am i stupid or diptrace is completely bullshit crap?? - Page 1
Forum section: electronics / projects

author: justin66
author_rank: Regular Contributor
timestamp: March 03, 2015, 07:11:22 am
content: ok so i did everything as their video tutorial suggested using diptrace and it is so bizarre i did proper circuit and did auto routing and that fucking diptrace routed some caps +'es to ground point and i figured that out after drilling 100 holes eching it tin'ing copper with solider because i didnt had liquid tin and also putting all components in when i powered it everything one trace burnt. what a fuck man?im so dissapointedi have put all the components correctly and here is some pictures for you to judge

author: poorchava
author_rank: Super Contributor
timestamp: March 03, 2015, 07:13:40 am
content: Doesn't matter. Who uses autorouters anyway?

author: amc184
author_rank: Regular Contributor
timestamp: March 03, 2015, 07:19:09 am
content: Well, DipTrace is a pretty decent CAD tool, so ......Seriously though, it looks like your PCB pattern wasn't correctly applied to your schematic's symbol. It looks like the symbol's positive pin was assigned to the pattern's negative pad, and vice versa.Aside for that, the layout is very bad anyway. There are times that autorouters are useful, but your board isn't one of them. A PCB this simple should have been laid out by hand.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 03, 2015, 07:22:31 am
content: So you didn't double-check the footprints and pins before using them?Step 1. ALL libraries are crap.Fortunately, it looks like C1 isn't even affected (I'm guessing the voltage is small, and certainly low current), so really you only boned one. And it can be assembled "backwards", so your board isn't even a waste!In fact... looking more closely, why are C1 and C10 the only ones affected? If computers make mistakes, damnit, they make the same mistake over and over again! All the other polarized capacitors appear to be the same symbol and footprint, but correctly pinned. You sir made a mistake somewhere, and it was inconsistent to boot! And now you rage at yourself in front of the vastness of the Internet. How does that make you feel?Tim

author: rx8pilot
author_rank: Super Contributor
timestamp: March 03, 2015, 07:32:00 am
content: Software does not make PCB's....people do. As you gain experience, you will never trust the software and use your own intuition to hunt down little details. If it is backwards, it is your fault unfortunately. I'll bet you won't let that slide again, but there will be more sneaky things out there.As Tim said, ALL libraries are crap. They work as a starting point, but you have to verify each and every one or this will repeat itself over and over.

author: amc184
author_rank: Regular Contributor
timestamp: March 03, 2015, 07:34:31 am
content: Here's the screen you screwed up on. If you go back to your design, you'll find that the symbol's pins aren't attached to the pattern correctly.If you come back with a few more details on your design, we may be able to help you make it into a functional layout.

author: justin66
author_rank: Regular Contributor
timestamp: March 03, 2015, 08:27:15 am
content: Quote from: poorchava on March 03, 2015, 07:13:40 amwell i thought that man dont has to do it anymore. im super wrong here. its actually my first pcb i had experriance before but its my first experriance with using any layout program. how do i impruve my circuit? and is it any good? my goal here is to have one tda power two small subs driven with low pass filter and other tda power two 8ohm speakers.circuit is fromhttp://www.simprojects.nl/transducer_amp.htmfor tda1554qit took me couple hours to layout all the components am i suppose to put traces too? how can i do better than auto router? i mean it looks good to me but its definetly looks crap for experts like you please at least show me a path. i could have made double sided pcb but i was scared that i wont iron paper to pcb correctly.why on the world there is librarys if its crap?

author: salbayeng
author_rank: Frequent Contributor
timestamp: March 03, 2015, 08:37:07 am
content: I don't use diptrace, but I'm pretty good with Protel.It's a common problem with all circuit layout packages.It's up to you to check the footprint matches reality.Basically pin1 is always thecathodeon diodes.Else pin 1 is theend with the mark, which oddly enough ispositiveon tantalums and other polarised capacitors.With SMD parts for example, the SMA diode package and the Tantalum size A are near enough interchangeable, except pin 1&2 swaps over.Pin 1 when looking at a component package on the screen is always on the left (or top), pin 1 when loading from a piece of cut tape is nearest the sprocket hole, i.e. on the right (or top) .Just wait till you get to connectors, pin 1 can be on left or right depending on manufacturer.With a Dtype connector pin 1 swaps from left to right for male and female.I got caught out so often with diodes that I made my own symbols and named the pins K and A.When you read a data sheet double check the numbering used by looking at the picture. The 78L05 in a TO-92 can be numbered 123 or 321.Watch for SCR's they usually have the gate at the opposite end to a bipolar or MOSFET.And when powering up a circuit, wind the voltage to no more than 5v, or stop when it gets to 20mA, then run around with a meter , checking what you thought was positive is actually positive.

author: Siwastaja
author_rank: Super Contributor
timestamp: March 03, 2015, 08:52:36 am
content: You are indeed super wrong about autorouters. They are for professional use, for those who know what they are doing, in some limited situations. Sorry, no luck there, you just don't draw a schematic and give it to an autorouter like that. And autorouters need configuration, too.Routing a PCB is both science and art. It's not trivial. It takes time. Learn it! I really enjoy it, but there is some learning curve involved, but you'll never get there without actually doing it by hand. Circuit layout is a super important circuit "component" itself! It's not just there to connect the components; it has parasitic elements that seldom are negligible. You need to think about the physical (electrical) properties when doing it, so it's not only a logical puzzle how to do it in smallest size and least vias/layers/jumper wires/whatever. Physical properties such as: capacitive coupling of signals, stray inductances of power and ground, bypass capacitor locations, etc. Even something as simple as trace widths to carry the required current.Many beginners seem to make the mistake of thinking that autorouters are handy for them. No way! For a beginner, I could even recommend the exact opposite; don't use the strict schematic-netlist workflow at all. Draw the schematic by hand, and start laying the board from scratch. This will keep you focused on trying to understand what your PCB is going to do (and avoid the mindset that you are just mechanically solving a puzzle of mapping the schematic on PCB). I still mostly use this workflow, but I might be a bit crazy. (I still use CIRCAD 98 as my CAD, even with its severe limitations, but I really like the simple no-bullshit flow; it's more like a drawing program with some PCB CAD features.)I totally hate playing with broken/poor software (and "management" side of things), because they alienate you from what'sreallyimportant, which, in case of designing a PCB, is, well duh, designing the PCB. But I love drawing, the actual art/science part, because every line matters. So I always just start doing the layout, throwing in components as I go.

author: justin66
author_rank: Regular Contributor
timestamp: March 03, 2015, 08:53:29 am
content: Quote from: salbayeng on March 03, 2015, 08:37:07 amim reading this and i feel so bad because i dont have money. my psu is old pc power supply ny solidering iron is even a station its just connected to mains plug and i dont even have a drill i had to borrow it. i wish i had tools you guys have

author: Siwastaja
author_rank: Super Contributor
timestamp: March 03, 2015, 09:03:18 am
content: You can do pretty well without a lot of money, in fact, being cheap sometimes gives better learning experience; you'll need to improvise. For example, need a current limit for your PSU? How about starting with a series resistor. Use a multimeter to measure voltage across the resistor. Solder a bunch of diodes to drop the voltage. Look for places where junk electronics go. Desolder yourself a good collection of eco parts. Benefit? You will be exposed to commercial designs. You will subconsciously start to learn how a proper PCB looks like, what kind of components they use, etc. Start analyzing these designs. Then start repairing stuff... Many hobbyists and professionals have started this way, with very little money, and only got "good equipment" after they are already pro enough to be really able to use that equipment.

author: DmitryL
author_rank: Regular Contributor
timestamp: March 03, 2015, 09:13:13 am
content: Quote from: justin66 on March 03, 2015, 07:11:22 amIt looks like it is youAnd your literacy examples seem to confirm it

author: justin66
author_rank: Regular Contributor
timestamp: March 03, 2015, 11:03:18 am
content: Quoteok as someone mentioned i did common noob mistake and thought that autorouting will do the jorb the main purpose trying pcb designing software was autorouting tool i thought it will take off part of the jorbhow can i impruve my current design? btw this trace burnt offhow can i find out where electronics go? i dont know any

author: void_error
author_rank: Frequent Contributor
timestamp: March 03, 2015, 11:13:05 am
content: I've been using DipTrace for a few years now and I must say that the libraries it comes with are not that good. For caps I usually use one from the Symbols library and then manually attach a pattern. NEVER forget to double-check everything. Also, for home-made PCBs I change the pads for most THT components with 0.1in pitch to 1.8mm with 0.3mm hole which makes drilling easier. Autorouting can be quite useful when you set it up properly but I only used it to give me an idea how to route traces for more complex designs, then I manually routed everything. Never watched a DipTrace tutorial. My only problem is that it doesn't have shortcut keys for flipping components in the Schematic Editor.One suggestion would be to spend more time editing the schematic, so it looks neat and tidy, no overlapping components or component designators/values. You'll also need more grid sizes / trace thicknesses. You can add more from View -> Customize Grid / Route - Trace Templates.

author: Corporate666
author_rank: Unknown
timestamp: March 03, 2015, 04:31:51 pm
content: 1) The program should get it right... you should be able to rely on the libraries, but you have to always check it. When you become more experienced with layout, you will see some things that jump out to you as being wrong. It's MUCH easier to see what is wrong when you have a logical and clean layout than your layout (sorry, don't mean to pile on but the layout is terrible).2) Don't worry about not having good equipment. I used one of those all-in-one kids toys things from Radio Shack when I was starting out. I used that for years! And a plug-in soldering iron. Better tools make things easier but only when you already know what you're doing. The tools don't make you more knowledgeable.3) As for layout, there are a lot of videos on Youtube. I think Dave did some too. It's largely art and experience, but you want to put related parts close to each other. Things that wire to lots of stuff are better in the middle. Power and ground is better going in one area. If you have inputs and outputs, it's better to have input on the left, output on the right - that sort of thing.And absolutely forget about the autorouter - I haven't used one in 10+ years.

author: BloodyCactus
author_rank: Frequent Contributor
timestamp: March 03, 2015, 06:02:20 pm
content: anytime I use a part from the diptrace libraries I copy it into my own library and double check it all and only use whats in my own parts library from then on.

author: rx8pilot
author_rank: Super Contributor
timestamp: March 03, 2015, 06:23:30 pm
content: Quote from: BloodyCactus on March 03, 2015, 06:02:20 pmI do the same in Eagle and it has kept me out of trouble. After only a few components, you get pretty quick at verifying and modifying the parts. Then you have a verified and non-verified library.Quote from: justin66 on March 03, 2015, 08:53:29 amMoney will not fix your problems. Time and discipline will. I started with ZERO, literally a soldering iron and a hand held DMM. I now have a very capable lab and just purchased a pick and place machine. I spent more hours studying, learning, and breaking things than I could keep track of. One thing I never focused on was the limitations of my tools. I was using freebie layout software, salvaged components, modified power supplies from unknown sources. I was still learning at warp speed.limitations of libraries and auto-routers became clear very quick, but it forced me to learn how to do it myself. The auto-router does not know how your circuit works, what currents traces need to carry, or how to keep delicate analog signals from being damaged by a clock signal etc.You have to learn how to do it. No way around it. Money and software will not make up for a lack of understanding.

author: justin66
author_rank: Regular Contributor
timestamp: March 03, 2015, 06:25:17 pm
content: well as i was suggested to check things out im completely raging i was checking traces and think what i have found. within 4minutes including numbering ic's pins i found few errors like lm 358 2nd pin goes straight to ground or +12v i cant remember but its not like that in circuit it shouldnt even touch any of those rails with out other component if my memory is good and now im completely understand why one of the traces burnt but now im pretty confused because it made connection that shouldnt been a thing so my new question is should i even use any of the software? i mean its neat and clean bur beside that it feels worthless can you please tell me what are you using that software for?

author: rx8pilot
author_rank: Super Contributor
timestamp: March 03, 2015, 06:29:30 pm
content: Quote from: justin66 on March 03, 2015, 06:25:17 pmLayout a PCB with pen and paper and then do one with software. You will soon know what the software is for. It's a tool. You don't expect a screwdriver to to turn screws automatically right?

author: justin66
author_rank: Regular Contributor
timestamp: March 03, 2015, 06:33:05 pm
content: that was all auto lied out and routed except few jumpers thanks for the tips why cant they create one that is good?and how about complicated boards like for example pc motherboard its multilayer and super complicated i couldnt believe its man made is it? and also how mutch time does it take than for for example just to recreate rapberry pi from a circuit? and also howbdo i do double sided board at home with ironing paper to pcb and so on?

author: rx8pilot
author_rank: Super Contributor
timestamp: March 03, 2015, 06:38:07 pm
content: Quote from: justin66 on March 03, 2015, 06:33:05 pmGoogle. Large PCB's done by career PCB designers 'may' have some sections autorouted as a starting point. The designer will then adjust to make it actually work based on experience and understanding the circuit function. Laying out a power supply is VERY different than a high speed digital circuit.

author: Zero999
author_rank: Super Contributor
timestamp: March 03, 2015, 09:05:04 pm
content: Another thing you should learn from this experience is the need for protection against over current.How did you power this circuit?Was it from a bench top power supply or a car battery?For test purposes I suggest you use a current limited lab power supply to power the circuit with first. You can initially set the current limit fairly low to only provide the quiescent current. If it immediately starts current limiting then you know you have a problem.Then when you've got it working, you should consider the power supply you'll be using. If it's from a car battery, there should definitely be a fuse. If it's from a switched mode power supply which is current limited, that's good but you may still want to have a smaller fuse on the lower current parts of the circuit as the short circuit current could be very high.Another possibility is PTC resistors (also called pollyfuses/switches) which have a low resistance in normal operation but increase in resistance rapidly when the current rating is exceeded. The advantage with a PTC resistor is it resets when power is removed and it's cooled down.

author: AndyC_772
author_rank: Super Contributor
timestamp: March 03, 2015, 09:24:24 pm
content: Quote from: justin66 on March 03, 2015, 06:33:05 pmThere's approximately one vaguely useful auto router in the industry, and that's the Cadence PCB Router, formerly known as SPECCTRA.Have a read of this data sheet:http://www.cadence.com/rl/Resources/datasheets/7432_PCB_Designs_FINAL.pdfIt's for Allegro, which is one of a very small number of properly grown-up PCB layout packages. Chances are your PC was designed with it. And yes, boards like that are almost exclusively routed by hand.

author: sleemanj
author_rank: Super Contributor
timestamp: March 03, 2015, 10:24:19 pm
content: The DipTrace libraries that come with it are large, but not brilliant, however the DipTrace library management, component and pattern editing systems are quite brilliant indeed. As a result, it's best to make your own components, either from scratch, or by copying an existing component and/or pattern into your personal library(ies) and modifying to suit, as time goes by you will make yourself a nice little library suited to your particular needs and preferences, and seldom have to go hunting for the right component. Incidentally, this is true for most any software of this type.As for autorouters, this is a religious argument if ever there was one!Some people will say "never use an autorouter", some will say "always use an autorouter", some will say "autorouters are only for amateurs", some will say "autorouters are only for experts", some will say "autorouters do a terrible job", some will say "autorouters do a better job than humans", some will say "autorouters take longer to setup than routing yourself", some will say "autorouters save you huge amounts of time" etc.... polar opposite opinions.I tend to the opinion that the autorouter is a tool, and tools are made to be used, but you don't use a tool without knowing how to use it and what the problems inherent in the tool are. Route important traces, critical areas, things you care about manually. Ensure your net classes, via sizes, trace sizes, clearance matrix etc is all setup correctly, create route keepout areas as appropriate for your purposes, and then run an autorouter. When the autorouter is done, clean up after it, there will be things you can see can be improved, so improve them, a good autorouter won't actually make an electrical connection mistake, but routing is more than having the correct electrical connections.The autorouter you use is important as well, the one built into DipTrace isn't terrible, but FreeRouting is better ( download binaries of last release here:https://www.eevblog.com/forum/chat/freerouting-is-gone-creator-was-bullied-by-zuken-to-take-it-down/msg461993/#msg461993) , in DipTrace File > Export > Autorouter DSN, load that into FreeRouting, autoroute it, save the ses file from FreeRouting and then in DipTrace File > Import > Autorouter SESFor me, routing is quite annoying, frustrating indeed, I hate routing, I would rather the machine do it where possible. I also do not enjoy climbing mountains and would rather fly a helicopter to the top. In both instances, other people would claim the opposite, but it doesn't make either position invalid.

author: CatalinaWOW
author_rank: Super Contributor
timestamp: March 04, 2015, 12:44:26 am
content: You ask why libraries are not good. It is a LOT of work to get them right. There are literally millions of parts out there, many with subtle differences from what seem to be the same part. Add this to the fact that a large library seems to be a marketing point (or to put it onto the customer side, something that people look for when they buy). So all of the CAD vendors throw user contributed parts, elderly parts and so on into their libraries. It would seem that a large user base could correct a library over time, but it doesn't turn out that way. Some of the reasons it doesn't is that not all users are equally diligent in getting parts right, some users require unique modifications to a part to deal with their fabrication process, and sometimes packages change over time.The advice you are getting is good. It is the advice given to users of high end, high dollar programs, to public domain software and everything in between. It comes from countless times finding that a library part is not what you want it to be. Sometimes wildly different, sometimes just a little. It isn't every part, but my experience is that no PWB has ever come to fruition without at least one correction to a library part.

author: Siwastaja
author_rank: Super Contributor
timestamp: March 04, 2015, 05:01:28 am
content: Quote from: sleemanj on March 03, 2015, 10:24:19 pmI have actuallyneverseen or heard anyone say anything among those lines (unless clearly trolling), but I have seen it a lot in meta contexts like yours here. But setting that aside, it seems to me that instead of polar opposites, there is quite a strong consensus on autorouting. Of course, the degree it's dismissed varies; some people think that it's completely useless, while some people just make the point of being careful and doing important parts by hand. But these are not opposite IMO. It's like "lose weight - don't eat candy" vs. "lose weight - keep yourself a candy day, but not too often". They are not opposite; the point is the same.Would it be nice if we had a perfect autorouter with artificial intelligence? I don't know. I have never wanted one, because I love doing the layout and in my books, doing the schematic (and keeping it absolutely perfect and in match with the layout) has been the tedious, do-not-want part (drawing every single bypass cap manually? On chips which have dozens of separate vcc/gnd pins? really? Those schematics are usually hard-to-read for human.). I would like an auto-schematic from layout! That would be an equally hard challenge to program right.

author: Corporate666
author_rank: Unknown
timestamp: March 04, 2015, 05:21:43 am
content: Quote from: justin66 on March 03, 2015, 06:25:17 pmWell, don't take this the wrong way - but when someone says "the program made a connection it wasn't supposed to", it reminds me of the tech support calls I occasionally get from my 70 year old aunt who will say "Windows just deleted all my pictures!". If she gets too insistent on the matter, I'll say "so, do you think there are a whole team of programmers at Microsoft whose job it is to occasionally make Windows just delete random stuff to frustrate users? Or... do you think maybe you *inadvertently* did something to delete those pictures - or maybe didn't delete them at all, rather just moved them?"In other words, Diptrace or any other tool doesn't put parts on the PCB and randomly connect them. It could be that the original library is wrong. Such errors are somewhat common (especially since parts change a lot faster than the libraries can keep up with), but it's much more likely you did something wrong in your use of the software that caused the issue.I'm not trying to bash you - but lesson learned... it's very important to check your PCB's, especially when you are just starting out. I always generate my gerbers and look at them in Pentalogix or GC-Prevue (both free tools). I've done probably 200+ PCB's and I still find errors in my final gerbers. As a novice, it's 10 times more important for you to be quadruple checking yours (as well as your PCB layout compared to your schematic).

author: salbayeng
author_rank: Frequent Contributor
timestamp: March 04, 2015, 06:38:46 am
content: Hi Again.There always people out there to help you.Post the nearest city to you on the forum, and maybe someone can point you to a local fabricator/engineer.I started off at ~ age 10, dumpster diving at radio repair shops to get parts, then you get to know the guys at the repair shop, (they used to put the good stuff in a cardboard box ina corner of the dumpster where I would find it!) , and they'll give you all sorts of broken stuff to examine / dissassemble, and there are a lot of guys out there with sheds full of perfectly good through hole and leaded parts that are just not needed any more.Try to find a local ham operator, most areas have "hamfests" or equivalent, it's a yearly bazaar of electronic cornucopia.My first multimeter (48years ago!!) was a tiny 20kohm/volt moving needle meter. My first power supply was a tri-ang model railway controller with a big rheostat. My first transistor was a BC108, (metal can style) it arrived in its own brown paper bag, cost me $1 (about 2months pocket money) and I picked it up at another local radio repair shop, and made great friends with the technician there.For your first assembly efforts you should be using veroboard (stripboard) this teaches you some good layout skills, being constrained to work in one direction. So all the copper goes east west, and all your links go north south. The double row TDAxxx don't fit very well on veroboard, unfortunately.As to your design efforts ,It looks like you are using a single sided PCB, autorouters will turn these into a bowl of spaghetti. Anyway, follow the guide below and you will improve your circuit immensely(a) Looking at your schematic , C6 c7 c8 c9 actually have the positive the wrong way around on the schematic, so these may actually be the right way around on the PCB.(b) Determine which way the "grain" of the schematic runs, in you case it's horizontal and runs left to right. Rearrange the parts on the schematic so they are not all tangled , and you have done this.(bb) check your grid is set to 0.050" (or 0.025") with visible grid of 0.100"(c) note which are the "bus" signals, e.g. +12 and gnd and the two nets running across the top. The bus signals will go all over the place and be the hardest to route, Generally you would run the gnds below all the IC's and the +12v above them. This also means that in general , capacitors will have the positive facing up.(d) put all the parts on the blank PCB in roughly the same position as they are on the schematic , i.e so J2 on the left ; U3 in the middle , U1, U2 on the right , move J2 to the right, next to the power amps.(e) align the parts (i.e. spin them around) so that pin 1 of U3 is top left (i.e. notch to the top) , and the heatsink of U1/U2 faces outwards (this should put pin 1 at the top??)(f) Parts with gnd at one end should initially be aligned north south with gnd at the bottom, parts that connect to a pin should be horizontal and placed near that pin (try 0.3" away initially) like C4, C2, R1R6C3C6,C7,C8,C9 , this should give you a neat row of parts either side of U1. R3 will probably be up the top, above the notch(g) turn on the rats nest mode, grab a part and wiggle it around to see which position gives nice horizontal lines, align all the parts neatly so that the rats nest are straightest over all. and all the parts are on the 0.100" grid(h) double check the pots, make sure they are grouped sensibly and you can get a screwdriver to them.(i) Now lay down a thick ground track (100 mil) as a straight line from left to right about 1" below U3 . Laydown a thickish (50mil) track for +12 from left to right about an inch above U3. You can attach one or two parts to these buses, but don't do the rest just yet, but keep thinking how are you going to get tracks to them later.(j) You will have a bunch of easy connections- don't do them yet! Find the nets with multiple connections these are more difficult , the nets of pins 1, 6, 7 of U3 will be most difficult , so start partial track laying with these. At this point it should be obvious which parts need moving around, fix them.(k) as a single sided board you will want to be laying tracks on the bottom layer, and these should bepredominately horizontal.(l) when you need to go vertical (ie to bridge over some tracks) swap to top layer, go vertically an integral number of grid units (0.1") and pop back again . You will need to drill the vias and place links at these positions. You can also use horizontal links (but vertical ones are most useful).I'll repeat that - most of your tracks go east west , the remainder on the "other side" go north south , you can route ANY board using this algorithm.(m) when you have done all the hard ones, go back and fill in the easy ones, and rearrange the power buses a bit.(n) when finished review the whole layout, you will find a few places where you can remove the top layer links and use a more convoluted track. Try to avoid using a link to join a ground that splits it into two subnets(o) at this point double check things like capacitor polarity. and the power pins to all IC's.(z) Don't forget a mounting hole in each corner , put these on a sensible grid like 1.500"inches or 50.000mm , allow a big enough space around screwhole to get the screw head in.And you are done!