am i stupid or diptrace is completely bullshit crap??

[justin66]

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 dissapointed
i have put all the components correctly and here is some pictures for you to judge

[poorchava]

Doesn't matter. Who uses autorouters anyway?

[amc184]

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.

[T3sl4co1l]

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

[rx8pilot]

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.

[amc184]

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.

[justin66]

Doesn't matter. Who uses autorouters anyway?

well 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 from http://www.simprojects.nl/transducer_amp.htm for tda1554q

it 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? 

[salbayeng]

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 the cathode on diodes.
Else pin 1 is the end with the mark, which oddly enough is positive on 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.

[Siwastaja]

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's really important, 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.

[justin66]

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 the cathode on diodes.
Else pin 1 is the end with the mark, which oddly enough is positive on 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.

im 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

[Siwastaja]

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.

[DmitryL]

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 dissapointed
i have put all the components correctly and here is some pictures for you to judge

It looks like it is you And your literacy examples seem to confirm it

[justin66]

It looks like it is you And your literacy examples seem to confirm it

ok 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 jorb 

how can i impruve my current design? btw this trace burnt off


how can i find out where electronics go? i dont know any

[void_error]

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.

[Corporate666]

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.

[BloodyCactus]

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.

[rx8pilot]

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.

I 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.

im 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

Money 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. 

[justin66]

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?

[rx8pilot]

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?

Layout 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?

[justin66]

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?

[rx8pilot]

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?

Google. 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.

[Zero999]

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.

[AndyC_772]

that was all auto lied out and routed except few jumpers thanks for the tips why cant they create one that is good?

There'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.pdf

It'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.

[sleemanj]

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 SES

For 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.

[CatalinaWOW]

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.