TDA2030A single-supply high-power amplifier
I built the single-supply high-power amplifier from the ST datasheet for the TDA2030A. I stuck with the reference design but replaced the BD907/BD908 transistors with TIP35C/TIP36C transistors and switched the power supply capacitor from 2200 uF to 4700 uF.
The first iteration of the PCB had oscillations, but the revised layout seems stable. I've tested it with a 4.5 ohm load and a 31 V DC input voltage. It swings about 26V peak-peak with this power supply before clipping. Sound wise, it seems fine, but I don't have the equipment to measure distortion.
This was primarily to practice PCB layout, so I'm sure there's plenty of room for improvement.
thanks I have been looking for one of these.
are those huge resistors really needed and if so how many watts are those?
The blue resistors for R6 and R7 are 5 W in the photo, but I replaced them with a 1 W resistor, and that seemed fine. On the scope, I saw about a 1V drop max across the 1.5 Ohm resistor. R8, the pink resistor in the photo, is rated at 2W. When I put some test signals through, it didn't heat up when going to 20 khz, so a 1W would probably also work here.
However, when the test signal got close to 100 khz, it started to heat up substantially.
If you're going to be using audio signals, 1W should be fine, but be careful about putting higher frequency test signals through it.
You will want your speaker/output ground (R7, Q2, D2, C7 gnds) to use a separate conductor, to go back to the star ground after the last power supply reservoir capacitor. Also, the power ground (C5 and C3 gnds) should go back separately (or maybe with the speaker/output grounds) from the audio signal input ground reference (C4, R2, C2 gnds).
The main thing is to have the input section's ground be separate from the rest of them, all the way back to the star ground point. Otherwise, the voltages induced across the inductance (and resistance, to some extent) of the ground-return conductor itself will distort the input signal.
Also, the power and speaker ground will need a WIDE trace, all the way to the jack or terminal block, and heavier wire than the input signal ground return.
Ideally, you would want the input signal and input signal ground, from the RCA plug, to stay extremely close together (tightly twist the two wires, all the way from the jack to the board), and then keep the input ground trace extremely close to the input signal trace, all the way to the chip. You should spread the input ground around and under all of the input components, if you can't use a two-sided board. Then you want a separate signal ground wire to go from the board to the star ground at the PSU output. Note that the input RCA jack should not be electrically connected to the chassis, or to anything else except the signal and signal ground from the source and to the board. Otherwise you would have a ground loop, i.e. a big antenna for hum.
Also tightly twist every pair of transformer wires, ALL the way to both ends (3 or 4 turns per inch). And keep the pair of connections from the rectifier to the caps extremely close together everywhere, too.
Any space between ANY pair of conductors makes them a better antenna.
Also remember to keep your small-signal conductors as far away from any large or dynamic currents (e.g. AC or outputs) as you can.
Any passive component that connects to an active component (chipamp or transistor) should be mounted RIGHT AT the pin. Leaving any empty trace length next to a chip or transistor pin is really asking for trouble, like instability/oscillation, due to the parasitic inductance of the traces.
Your Zobel network should be connected as close to the last active device's output as possible, and should go directly to its ground, or the speaker ground, which should also be as close to the active device as possible.
The power decoupling caps (C5 and C3) should be connected as close to the point of load as possible. The smaller-value decoupling caps should be within a millimeter or two at the most, of the device pin, and should go directly to its load ground. Otherwise, you might have instability/oscillation. I would think that C5 and C3 should be as close as possible to Q1, with a separate +V wire to the power supply. That +V wire should also feed the chipamp's +V at pin 5, which should have another set of decoupling caps (maybe at least a few hundred uF up to 2200 uF, plus a small one in parallel and very close to the pin) from pin 5 to the output side's ground.
i.e. I would break the +V wire, on the schematic, between R1 and C3, and connect the cap gnds to the right of that point to the power/output ground, and also have a separate +V wire to the power supply for everything to the right of that point. Then I would add at least a small electrolytic cap, i.e. where R1 connects to +V, and connect that cap to the input side's ground.
Keep input side ground and output side grounds completely separate, on the PCB, and run a separate wire for each, all the way back to the star ground point near the last PSU cap's ground.
Thanks for the helpful feedback. I'll take them into consideration if I have time to do another rev of the board.
I did some frequency response measurements, attached are the results. This was with my 31 V linear regulated power supply and near clipping into a 4.5 Ohm dummy load. I calculated the dB as 20*log(voltage/max voltage)--is that the correct formula to use?
Here's another revision based on gootee's comments. Changes include:
* Separated signal and power/speaker ground
* Added C9 and C10 to pin 5 of chipamp
* Moved C3 closer to Q1 emitter pin
* Made the board size a bit smaller (now 1.7 x 4 inches)
* Removed on board connector pads for input--input will now need to come in through a header or air wires
* The cross hatch pour is unconnected
Vs is shown jumpered to R1 on the board, but it could be provided by a separate wire from the power supply.
The unfortunate thing about this layout is the jumper between the collectors of Q1 and Q2. I couldn't come up with a better way to connect them.
Is this an overall improvement in the layout?
I also found that the output capacitor C8 and input capacitor C1 are causing the rolloff in the low frequency response. Replacing C8 with a 4700 uF capacitor and C1 with 1 uf capacitor reduce the rolloff.
I also will be building this amp this is my diagram that i will be work with only two things have me goin in circles here WHAT THE HELL ARE C3 AND C7 please help
I believe that C3 is a bypass capacitor to smooth out high frequency noise from the power supply. C7 and R8 have lower impedance as the output frequency increases. Effectively, this limits the high frequency output to the speaker (it goes through R8 and C7 instead).
C3 is to create a low impedance before C5 starts to go inductive.
C7 is to put R8 into the load at higher frequencies for stability of the amplifier.
thanks for the info now what do ask for when go to purchase this since in the diagram i don't see a positive or negative i think its not just a regular capacitor so if i can get a pic so i can see it well that going an make it so much easy for me
i hav a few of these tda2030a i pulled out of a old home theatre system an being it was made in china it also had sum generic ones to the part # d2030a but i might only use these to first try an make a functional amp and then swap it out after also in the theatre only half of the parts i need i can see the rest i can't figure out how they used it hope to get more help me
can you tell what each capacitor are here and voltage
this is my first chipamp my first diy project i don't know much but i do hav a good idea so can you give me the voltage of each capacitor and exactly what its is i am going to ask for when i go to the electronic parts store please
|All times are GMT. The time now is 01:58 AM.|
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2013 DragonByte Technologies Ltd.
Copyright ©1999-2013 diyAudio