually autoroute something useful beyond trivial things is years away, perhaps decades or more.
My experience with PADS/Mentor "blaze router" and "Specctra" (now Allegro PCB router) was very good. Altium on the other hand... no (I mention Altium because I think most people's bad experience is coming from this).
Specctra and blaze worked fine in 1998-era PC hardware. I used them for high speed designs (even then we had ECL and PECL).
Is it Yageo's responsibility to publish a different 0402 footprint for each board house's capabilities?
Capabilities, while not identical, are similar. I use the same 0402 footprint regardless of the board house.
Altium has multiple footprint creation wizards for making footprints, but they are made to your specifications, so that they fot your assembly requirements.
The limitation here is that only KiCad has an open format for design files to begin with. Maybe we should be agitating for a better open-standard for schematic capture? I'd love to be able to output a schematic from e.g. a spice simulation, then import that into my ECAD suite. The netlist (which is part of the Gerber output) is human-readable, so I suppose its possible to extract the schematic from that. But then, it'll be computationally expensive to arrange that information in an easy-to-read format.
It is unreasonable to expect a tool to support the formats of others for export.
Even five figure professional tools only do those exports and then have separate importer plugins. For example Altium Designer recently added a functional kicad importer.
But the DXF stuff? Excellent for integration with mechanical CAD tools and for use with RF simulators like CST or HFSS. QUCS Studio is the odd one out that they support importing kicad layout files into their EM simulator.
The thing is that while the files look similar superficially, LibrePCB has a lot of differing library concepts: https://librepcb.org/features/library-concept/ Just as an example, LibrePCB has UUIDs for _everything_. That makes conversion from/to KiCAD more difficult.
It wouldn’t make sense to add yet another giant parts library to the world of PCB design. Make it easy to import from the major part and footprint libraries found linked from DigiKey.
Don’t try to reinvent the wheel.
> - Is there auto-routing? How good is it?
Autorouting is of very limited value for only certain narrow use cases. Even the high dollar CAD packages won’t route your board for you in a reasonably good way, but they can be useful for routing length-matched buses and such after the user has set up all the constraints properly.
> - "Import formats: DXF". For what, the board outline? DXF is for mechanical CAD. You can't import a board layout or schematic that way.
DXF import is a very common operation in PCB layout, not just mechanical CAD. It’s used all the time to pull in board outlines, important silkscreen items, and other features.
These criticisms are really a stretch for a project like this that is just getting started. If you’re expecting a feature set identical to four and five-figure CAD programs that have been developed for decades then, yeah, you’re going to be disappointed. Can we not just appreciate that this project is ramping up and providing more options?
I think you have forgotten when you were a beginner.
Have been designing PCBs off and on for 20 years. This is what I use the autorouter for. I put together a placement that has logical clustering and flow to it and try running the autorouter. If it has a really hard time with lots of vias, I focus on tuning the placement in that area until it can get a relatively ok autoroute. Then I tear up the traces and manually route. I figure “I can do cleaner routing than the autorouter, but if it thinks the best it can do is 20 vias on this group of traces I don’t stand a chance”
But for the average PCB, which has mix of switch-mode power, analog, high-speed digital, and low-speed digital, it takes longer to specify the constraints so the autorouter can do a good job, let alone wait for it to hopefully complete. So it's rarely used outside of particularly tedious but regular tasks, like hooking up a wide memory bus.
(I do think this is something where AI could make a big improvement. If it could infer most of the constraints from the circuit then it would help with saving time. The challenge then becomes marrying the ML-generated output with the hard constraints effectively)
What would be helpful, however, are some better checking tools. Some mistakes, like running a trace right through the bottom side of a through-hole and creating a short that wasn't there on the schematic, seem very easy to detect and warn the user about before they end up spending hours cutting traces and running bodge wires.
I have not checked if kicad or Librepcb have it, but PADS and Altium do.
I don't care as long as it has the usual industry standard footprints. For anything unusual I can make my own footprints.
>Is there auto-routing? How good is it?
I don't care, I won't use it. It's all garbage compared to what a human can do.
>"Import formats: DXF". For what, the board outline?
Yes, or silkscreen graphics or other unusual copper pours. Some people don't even mount components on the PCB, they use it as an artistic medium.
>"Export formats: PDF, SVG, pixmap, BOM, pick&place, Gerber/Excellon". None of which have enough info for import into another EDA program.
These are the only formats I need.
Been using KiCad but I'll take a look at LibrePCB.
A thousand times this.
There's two kinds of people:
1: Uses library parts
2: Makes their own parts, has been bitten by the library parts being wrong (wrong pinout, footprint size etc)
Side question: Has anyone used Wave Function Collapse for auto-routing?
Apologies if this is a “bad” approach. I have yet to make my first PCB. I’m suggesting it because I’m inspired by the impressive results in the game Townscaper.
I'm curious if that has any implications for future nano-scale tech; we might see an intersection of DFT and electronics design.
One of the main "selling points" is the advanced library concept: https://librepcb.org/features/library-concept/
1) Those who believe in library managers
2) Those delivering boards on a regular basis
The vast majority of time in PCB design is spent reading datasheets. The second largest chunk of time is spent doing the engineering schematic design and analysis. After that is PCB placement. After that is building schematic and PCB symbols. After that is actual routing.
Yes, building library symbols annoys me. It's tedious and error prone. However, it's integral to your design and you can't skimp. The sooner you accept that, that better off you will be.
(A good example is your vias underneath a QFN for power and heat transfer. If your via rules change because you have a different board house, some of your physical symbols may need to change slightly. This sucks, and no library manager is ever going to solve this.)
Library managers for PCB design have all the same pathologies as bug ticketing systems in software development.
Draw the parts. It's not that hard. Don't worry about libraries. Yes, somebody may have done it already. No, that one isn't the same. Just draw it, you have the datasheet. Make the symbol that fits your schematic, it'll be way better than shoehorning in the one you found.
I get it, I'm annoyed every time I have to draw a symbol, but that's just how it is. Every project I work on, I make a new library and draw symbols to put in it. I copy most library symbols I use into it so I can modify them. I reuse my own symbols, but I modify them for the new project. It's a fact of life... embrace it.
I download 99.9% of the symbols I don't already have available locally from online libraries. Why would I draw a symbol for random part when the manufacturer provides one and has uploaded it to all the usual places.
What are the usual places for you? I rarely find proper footprint+symbol on snapeda for example, plenty of plain wrong or subtly wrong are however found on regular basis.
I hope you are doing well! This is Ron Publico from SnapEDA and we want to help you regarding your experience about our footprints and symbol at SnapEDA. May we ask if you can share us more information and send us an email to support@snapeda.com?
Our team is more than happy to help you and investigate those footprint and symbols that you have check earlier.
Kind regards, Ron
For a while, everybody was shipping Altium libraries. This was really good because, as we well know, engineers are lazy. Thus, somebody would simply pack up their internal libraries and ship them. This meant that every symbol had been shipped and tested in a real product. Consequently, the libraries generally didn't have any fatal faults. And you could extract the symbols and make whatever edit you needed to fit into your own library management stuff.
And then Altium decided to enshittify things in order to extract rent from library management. Now, you couldn't extract symbols or footprints from a library, or you had to register with their cloud garbage.
And then SnapEDA and its ilk came along to "fix" this problem that Altium just caused. Except that engineers are lazy. Nobody uses SnapEDA for actual internal libraries for production boards inside the semiconductor companies. Consequently, the libraries have minimal feedback and you have to beg people to send you fixes. Which, of course, they don't do because engineers are lazy.
And don't get me started about the "licensing terms" behind using SnapEDA symbols.
The feedback our users give us is essential, and all our content is created using internal standards developed from the opinions of our community and manufacturers. If you can provide any specific feedback about our parts, please contact us. We'd be happy to assist!
LibrePCB is more simple.
Among the nerds, the backlash has started. Watch out, Fusion 360.
In the world of doing stuff with atoms, no one ever wanted their drafting table to have authentication, ACL, 2FA, or storage/backup.
Like yeah I agree it would be wonderful to have alternatives, but it's a little dramatic to call the existence of this very small project the start of a "backlash"
If this works well I might give PCBWay a try.
I do have the advantage of one lab back in college where a pro spent 90 minutes instructing a bunch of teenagers how to prepare Gerbers for a class project through Advanced Circuits, but beyond that I've had no problems sending files to OSH Park, JLC, PCBWay, Sunstone, or Advanced Circuits whether they were generated in Eagle, Kicad, or Altium.
Even at the low-margin providers like JLC and PCBway they still have a human look over your gerbers (and most provide web viewers for you to see what you've uploaded in those files) to make sure you're not going to order the inverse of your board, or make all your vias unplated, or swap your copper and silkscreen layers, or anything goofy like that. If you do screw up the design, that's on you and the tools won't help, but prices are dirt cheap and turnaround times are screaming fast these days, so it shouldn't be too bad.
I don't understand why newcomers find plotting to gerbers so intimidating.
As my eyes and coordination are not as good as they were hitting buy now and having fully assembled boards come back for basically the cost of the parts and the PCB was game changing for me.
You could always have fully-assembled boards come back for basically the cost of the parts...as long as you were at quantity 10k units. Hooray for automation!
I've only done low-volume hobbyist stuff, & prefer KiCad, but I can see that not having to fiddle with BOM/CPL would be a +1 to EasyEDA.
PCBWay less likely to run into issues with weird design features and parts specs, but they are slower and more expensive.
Elecrow also takes Gerber’s from EasyEDA.
Their website is an atrocity but I guess that's fine.
I've been using them for the last few months and I have no complaints.
PCBway is among the better board fabs in the world - certainly in terms of customer service, and very hard to beat in terms of value for money. The fact that they get you quote and acceptance in under an hour (during US working hours!) is incredible.
American board fabs could learn a thing or two from PCBway. They set a very high standard in terms of service. I’m very impressed by it.
I wouldn’t send a server motherboard or a radar frontend design to them (for a multitude of reasons - ITAR controls likely forefront among them) but most circuit designs aren’t in that league of board design. Most are two to six layers and 300 or fewer parts placed.
PCBway does pretty superlative work serving that niche.
Spoken like someone who didn’t read the comment they’re replying to?
The person you’re replying to said PCBWay was good. Quoting that comment: “they seem to legitimately do a good job” “Quality is as good as you'd want and the price is reasonable.”
Last time I used them their process was so stone-aged that they couldn't do solder mask between the pins of a QFP-64 package
As part of our jobs, our small group of people in their early 20s would handle this inbound phone number for NA and any voicemail that came in after hours. We'd do basic qualification, write up the lead and if it was good pass it to the inside sales rep who managed whatever region it came from.
I remember looking at the license holders and it seemed like everyone had at least a few licenses to that product. Siemens owns all that now.
Curious how PADS stacks up today, if anyone is familiar with the tool.
So it's true value is in large, complex designs with a decently sized team working on it.
That said kicad is catching up to it for all the simpler stuff.
I have high hopes for this one! Hopefully I'll get to work on a hardware project again and really try it out, I haven't had a reason to do any custom electronics lately though, and it's z but expensive and clutter creating to do on a whim very often.
2L->4L may require some retooling, but 4L+ is all the same.
Not simple at all. Switching regulators are sensitive to PCB layout, component selection, and parasitics of the PCB itself. You can’t really treat switching regulator schematics as cut-and-paste building blocks like this because the layout requires an understanding of how the circuit works, where the switching nodes are, and how to organize everything to keep parasitics low.
If you take a random 48V switching regulator schematic and lay it out without understanding these details, you’re likely to blow the switch up from ringing or at least have terrible EMI radiation.
The basic building blocks for beginners would be more like low-speed logic circuits and simple microcontrollers circuits. Jumping into medium voltage switching regulators and battery charging (which can result in fires very easily if you’re not careful) is far from simple.
What it can't do is tell you how to lay out the board to get the result you want. The switching IC datasheets typically have layout examples, and these are sometimes complete nonsense.
As mentioned - most manufacturers have recommended layouts and written layout recommendations: keep your loop small, route things this way, put a via here. If they don't, learn from the recommendations from TI's excellent documentation.
This isn't that hard.
This lack of professionalism is a bit off-putting to me. Just saying, don't put stuff like that on your front page.
(There's some other word choice that's correct and makes sense, but seems a little unusual, that makes me think/supports that.)
Startup looking at a post-layout DFM check workflow: https://cadstrom.io/
Cadence is probably the biggest EDA company talking about ML/AI in the PCB space (that I've noticed) with their recently announced "Allegro X" stuff. The videos are mostly marketing fluff, but they seem to be on track with what I'd expect for "AI assisted PCB design". https://www.cadence.com/en_US/home/tools/pcb-design-and-anal... https://www.youtube.com/watch?v=RlWfSQq0NkA
They also have a neat machine-learning optimization tool for their electronics simulations: https://www.cadence.com/en_US/home/tools/system-analysis/opt...
On the chip-design side of EDA, both Cadence and Synopsys have a bunch of AI-assisted tools that supposedly are being used right now. I'm not as familiar with that stuff so I prefer to read the humorous Deep Chip summaries: http://www.deepchip.com/items/0593-08.html
And lastly, there's some recently published and soon-to-be-published work showing that there's potential to speed up electromagnetic simulations with neural nets. It's all just proof-of-concept for now, but I'm hoping this proves that ML/AI can be can be integrated in a useful manner in commercial electromagnetic solvers :) https://shielddigitaldesign.com/posts/2022/ml-replace-field-... https://shielddigitaldesign.com/posts/2023/s-param-from-via/
Maybe a better approach would be to have an LLM generate RTL code for an FPGA.