Hey Guys,
I've just put together my first PCB and I was wondering if there was anything major I've missed or messed up. It's all working on a beard board and in still laying out the power regulators and supply on a separate bread board. This board contains -> TL071 Buffer -> LM1875 -> Output Mute relay controlled by a 555 timer. Pots and LED's are all of board hence the pads.
I've tired to keep all power on the bottom layer and signal on the top, but there are short vias here and there to get over tracks. the Audio and Power grounds will be star grounded.
Anything of major concern here?
I've just put together my first PCB and I was wondering if there was anything major I've missed or messed up. It's all working on a beard board and in still laying out the power regulators and supply on a separate bread board. This board contains -> TL071 Buffer -> LM1875 -> Output Mute relay controlled by a 555 timer. Pots and LED's are all of board hence the pads.
I've tired to keep all power on the bottom layer and signal on the top, but there are short vias here and there to get over tracks. the Audio and Power grounds will be star grounded.
Anything of major concern here?
Always have a look at the component placement during layout to get the shortest tracks. Example, if you move r8-10 c13-14 a little down, you can put c10 above r8, with shorter tracks. Same with c8, put it left of u2.
I'll be sending it away. Any particular reason I should or shouldnt?
Yeah I was thinking I'll need to optimise it a fair bit further. Apart from that would there be any major cause for concern? Also is there a specific limit everyone uses for track length?
In this case, add top and bottom ground planes on the entire PCB. You could also stitch them together as a good practice, but in this case you only have THT components so it's not necessary. Also, I would space the tracks a bit more (for example the tracks between U3 and R8). As e general rule, you can use components to route tracks under them (especially with THT components). I believe you could do that with the components around U3 (C10, R8 etc) and reduce some track lenghts.
Not in this case I think. But sensitive and/or high frequency pcb needs quite some attention. And it just look better when it is tightly. Like c1,c2, c6 and c7, rotate them 180 degrees.
Although it is not completely clear to me how your heat sink is mounted, it appears it might be resting on the PCB. If so, do not rely on the solder mask to act as an insulator. Best practice would be to move all conductors out from under the heat sink, or place a suitable non-conductive material between the heat sink and the PCB.
Yeah i wasn't sure on the ground pours on the signal layer as I know it can act like an antenna for EMI.
I'll go and redo it tonight with the tips above and repost. Thanks so far!
Looking pretty good for a first layout but I think you should take your time and move things around a bit.
I see at least little things you could do to shorten tracks. Maybe you can even omit some of those vias where you change layers.
Take C6&C7 for example. If you turn them (together) 180° so that C7 ends up on top it makes tracks shorter.
This might or might not have an effect but I always go for shorter and more direct tracks.
Function over form without going overboard. It is kinda nice if resistors etc are lined up a little.
I find that placement more often than not is what feels like 80% of the work but also fun.
Look at your current state of placement and imagine the tracks.
Sometimes you need to connect all the tracks now and then to see if you´re there already.
(quick routing with 1mm tracks or so)
Quite often I realize I need to go back to a different placement; if not I clean up the (quickly routed) tracks and make them nice.
Grounding is important of course and voltage supplies should have bigger tracks (at least partially) or even polygons.
You used the thinnest of tracks for your supplies which is something I definitely would want to change.
Here is one I had in my Kicad-folder for inspiration (not mine):
LM1875 amp
Looking closer: You bias your opamp TL071 at 5V which should work but I´d use the +32V, maybe regulate to 24V or so and then use that for the supply voltage of the opamp (it can do up to 30V).
You can take the +24V and bias the input of the TL071 with two resistors at 12V. Just an idea; then there would be no need for an external 6V&12V.
hmmm, i'm keeping the 32 and 16v for the widest output range with my lm1875, but i guess i could go 16 and 8 for the tl071 which means i could lose one of the rails. thanks for the idea 🙂
Just with the supply tracks, I've got them as the thicker traces on the blue bottom layer. Is there something ive overlooked?
Forgot: Grounding sure is a whole big topic in itself but for starters I would try and not interrupt the ground plane as heavily as you do.
Think about the ground pin of the lm1875 and its way back to the main capacitor. There are bottom tracks in between that prevent direct current flow. I think you can put some of those tracks on the top layer.
You could try and move c12 a little to the right and c14 to the left and get a direct ground path.
Think about the ground pin of the lm1875 and its way back to the main capacitor. There are bottom tracks in between that prevent direct current flow. I think you can put some of those tracks on the top layer.
You could try and move c12 a little to the right and c14 to the left and get a direct ground path.
Looks quite good to begin with, that said above suggestions will help improve it.
After you got it more or less where you want it to, leave it aside and forget it for a couple days, serious 🙂
Then look at it again with fresh eyes, you´ll most certainly improve one little bit or two you hadn´t noticed before.
As of heatsink insulation, if screwed to the board which adds significant pressure and considering it sharp edges, which can even have burrs, I suggest you cut a slightly larger insulation material rectangle , even humble cereal box cardboard will do but if getting some stronger fiber material even better, and use it as an insulator/separator between heat sink and PCB surface,
As said above, solder resist is thin and easy to cut through by metallic edges.
After you got it more or less where you want it to, leave it aside and forget it for a couple days, serious 🙂
Then look at it again with fresh eyes, you´ll most certainly improve one little bit or two you hadn´t noticed before.
As of heatsink insulation, if screwed to the board which adds significant pressure and considering it sharp edges, which can even have burrs, I suggest you cut a slightly larger insulation material rectangle , even humble cereal box cardboard will do but if getting some stronger fiber material even better, and use it as an insulator/separator between heat sink and PCB surface,
As said above, solder resist is thin and easy to cut through by metallic edges.
After taking the suggestions onboard (Excuse the pun 😉) heres round 2. a few components shifted around and the top signal layer has received a ground pour too 🙂 It felt much easier after moving components about.
Again. any feedback welcomed 🙂
Cheers!
Again. any feedback welcomed 🙂
Cheers!
To quote myself, ahem, I was thinking C14 is your main filter capacitor for the +32V so forget what I wrote there.
Looking better now.
The tracks on the top layer look pretty thin to me.
Especially from the output where is much current flowing. Make them 3mm wide or even use polygons.
Here is a nice example how to use all that copper you got:
Modulus
Its nice you have separate audio and PWR ground but there is no filter capacitors; I guess you have a separate PS.
The PWR ground on the bottom is pretty much blocked by all sorts of tracks which renders it not so low inductance.
Fortunately the GND on the top layer is OK for output and LM1875.
You could enlarge that GND polygon on the top layer so it fills around your connector on the right.
A bit better than just that single thick track.
I personally would put R9 much nearer to the IC as this is the feedback path.
Use thicker tracks also (1mm or so to make them less inductive; I try to use 1mm throughout actually, power and output much bigger where possible).
You could move C11 down a bit and put R9 there (180°) and connect with a small trace through legs 1+3 of the LM1875.
Some people go as far as just soldering it directly to the pins of the IC from the bottom.
No, I have no affiliation with Tom but you could read this for inspiration:
Taming the LM3886
There is obviously lots to PCB layout and you could easily get lost especially here in the forums.
Many threads about PCB layout and grounding!
Here you also see another nice example of a well-made layout for a chipamp:
open source layout
I use these PCBs and they are not only public but also real good.
Observe the use of polygons/wide tracks for the power&output.
The (low level) input side of the circuit has its own GND plane, only to connect and meet with the "dirty" ground later,
Taming the LM3886
There is obviously lots to PCB layout and you could easily get lost especially here in the forums.
Many threads about PCB layout and grounding!
Here you also see another nice example of a well-made layout for a chipamp:
open source layout
I use these PCBs and they are not only public but also real good.
Observe the use of polygons/wide tracks for the power&output.
The (low level) input side of the circuit has its own GND plane, only to connect and meet with the "dirty" ground later,
Awesome, Thanks this has been a really good learning experience so far 🙂
As for clearance between tracks and pads is there any distance I should follow to avoid issues?
Member
Joined 2009
Paid Member
You may want to add resistors to ground to the output after the output capacitor so that the dc level is well defined. Possibly on the input jack too. Do you have fuses in the power supply? if not, could be added on-board.
Also, add your name to the board, this is no time to be modest!
Also, add your name to the board, this is no time to be modest!
Long story short is I'm using a SMPS going into a board with LM317T's and other filtering on it (because of "silly" local laws about wiring anything 240v). Witrh the output resistor would that be just to "bleed" off any residual DC that leaks through the cap?