Welcome to Solid State Guitar Amp Forum | DIY Guitar Amplifiers. Please login or sign up.

February 26, 2024, 05:53:25 AM

Login with username, password and session length

Recent Posts

 

Rod Elliott's Project 27 and Amp

Started by ghoshsubha444@gmail.com, February 27, 2013, 04:54:55 PM

Previous topic - Next topic

ghoshsubha444@gmail.com

HELLO,

I am currently drawing pcb for rod's project 27mk2. there are few capacitors in the diagram greater than 1uf in non polar which are hard to find in small voltage. so i would like to replace them with electrolytic capacitors. i have edited that image in paint...please verify if their polarity are ok.
Thanks in advance...
Subha

Enzo

Non-polar electrolytics should not be hard to find.

I am assuming you want radial leads or could at least use them.

From Mouser:
647-UVP1H2R2MDD   2.2uf 50v NP  22 cents  5700 in stock.

647-UVP1H010MDD1TD   1uf 50v NP   12 cents   189 in stock

667-ECE-A1HN100UB   10uf  50v NP   19 cents   1934 in stock


Those are just ones I selected, there were a number of options at each value in terms of brand, voltage, etc.


Other large suppliers like Digikey ought to have similar selections.


ghoshsubha444@gmail.com

Thanks enzo for your reply...I am from the other part of the world, India...where i have to rely on my local market. Sad but true...here larger value non polar capacitors are available in very higher voltage values like 300v,400v...which are not only costly but also huge to fit in boards...that's why i have asked here to substitute with polar electrolytic..

So can you please verify whether the polarity of those capacitor are correct or not??(please look at the second picture)....

J M Fahey

Dear goshashuba.
I live in Argentina and have the same problems as you.

*Very* short answer: use standard (polarized) electrolytics.

C3/8/10 polarity is not important.

Just for consistency use C3/8 with negative to ground, and C10 with negative towards R13.
The general rule is "negative towards the point closest to ground and positive towards the IC".

I repeat it, if you have no DC voltage there, it will work the other way, but having a "rule" saves times lost thinking about it.

Symmetrical fed Op Amps have offsets measured in a few millivolts, that's why you can consider them "0".

Now, on the transistor, that's different:
The base needs to be fed some "positive" current (it's an NPN) through R15.
If one end of R15 is grounded, yet it has to be more positive than the other end, it means the other end (connected to base)  has to be "more negative than ground", so you need C15 negative connected to Q1 base.
As of C14 it's easy: Q1 emitter *has* to be 700mV more  negative than base .... which is already somewhat negative by itself, so C14 negative goes to emitter.

I detailed *why* I suggest such polarities so you can determine yourself what to choose in any other similar case.

ghoshsubha444@gmail.com

Dear Fahey

Great explanation...Yes c14's negative should be connected to emitter..Similar to input buffer in microamp....

Thanks

ghoshsubha444@gmail.com

#5
Hello

I have just completed drawing p27 pcb (preamp board) on 1.75"*2.5" board area.
please check my attachments...(pre2.pdf)
I have used trimmer instead of real pot for checking purpose.

couple of questions to ask..
when drawing PCBs i sometimes find free spaces so that i can thicken certain tracks..Is it good to widen tracks unnecessarily (without wasting any extra board area of course! :)). Cause wide tracks are stronger..Which is beneficial for home PCB etching and soldering
For example I am uploading a PCB image from General_guitar_gadget_com. The tracks can be broken any time..  :)

phatt

Hello ghoshsubha444,

I'll assume you are going to hand drill this PCB?

If so,, word of advice;

Although wider tracks will be much easier to work with for DIY builders,, The Pads are the issue not so much the tracks.

Most software defaults to small pads which is fine for a million dollar factory but bound to frustrate those new to pcb building.

So try to find the Global editing menu, some call it DRC (design rule check).
You may find it possible to force larger pads on a lot of components.

Also print out a few track only copys *In actual size* to get a real world idea of how hard it will be to drill pads and leave enough copper to solder the components to cling to. 8|

On screen it might look big and easy to do but too late after you etch it all.

Also remember that for first time pcb makers there is a very good chance that you may want to change a component *After the build* and smaller pads will not like being tampered with more than once.

Re the GGG Dynacomp layout;
I'd steer well away from tracks like that.
Not only are the pads small the tracks are not consistent and go horribly close to other tracks.

Phil.

J M Fahey

Fully agree with phatt, who is very experienced at homebuilding.
Yes, PCB software usually wants to outdo others by saying "*they* put 6 components and 15 tracks inside a stamp sized PCB, *we* put 12 components and 25 tracks there".
Crazy  :duh
And launch the software pre-set for that. :loco

Which is fine to design PC Video boards or Cellphones, but not for brute hairy cavemen (literally) like Rock Musicians.

Pads need to have enough copper around the hole, tracks must be wide enough so hairline cracks (very common in home etching) don't interrupt them, BUT, there's something you missed, they must not be too close either.

As an example, the power tracks you show "inside" the IC footprint are too thick and *will* touch the IC pads.

You'll need to halve most of your tracks, and avoid them getting closer than the free space you now have between IC pads.

To put it into numbers: I usually design with 40 mil tracks, whenever possible I widen them to 50/70 and up to 100 mils (*IF* I have a lot of free space, of course) and neck them down to 30 mils at certain critical points, and only for a short length, such as to pass between 2 components.
And never try to pass a track between IC pads.

Also if you have "free" space you can fill it with "Fills" or "Polygons", but avoid the cheesy "copper pour", so much abused.

Why?
I always see it very poorly used: skinny tracks (BAD) and a too tight *useless* copper pour, good only to save etchant but all that copper serves no useful purpose.

*You* apply "fills" attached to high current or ground tracks.

This is my general purpose 2xTDA2030/2050 amplifier and PSU, single supply to be able to use *any* 12 to 24VAC transformer I "rescue" from a dead amp. or find in a dumpster.

The top overlay and the bottom tracks, ready to laser print and thermal transfer:

ghoshsubha444@gmail.com

Thanks Phatt and Fahey for your reply and great explanations..

I have some experience in etching PCB...

So the summery of the above discussion is too much thin tracks will cause terrible problem for home etching board.

Too wide tracks are not necessary either meaninglessly. The difference between tracks are also an important parameter must be in consideration.

I think ironing image on the copper board weaken the copper layer to stay attached to the board and too slim tracks often wore off..

Now my question is -
Is it bad to have ground plane (not closed:)) ??

please see my attachment of p27 pcb 100% sized image and rate it overall for spacing and widening only..(1 to 10).

Thanks





Roly

Just some general observations.

Hi @ghoshsubha444.  Having done many hundreds of board both professionally and at home I can only agree with @phatt and @JM.  There are a lot of things you can do with a professional PCB maker that you really can't get away with at home, such as tiny pads and running traces between IC pads.

There is no virtue in making traces thin (except where you really have to, and then it's a good idea to see if you can change the layout so you don't need to).  Home builders often get into trouble trying to imitate professional boards by hand, and I've seen home built amps with tiny boards mounted on a huge chassis.  Unless you are tight for space don't worry about making the board a bit bigger so it is more "comfortable" to etch, drill, and solder up.

As a general rule the available space should be reasonably evenly divided between trace width and spacing in between.  Very thin traces can get cuts from stress cracks, over-etch, imperfect resist coverage, dust, (and even once an eyelash on the photographic negative  ::) ).  So in general it is better to err on the side of large tracks than small.

At home I often do boards by hand using a waterproof felt tip pen and the second layout would be much easier to do like that than the first.  You can do things like splay the legs of a transistor so they form a little tripod.  This not only gives you more space to work with when soldering it also supports the transistor better.

One problem with very tight spacing is when you are soldering you get blobs jumping across to other pads where it shouldn't.

PCB layouts are called "artworks" and there really is an art to producing a good layout, but the important thing to keep in mind is what sort of production process the final board will go through; there are a lot of differences between a board intended for one-off home etching and hand soldering, and one that will be reproduced thousands of times and be wave soldered in an automated bath, and you need to be aware of where you will end up right from the beginning of the process, the initial layout.

When you are using artworks from web sites you are often dealing with the output of amateurs who haven't given enough thought to how people, who are perhaps not as skilled in building, are actually going to put their creations together.  If you look at the boards that Heathkit supplied you can see that they assumed the typical builder would be ham-fisted and using a 100W plumbers soldering iron (or maybe a blowlamp  ;) ) and they were big with very generous tracks, pads, and spacings.

So when you are home-brewing, make everything, track width, track spacing, pad size, case size, human scale so it is comfortable for you to build, and later service/modify.  When you want to build your own digital wrist watch using SMD, or transmitters for tracking small animals (as I have), then it is worth the struggle, but otherwise you are only making a rod for your own back.


Specifically, it is more important with a ground plane that it is thick enough to carry the currents demanded of it, than it go right around, and that you don't end up with ground return currents in common with different stages sharing the same track, in fact there may be some benefit in not creating a full loop.  If you look at PCB's from ghetto blasters and home stereos you often find that the grounds from various stages are brought back to the power supply in parallel and connected there, just to avoid this "ground resistance in common" problem.  Home builders in particular tend to underestimate the currents flowing around power supply rectifier circuits, and in output stages, and make the tracks too thin.

I also must say to you that checking a PCB layout is quite a bit more difficult than checking a circuit drawing, and in reality you can't expect that anybody on a web site will check anything but the very simplest of layouts for you - you just have to go over the layout with the circuit next to you and check that every line goes where it should, and nowhere else (or perhaps you have a good friend locally who is also into electronics).  That's one reason why we still call the first power up the "smoke test".  :cheesy:  One trick is to try and re-draw your circuit working only from your layout.

I hope your build goes well for you.   :tu:

If you say theory and practice don't agree you haven't applied enough theory.


phatt

Quote from: ghoshsubha444@gmail.com on February 28, 2013, 02:26:08 PM
Thanks Phatt and Fahey for your reply and great explanations..

I have some experience in etching PCB...

So the summery of the above discussion is too much thin tracks will cause terrible problem for home etching board.

Too wide tracks are not necessary either meaninglessly. The difference between tracks are also an important parameter must be in consideration.

I think ironing image on the copper board weaken the copper layer to stay attached to the board and too slim tracks often wore off..

Now my question is -
Is it bad to have ground plane (not closed:)) ??

please see my attachment of p27 pcb 100% sized image and rate it overall for spacing and widening only..(1 to 10).

Thanks


I assume you mean a loop around the outside? NO steer well away from ground loops.

Go to *Valve Wizard* site and find the pdf on Grounding problems.

http://www.valvewizard.co.uk/Grounding.html

It is all still relevant with SS design.
It's all Valve stuff but actually much easier to grasp the problem when looking at Valve gear.

The issue is power supply current getting into/onto Signal path.

Just hold an electric guitar next to a big transformer and listen to the HUUUM. That should give you an idea of what you want to avoid in PCB layout.

i.e. Don't run the High current power rail next door (parallel) to a sensitive audio input.
If you must, cross them at right angle .

Re heat from iron;
No! If your iron De-laminates the copper from the board then you have purchased crap PCB.

I hold the iron on for 1~2 minutes and I press hard.
I use glossy magazine paper which comes off in warm water in around 5 minutes of soaking.

Don't forget to set your laser printer to max ink density so you get max ink onto the board other wise it won't work well. 
Phil.

bobhill

Having etched quite a few boards in my time, I have never delaminated the copper from the board, and like Phil, I use a lot of pressure for a couple of minutes. The heat from the iron has a lot to do with how easily the image transfers. When I used photo paper, I cranked the iron to the max. With PNP blue, a lower temperature makes excellent transfers. Too high a temp with the PNP will make it smear. Then after transferring the artwork, I compare every track to a copy of the drawing I print out on transparency so it can be overlaid with the board and any necessary corrections made. And like Roly, those corrections are made with a permanent marker, in my case a Sharpie very fine point industrial waterproof marker.

Of course, after etching comes the inspection with magnifying glass, and meter check for shorts between traces. Then drilling with bench top drill press, compare to the transparency for missed holes, go drill that last one I missed, populate and solder away.

The only thing I can see from scaling up from pedals to amps is to have a very good idea of your current flow through the different circuit building blocks. Power and ground traces need to handle everything you throw at them, so size them accordingly for the main power busses. Pre amp components draw in the mv range (and micro amps of current) so those traces can be smaller. Power amps deliver a lot of voltage and current, and in a lot of SS amps I have seen, the traces will be accordingly larger.

Have fun, just don't get so lost in the project you forget why you are doing it.

ghoshsubha444@gmail.com


phatt

Why Yes,  We do carry on a lot don't we?  :lmao:

Tiss all good because others read this as well and often some gems of advice are hidden in details,,, as I have found myself.  :dbtu:
Phil.