Connect with us

Audio Amp

Discussion in 'Audio' started by Mitchekj, Feb 11, 2010.

Scroll to continue with content
  1. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    I've recently found an old speaker lying about, and have it hooked up to my laptop at work. The laptop's speakers are, well, poor. This speaker sounds great (even made a little box for it) only problem is that it's a little low on the volume.

    I've gone through all the windows options and have all volumes maxed out, still just a tad bit quiet from the speaker. So it seems I'd need some type of small amp to get what I want out of it. Problem is, I don't know much at all about audio.

    I'd like to build the amp myself, in part to test out the new "PCB fab in a box" I have. I've measured the resistance of the speaker w/ an LCR, it reads ~7 Ohms, so this would be an 8 Ohm speaker? What kind of power would I be looking for? 10W? Just need a 'little' more boost, and maybe some bass/treble adjustments. I've found plenty of reference designs on the net for all different kinds of amps, just don't know what I need. lol.
     
  2. Resqueline

    Resqueline

    2,848
    2
    Jul 31, 2009
    For office listening you'll be perfecly happy with 0.1W, for workshop levels you'll need 1W, and 10W is practically party level.
    The problem with PC sound outputs is that it's made for 32 ohms headsets so an 8 ohm speaker overloads it, leaving even less power. A 2:1 transformer would set the impedances straight and improve the volume.
    But like you say there are plenty of choices (too many for me to make a choice). Pick some examples for me and I'll yay or nay for you.
     
  3. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    http://www.redcircuits.com/Page33.htm

    That one caught my eye... if it isn't painfully obvious, it's been >10 years since I last studied anything audio electronics related. lol. I can see how the circuit works, but as far as the whole speaker impedance thing works, I'm at a loss.

    Thanks for the help. :)
     
  4. Resqueline

    Resqueline

    2,848
    2
    Jul 31, 2009
    Yes, that one will fit the bill perfectly, and since you want the layout practice it's only beneficial that it's an old-school discrete component amp.
    If you have only one speaker then you'll want to sum the r&l signals going into the amp with a couple of 33 ohm resistors.
    Impedance is as easy as a battery & a load. If you short it real good then the short won't get hot, but the battery will. Not much use in that. But if you load the battery with a resistance ten times higher than the internal resistance of the battery then almost all the power is delivered into the load.
    For antenna systems on the other hand you'll want the load resistance equal to the internal resistance for maximum power transfer. It's "easy" to check with math that it's so.
    Well, no-one can cover it all. I have my own problems with other matters.. :)
     
  5. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    Haha, thanks for that. Makes sense now. Impedance matching, ugh... how soon we forget. I'll go ahead and re-capture that schematic and do a layout, see how it pans out. :eek:
     
  6. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    Well, here's a draft version. I'm not all that experienced w/ doing layouts, but getting better as I do it. :) Managed to get a one sided board, at least.

    So my questions: For audio, does using this large ground plane help keep noise down? Or will it make it worse?
    Have I got all the 'high' current paths taken care of with the larger 50mil traces? (Will be using 2oz. copper, if I recall, may even be 3oz.)

    Thanks for the help!
     

    Attached Files:

  7. Resqueline

    Resqueline

    2,848
    2
    Jul 31, 2009
    Ok, here goes, you better brace yourself.. ;)

    I'd have the track from J2A pass by C8+ before going to J3A.
    The ground plane exits out from C8 are very long & thin, I'd try to expand/ improve at least one of them to at least 50mil.
    Q3 & Q4 should have a b-c-e pin configuration, not c-b-e.
    D1 should ideally be placed so close to Q3 & Q4 that it can be put in thermal contact with their heatsink.
    C3 should physically be placed directly in the path between R4 & R1, not on a track leading off from them.

    Other than that it looks ok to me. I rarely managed to get it right on the first try myself.
    I believe the ground plane is a good idea and that the "high current" paths are wide enough.

    Oh yes, make provisions for summing resistors on the input, you have plenty of room to spare there
     
    Last edited: Feb 14, 2010
  8. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    All points identified have been changed. (Good catch on the CBE/BCE thing, I just relied on Altium's default TO-220 pinout, doh.)

    D1 is going to be one of those little glass passivated DO-35 buggers, I can probably 'glue' or otherwise (VHB tape?) secure it to the heatsink for Q3/Q4, will that work?

    I hope the summing resistors are in order? If you were referring to something else, please do enlighten! :)

    I'll probably end up using the 1/2oz. copper clad board, occurred to me that the small traces may suffer when etching that heavy copper stuff... that and undercutting issues.

    Looks workable?
     

    Attached Files:

  9. (*steve*)

    (*steve*) ¡sǝpodᴉʇuɐ ǝɥʇ ɹɐǝɥd Moderator

    25,299
    2,737
    Jan 21, 2010
    From what Resqueline is saying, it may be better to use a non-smd part and have it mounted so that it can be attached somehow to the heatsink.

    I haven't looked at the circuit (sorry) but I'm assuming it is part of the biasing.

    Undercutting is generally not an issue until the width of the tracks approaches (say) twice the thickness of the copper.

    I've etched tracks 0.2 mm wide without any real issues, and contemplated 0.1 mm between pads of BGA devices (can't report on the success of that yet as although I can design them, they're really hard to transfer to the copper!)

    Having said that, I would rarely use anything smaller than 0.4mm tracks if I can avoid it.
     
  10. Resqueline

    Resqueline

    2,848
    2
    Jul 31, 2009
    Yes that's much better but there's still a couple of issues (one new). ;)
    The C8 ground track is still far too long & narrow. I guess you'll have to try to force apart a couple of the other tracks.
    D1 cathode is not supposed to be connected to Q3 & Q4 emitters, only to R9.
    Yes, it can be mounted a little off the board and just be bent towards the heatsink, just touching is ok, maybe with a dab of heatsink paste.
    Summing is ok. Strange having a default c-b-e pinout on TO-220's, that must surely be corrected in their next version..
     
  11. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    Steve: The kit I have says it can do 6mil, maybe even 4 mil traces... so that's part of this test. :) (0.15mm - 0.1mm) I'm going for 10mil, should be doable. The diode is an axial thru-hole type, too. Just wasn't sure how to get it into good contact w/ the heatsink. If bending it into contact works, then that's sounding like the way to go.

    Resq: Thanks again. Now I see what you're saying about C8's GND trace, I though you meant the relief from the pad (now it's solid.) That makes sense! That and D1. :eek:
    Rev X3 in progress, lol.

    Good thing I always breadboard things before putting copper down, I'm prone to mistakes! Best way to learn though, eh?
     
  12. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    Ok, looks like I may have a handle on this one. I moved some things around to try to minimize track lengths, and to get the ground connections as wide as possible to everything.

    I had planned to use a strip of 1/16" thick aluminum as the heatsink for Q3/Q4, running the length of the board. Isolated electrically from the heatsink with a layer of thermally conductive padding. At first thought, that seems like plenty. Just how much current is going to be flowing, anyhow? They're 3A rated packages, and Vce is 1.2V.. so if they're doing 2A (at full saturation,) that's 2.4W, when less than saturated, well, you get the idea. Warm! Any insight as to what kind of power dissipation they'll be seeing?

    the log pot VR1, all the connectors, and the switch will be fly-wired onto the board and mounted to the chassis, as I've envisioned it anyway. I was going to put it in a small plastic box.

    On the plus side, looks like I have most of this stuff in-house, so I only need to order a few things. Cheap! :) Get this thing breadboarded up and debugged in no time.
     

    Attached Files:

  13. (*steve*)

    (*steve*) ¡sǝpodᴉʇuɐ ǝɥʇ ɹɐǝɥd Moderator

    25,299
    2,737
    Jan 21, 2010
    A few notes on aesthetics. Probably not important for operation, but my collegue always likes to make is boards "look nice". These are some suggestions I know he'd make:

    1) Unless required for some reason, avoid changing the width of tracks. It looks messy. (S1 to C4 and C4 to Q1 (amongst others)

    2) Unless required for some reason, make the tracks slightly smaller than the pads (C3 to R4 he would like, R10 to R11 he would not)

    3) Where a pad is in the middle of a ground plane, unless otherwise required, it makes good sense to have it isolated from the ground plane and connected by a track than it does to effectively place a hole in the ground plane. The reason is that it is easier to hand solder it. An example is many of the connections to the ground plane.

    4) Add the board name, the date, version number, etc. somewhere in the copper. It makes sense if you ever want to create another one, or fix a bug in the layout.

    5) Fill in those large areas of etched board. If you are etching it yourself, it will save your chemicals and speed etching.

    6) watch out for little pointy bits of copper in your ground plane. Any etching under them can result in them lifting and becoming a problem. You don't have any extreme examples, but the there are 2 under the left hand end of D2. I would either move the track to the right a little further away to allow the ground plane to connect fully around the pad, or manually edit this so the points are removed, Looking at them more carefully, they do already have squared off ends, but the one to the left of R6 does not.

    7) there's something odd about the round pads for VR1 They're not chamfered like the rest and the solder mask(?) appears the wrong size on one pad.

    8) there are no holes shown in the pads. My colleague insists that 0.5mm holes in the copper are etched as it makes later drilling easier and far more accurate (effectively acts to centre the drill)

    How are you making the board? The manufacturers claims that you have sound very like those of a certain blue toner transfer material. Be aware that if you're using this stuff that surface preparation is critical and that whilst 0.1mm tracks are possible, they require (in our experience) a 1200dpi laser and almost "clean room" techniques.
     
  14. Mitchekj

    Mitchekj

    288
    0
    Jan 24, 2010
    Sounds advice, thanks. :)

    These are all the little tips and tricks I'm trying to learn. Connecting the dots is the easy part, hehe. The main point of this whole excercise: to get experience with it. As a tech, so far, I've never really had to do any layout or design work. But it does fascinate me, and I can always appreciate a well designed PCB. As you say, they just look good.

    One of the EEs I work with has had some good experiences w/ this particular PCB kit, which is why I got one. He said our printer in Engineering is up to the task. I'm assuming he knows how to prep everything. Another good source of info for me, that guy is.

    I haven't been picking his (or other EEs at work) brain on this board since they probably don't want to spend the time tutoring a nublet, plus I've been doing it at home on my off time. So you guys have been awesome help. :) Thankfully I can take my work laptop home, even put Altium on it.

    Ah, that's the other thing... I installed Eagle on my home computer (it's free, can export gerbers, etc.) but the guys at work said to not even bother with it, learn Altium instead. Any of you guys have experience with this kind of thing? I've been using both, they're pretty easy to learn the basics of, hard to master, I'm sure. Though Altium does seem to have a more professional, fully featured feel to it. I don't think I'd ever shell out the thousands of dollars for it, though. Is something like Eagle a complete waste of time for home use?
     
  15. Resqueline

    Resqueline

    2,848
    2
    Jul 31, 2009
    That should work nice. There are (of course) still a few moves that could be made if you want to nitpick. steve has some of the finer points. Reintroduce ground pad relief.
    I'd move R6 & R9 a bit down on the board, and maybe put S1 vertical. That could allow the ground plane to widen and make a path directly between Q4 & C8, and perhaps extend to fill in the vacant areas too. I don't know how easy it is to "pull" on the tracks in that program to make more room for the ground plane in some spots.
    A strip of aluminum will do the job keeping it cool. I'ts not going to dissipate much. A TO-220 on its own can dissipate 1.5W but that will boil water of course.
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-