6 ms·
The usual questions: - How comprehensive is the part library? - Is there auto-routing? How good is it? - "Import formats: DXF". For what, the board outline?
by Animats 3y ago
The usual questions:
- 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."
- Alupis 3y ago> Is there auto-routing? How good is it? 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.
- fnordpiglet 3y agoNewbies probably value it as it’s a feature newbies use. Newbies are people too. (Disclaimer: I’m a EDA newbie myself, so I value it)
- stvltvs 3y agoIt's been a long while since I've designed PCB, but doesn't auto-routing provide a good starting point that the designer can refine? I remember it reducing a lot of grunt work.
- Alupis 3y agoIt creates more problems than it solves for anything but very trivial layouts. 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.
- aswanson 3y agoAdc near a switching power supply made me lol. Some guy at a previous gig did that with 190v pwm motor drives. No autotouter in the loop. Just a bad human.
- dragontamer 3y agoRats nest is good enough IMO. Just saying "Pin#20 needs to be connected to Pin#88", with a visual indication that they're not connected yet, is plenty. A Rat's nest is more than enough to figure out which parts need to be placed next to each other, at least for beginner boards with like ~50 or fewer components on them (and maybe ~100 or less nets/traces to manage) 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.
- CamperBob2 3y agoPlacement is usually as important as routing, if not more so. At the same time, the act of thinking carefully about placement will often making routing easier. I try to take a holistic view -- I don't see routing as grunt work, or as an unnecessary chore, but as part of the design process. 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.
- dragontamer 3y agoUnless ML tools know which nets have how much current/voltages on them, as well as which ones are sensitive to noise... as well as rise/fall times of each pin, its a hopeless job. 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.
- CamperBob2 3y agoThe tool will have access to the same data sheets and SPICE/IBIS models that you do. It will know what to do. Eventually.
- dragontamer 3y agoAre you going to put the source-code of your programs in there too? I'm not sure how a ML model would ever know that... say... Pin A5 is a rarely-changing GPIO that's effectively DC. Or that Pin-B6 is configured as an analog-DAC in this particular application (and therefore slowly changing). 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.
- gaze 3y agoProfessionals _do not_ use it. It’s not helpful. If you get your placement right, routing won’t be so bad. If you get your placement wrong, the auto router WILL land you with an awful PCB
- stavros 3y agoAgreed, I wouldn't use autorouting, it's really hard to get right and thus it has invariably mediocre results. Plus, I like routing by hand, it's calming.
- ajsnigrutin 3y agoBecause professionals use expensive professional software, and even a newbie wants to put an esp32 and 4 sensors on a pcb and order 5pcs from china for a price of two cups of coffee... and an autorouter is very helpful then, because for such a usecase, the routing is the 'hardest' part of the pcb design.
- noncoml 3y agoEven a newbie will outgrow the auto-router very very fast. Tools to help with high speed are much much more important
- ajsnigrutin 3y agoWell yeah, but there's a greater chance that s/he'll start using the software in the first place, if it has autorouter :)
- slabity 3y ago> Why do people always ask for this? It's a feature only newbies use 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.
- Alupis 3y agoI don't think that's a fair position to take. PCB design is complex - there are very few complex tasks that can be whittled down to a single click of a button with good results. 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.
- deepspace 3y agoIt's been 30 years since I was working closely with PCB designers, but back in the day, the professional CAD folks would absolutely run the autorouter first, and then use that as a starting point to tweak the layout. 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?
- syntheticgate 3y agoI'd suggest design complexity has scaled at a faster rate than the autorouting tech. In a closer-to-DC world years ago, optimal routing was nice but often not a requirement. In today's high-speed designs, proper routing can be the difference between working and not working, and there is a constant battle of constraints and trade-offs that humans can deal with more effectively. Attempting to constrain a complex design such that an auto-router can be successful can often result in an over-constrained problem which then makes the auto-router unsuccessful. 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.
- noncoml 3y agoCouldn’t agree more. Auto routing is useless. Give me tools to make it easier to route pairs and for length matching.
- petsfed 3y agoThis alongside the question re: DXF really reveals the inexperience of the question asker. 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.
- phendrenad2 3y agoYou clearly aren't a retrocomputing hobbyist, so you aren't in the know. Trust me, autorouting is essential for some use cases, and it works great for those applications.
- sweetjuly 3y agoWhat's so special about retrocomputing that makes it more tractable for autorouting? Autorouting isn't a thing in industry for PCB design because managing EMI for modern ICs is so challenging. Is retrocomputing able to get away with it due to slow rise times on very old chips?
- phendrenad2 3y agoExactly, EMC is only really an issue above 50MHz, much higher than most retrocomputers were capable of.
- bogantech 3y agoThe issue is not the frequency of your signals but the edge rate.
- phendrenad2 3y agoThat's... not entirely true actually.
- LIV2 3y agoI am, and I have made a few popular designs. 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?
- phendrenad2 3y agoYou'd route 100+ signals by hand on a two-layer board? You either have too much money or too much time.
- dbrgn 3y ago> How comprehensive is the part library? 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.
- ShadowBanThis01 3y agoAlong those lines: Does anyone know what the best way to contribute to these projects is, among those offered? I will go to extra effort to avoid fees being imposed on the recipient of the money.
- dbrgn 3y agoI assume you're talking about https://librepcb.org/donate/ https://librepcb.org/donate/? Probably GitHub Sponsors (no fees at all) or OpenCollective (fees depend on the payment method, a "platform tip" is optional).
- ShadowBanThis01 3y agoThanks! That is what I meant, and also for future reference on other projects.
- Findecanor 3y ago> DXF is for mechanical CAD. You can't import a board layout or schematic that way. 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.
- SV_BubbleTime 3y agoYou kind of can in KiCAD. You import to a footprint, and change the lines to the type you want (courtyard, silkscreen, front copper, etc), and for things like pads you can use DXF for reference and centerpoints then put your pads in. 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.
- junon 3y agoDXF was integral in importing things from freecad for outlines, designs, and in some cases even silkscreens. 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.
- jhallenworld 3y agoYou need to try a better autorouter. 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).
- polishdude20 3y agoI wish parts manufacturers could create an open or universal part file standard. Even just a schematic symbol and footprint would do. Make it compatible with all PCB eda software
- petsfed 3y agoThere's a lot of good reasons why its not universal. Chief amongst them is that there's no guarantee that a given footprint will work in the context of the overall assembly. Will you get tomb-stoning? Will the combination of fab capabilities and assembly capabilities necessitate a larger aperture for a given pad? If so, will that cause the solder to migrate during reflow to an adjoining pad? Is it Yageo's responsibility to publish a different 0402 footprint for each board house's capabilities?
- stonegray 3y agoBy this logic, EDA software shouldn’t include any footprints at all Capabilities, while not identical, are similar. I use the same 0402 footprint regardless of the board house.
- RF_Savage 3y agoAnd it is why many professional one's don't. Altium has multiple footprint creation wizards for making footprints, but they are made to your specifications, so that they fot your assembly requirements.
- rcxdude 3y agoTBH, you should treat them as if they don't ("size of part library shouldn't be part of the evaluation, let alone top of the list of "standard questions"). And generally external libraries are suboptimal as well, for various reasons. What I want is tools for quickly importing and generating footprints, like Altium's generator (and support for mechanical dimension constraints like mechanical CAD has had forever would really help. It boggles my mind that no PCB tool has them, it would be such a killer feature)
- petsfed 3y ago>"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. 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.
- RF_Savage 3y agoUsually the other programs have specific importers for other tools. 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.
- dbrgn 3y agoHow is the KiCAD format more open than LibrePCB? Both are custom formats using S-expressions. The thing is that while the files look similar superficially, LibrePCB has a lot of differing library concepts: https://librepcb.org/features/library-concept/ https://librepcb.org/features/library-concept/ Just as an example, LibrePCB has UUIDs for _everything_. That makes conversion from/to KiCAD more difficult.
- adhesive_wombat 3y agoThe default generic output standard these days is IPC-2851 (which is basically the same as ODB++ but managed by the IPC consortium).
- Aurornis 3y ago> - How comprehensive is the part library? 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?
- BMc2020 3y agoAutorouting 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. I think you have forgotten when you were a beginner.
- skupig 3y agoHave you? I routed my first board a year or two ago and found pretty quickly that autorouters suck even at simple tasks. The only way to get usable results is to simplify with smaller autoroute jobs and better placement, at which point you could easily do it by hand anyway.
- tonyarkles 3y ago> simplify with […] better placement 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”
- madengr 3y agoComprehensive part libraries are not an issue. It just needs a basic set of symbols. Most people doing PCB design will create their own symbols and footprints. Altium has an excellent footprint generate, which you can then tweak the output.
- leptons 3y ago>How comprehensive is the part library? 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.
- bogantech 3y ago> >How comprehensive is the part library? > I don't care as long as it has the usual industry standard footprints. For anything unusual I can make my own footprints. 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)
- leptons 3y agoAnyone technical enough to contemplate making a PCB using discreet components or anything more than a "dev module" should already be capable of designing their own footprints.
- joshspankit 3y ago> auto-routing 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.
- the__alchemist 3y agoWith PCB design, you can work at a few abstractions above that. For example, nets, and the various abstractions used in electronics (resistance, capacitance etc). Even for RF and high-speed designs, I don't think that's an appropriate granularity to model the system with. I'm curious if that has any implications for future nano-scale tech; we might see an intersection of DFT and electronics design.