TDA7294 PCB - Needs Checking

Status
Not open for further replies.
Jump to Latest
W

Wizardmaxx

Member
Joined 2009
#1
HI

I have been messing around with Eagle and do not profess to knowing what I am doing, but have below a pcb for a TDA7294 that I threw together. It is the standard circuit from the datasheets with a minor mod to the input and a bypass of the mute and standby circuits.

Any help checking for errors or a better layout as far as signal / power tracks would be appreciated. I was also unsure on the signal gnd as I have read that this should be seperated from power gnd by a 'resistor ?' if memory serves me correct

Many Thanks

Wizard

URL]
 
#2
Long traces - susceptible to interference and crosstalk. Try and shorten the feedback circuitry. even the point you're tapping it from needs to be evaluated, it should not be from a branch off the main output terminal, it needs to be as physically close as possible.

Try and compress the circuitry to use more of the horizontal space - the more vertical it becomes, the longer the traces get.

As to the grounds, it would be better to have a single trace to both the ground pins, instead of a thin one and a very fat one. See where the ground currents are flowing - there is no high power ground current flowing through the chip. You have to treat it as a signal ground, and resist the temptation of hooking components into the nearest ground path.

I would use the shortest possible distance between power ground and the speaker ground, and the shortest possible traces to the power supply pins. Remember the 7294 can pass up to 10 amperes, long traces present sufficient impedance to create problems with current delivery.

If you aren't too squeamish about it, I would actually solder the feedback resistor underneath the board, between pin 2 and pin 14. That is the best possible way to create a short feedback loop. This will also simplify your PCB to a large extent. I would use the right side of the board for power and speaker, and the left side for signal entry. The ground can be connected through a low value ~1 ohm resistor, but it is not strictly necessary - though a resistor will definitely make the routing easier, and a jumper can be avoided as the ground entry pins are to the opposite side of the power pins, where you will typically get the ground from.

The mute and standby circuit can be kept at a further distance from the chip. It is simple DC biasing, and does not need to be in proximity. the power supply buffer caps need to be very close to the chip, and they also need a small value ceramic cap in parallel for HF stability and properly decouple the inductance of the supply leads. These two can be also soldered under the board and are power bypasses, so should be tapped close to the power or speaker ground and not signal ground path.

If you are having problems, you can think of intelligent ways to use the NC pins to create more routing possibilities. Personally, the TDA7294 is on the borderline of my list of chips suitable for P2P wiring because of its mute/stby circuit and the requirement of the bootstrap cap, but it can still be done.
 
#4
Looks nicer. I'll wait for the real experts to comment, my one additional suggestion is to move the output terminal to the right-hand edge of the board, somewhere near the bootstrap cap next to the chip. The ground run can be taken from there, near the cap on the -rail. This would make the output trace even shorter than it is currently.

Ditto for the input, it can be moved right next to the input cap and the ground can be just next to it as well. Looks good enough as it is, but this would be worth a shot if you still have time to get it done.

That way the front of the board can be used only for power input.

I see you've knocked the NC pads right off the board, I presume you'll cut the pins off/ What I actually meant was to use those pads and pins to make the routing easier, for example the ground pins on the signal side or the supply pins, but this looks good (though a little convoluted - but I guess it'll be fine).
 
#6
Better - now one last (!) thing 🙂

Is it possible to simplify the traces from pin 2 and the feedback resistor and cap? The journey looks a little long-winded.

I would move the resistor up near the chip and use it as a jumper to cross some of the tracks you're having issues with. the cap can also be moved up and the ground traces also be slightly improved (short/straight).

The caps associated with mute/stby are not critical, so you can relocate them a bit or orient them one above the other (instead of side-by-side) like the PSU caps. Or you may slightly increase the horizontal size of the board to get some more space. I would also route the ground for those two caps from a separate path from the power ground, instead of hooking into the signal ground. Ideally signal ground should be connected to only three points: The input resistor, input ground from RCA socket, and the feedback R/C. For chips which require a signal ground connection, it can be the fourth node. This ground (ideally, a single point) should then follow a single, untapped path to the power ground.

I'd wait for a few other posters to comment as well. Good luck 🙂
 
#7
Thanks Again Sangram.

Your comments have been very useful. I have changed three of the resistors to 'upright' and included a jumper for pin 1.

Now that the layout is just about there it is time to check for errors. I have changed only the input capacitor from 470nF to something a bit beefier, otherwise the topology is the same as the datasheet.

URL]


URL]
 
#8
Looks good - debugging would be a little easier with the component markings on the overlay, but it's still cool 🙂

And would it be possible for you to post a pdf or mail one to me pls? I'd like to pinch it, thanks 🙂

Looks like it won't blow up, everything seems to me in the right place, and it looks (IMO) a lot better/more compact than the first attempt. I'd say it's good to go, personally speaking.
 
#16
Wizardmaxx said:
Hi livenicely

It is a single sided board. It has options as far as the earth layout goes, but that's all.

Wizard
Click to expand...

ohhhh my mistake. so much sorry. i have just read top.pdf and bottom.pdf and be worried but not read ur lines. so much sorry. its really good and wonder full.thank u so much. can u plz suggest me that which paper is good to transfer image on board butter paper or just 80 gram printing paper or a piece of news paper. thank u so much for pcb again
 
#17
My bad

Don't use the mirror of the PCB bottom as it is already mirrored as you can see from the first board I built. Turn it arournd and the the input will be on the right hand side. 🙁

I only picked this up when I made a second board and was going to transfer a silk layer on.

I will put some new attachments once I have sorted it out.

Wizard
 
#20
Here is the schematic of the inverting configuration.

URL]


The board layout for the inverting board has a huuuuge cap on it at 37.5mm pitch and 42mm length. Take that into acount when drilling.

Also the pdf for the non-mirrored layout is at 2x size.

I will be making a new layout for the non inverting with a modified stby/mute setup if anyone is interested.
 
Status
Not open for further replies.
Top Bottom