checking if there are any issues with pcb layout (update to previous post)

[snow123]

previous post

its been awhile, but i finally finished making a new PCB for my "tube booster" (its basically a tube screamer modified to be strictly a clean boost/eq pedal). all of the signal traces are .012", and most of the power traces are .016", and there are 2 ground planes; 1 on top, and 1 on the bottom.

are there any issues with the layout?

board


top ground plane (eagle doesnt let me export a pic of the bottom plane)
schematic (for some reason it wouldnt let me upload the schematic on here)

[duck_arse]

SCALE YOUR CIRCUIT DIAGRAM before it eats the entire world's bandwidth, please!

I went to look at it to see why the two leds were facing the same way, D1 and D2, but ran screaming when the image locked-up my browser.

welcome back, snow.

[AtomicRob]

It's a little hard to tell without the ground planes showing, but it looks like you have a lot of traces top and bottom - how chopped up are the ground planes, and how are the top/bottom planes connected? I'm admittedly not an expert but for that reason I try to keep things as simple as possible, and for me that usually means routing most of the signals on top, and only routing on the bottom where I can't avoid crossing traces, and then one star ground or simple (unfragmented) ground plane on the bottom. In the layout you shared I see many of the bottom routes aren't actually crossing any top routes, so if those were moved to the top you'd probably have a more continuous ground plane on the bottom, and not need two ground planes. With two planes or fragmented planes, I'd be worried about having loops or inadvertantly creating an antenna.

[snow123]

It's a little hard to tell without the ground planes showing, but it looks like you have a lot of traces top and bottom - how chopped up are the ground planes, and how are the top/bottom planes connected? I'm admittedly not an expert but for that reason I try to keep things as simple as possible, and for me that usually means routing most of the signals on top, and only routing on the bottom where I can't avoid crossing traces, and then one star ground or simple (unfragmented) ground plane on the bottom. In the layout you shared I see many of the bottom routes aren't actually crossing any top routes, so if those were moved to the top you'd probably have a more continuous ground plane on the bottom, and not need two ground planes. With two planes or fragmented planes, I'd be worried about having loops or inadvertantly creating an antenna.

well i try to have most of the traces that (if they were on the bottom) would be covered up by the pots, on the top (so that they're easier to access), and have (most of) everything else on the bottom. hope that made sense.

[snow123]

SCALE YOUR CIRCUIT DIAGRAM before it eats the entire world's bandwidth, please!

I went to look at it to see why the two leds were facing the same way, D1 and D2, but ran screaming when the image locked-up my browser.

welcome back, snow.

how do i do that? also, thank you for catching that error, its now fixed.

[Kevin Mitchell]

SCALE YOUR CIRCUIT DIAGRAM before it eats the entire world's bandwidth, please!

I went to look at it to see why the two leds were facing the same way, D1 and D2, but ran screaming when the image locked-up my browser.

welcome back, snow.

how do i do that? also, thank you for catching that error, its now fixed.

Export or edit for a lower resolution. Thing's MASSIVE!
Anyways, you've come a long way, man. I'm impressed!

Did you run the DRC to check against design rules?
You probably didn't set any but it will at least check the basics (shorts, unconnected wires and so on) comparing against the linked schematic.

Curious, what's with the 3 different styles of resistors? 1/4w, 1/8w & SMD 0805.
What was the thought behind this?

[ElectricDruid]

Personally, I'd probably double the widths of all the tracks. You don't *need* to from a current handling point of view or anything, but thicker tracks are more robust and don't lift off the PCB so easily if they get overheated, and don't get damaged so easily if you scrape them with the end of the soldering iron and so on. And since you've got absolutely tons of space on that PCB, why not?!? You could probably double the widths on all the existing tracks and run the DRC and still get no errors without even having to reroute anything at all.
That said, there's plenty of professional boards around here that use narrower tracks than I do (lookin' at you Aion!) and no-one moans at them about it!

+1 agree what Kevin said: You've come a long way in a short space of time. Nice work!

[snow123]

SCALE YOUR CIRCUIT DIAGRAM before it eats the entire world's bandwidth, please!

I went to look at it to see why the two leds were facing the same way, D1 and D2, but ran screaming when the image locked-up my browser.

welcome back, snow.

how do i do that? also, thank you for catching that error, its now fixed.

Curious, what's with the 3 different styles of resistors? 1/4w, 1/8w & SMD 0805.
What was the thought behind this?

the reason that R100, R101, R102, and R8* aren't 1/8w are:
R8* is an SMD because it is optional (im probably not gonna use it, but options are nice), and because the 1/8w package wouldn't fit there (plus the SMD package fits perfectly).
and R100-R102 are 1/4w 'cause the spacing lines up nicely with C101 and D100.

hope that made sense

[snow123]

SCALE YOUR CIRCUIT DIAGRAM before it eats the entire world's bandwidth, please!

I went to look at it to see why the two leds were facing the same way, D1 and D2, but ran screaming when the image locked-up my browser.

welcome back, snow.

how do i do that? also, thank you for catching that error, its now fixed.

Export or edit for a lower resolution. Thing's MASSIVE!
Anyways, you've come a long way, man. I'm impressed!

Did you run the DRC to check against design rules?
You probably didn't set any but it will at least check the basics (shorts, unconnected wires and so on) comparing against the linked schematic.

just downscaled the image, and added a pic of the top ground plane.

thank you!

i did run the DRC, and there arent any issues, but i wanted to check with you guys to see if there's anything that could be improved upon.

[snow123]

Personally, I'd probably double the widths of all the tracks. You don't *need* to from a current handling point of view or anything, but thicker tracks are more robust and don't lift off the PCB so easily if they get overheated, and don't get damaged so easily if you scrape them with the end of the soldering iron and so on. And since you've got absolutely tons of space on that PCB, why not?!? You could probably double the widths on all the existing tracks and run the DRC and still get no errors without even having to reroute anything at all.
That said, there's plenty of professional boards around here that use narrower tracks than I do (lookin' at you Aion!) and no-one moans at them about it!

+1 agree what Kevin said: You've come a long way in a short space of time. Nice work!

could parasitic capacitance or crosstalk (or anything like that)become an issue with larger traces?

thank you!

[snow123]

but yea, larger traces definitely arent a bad idea, especially considering that i havent done much soldering recently, and am pretty rusty lol.

[snow123]

how does this look?


most of the signal traces are about 0.024", and some of the power traces are 0.032" (most of them are 24mils though). but there are some tighter fits (like the OUTJ, +9V, and VR/N$11 traces) where i had to make the traces 0.020".

[ElectricDruid]

could parasitic capacitance or crosstalk (or anything like that)become an issue with larger traces?

Not really at the sort of frequencies we're talking about for audio. It's perhaps not a great idea to run long tracks in parallel, but that doesn't generally happen anyway. Fat tracks are a good idea, but fat gaps are a good idea too. More space between tracks is going to decrease crosstalk and capacitance. I generally try to keep everything a *long way* from the maximum tolerances specified by pretty much any modern PCB house. 6 mil minimums are pretty common, but you can double it and you won't find it limits your PCB designs. While running tracks between IC pads is useful for microprocessor stuff and designs with a lot of logic, I've done plenty of pedal and eurorack PCBs and *never* had to resort to that! And if you avoid tricks like that, you simply *don't need* those tight tolerances.

[snow123]

how does this look?


most of the signal traces are about 0.024", and some of the power traces are 0.032" (most of them are 24mils though). but there are some tighter fits (like the OUTJ, +9V, and VR/N$11 traces) where i had to make the traces 0.020".

anyone?

[niektb]

Thicker traces are definitely an improvement! I see you've snugged those resistors (and some capacitors as well) really tight together, even though you don't need to. Spacing them apart will make assembly a bit easier.
I would increase the Width and Isolation of your polygons as well! (I normally use 12~14mil for both values).
Also a tip for the future, if you try to layout a board that's more dense: try to have your vertical traces on top and the horizontals on bottom (or vice versa, doesn't really matter). This works because the speeds are not so high and it helps you avoiding a lot of puzzling and a lot of vias
Stitching vias are also generally a good idea to connect your ground planes properly together, be sure though to adjust your DRC settings so they get covered by solder mask (tab Masks > Limit > 14mil or something like that)

[ElectricDruid]

I agree too, I think the new version with thicker traces looks much better.

[snow123]

Thicker traces are definitely an improvement! I see you've snugged those resistors (and some capacitors as well) really tight together, even though you don't need to. Spacing them apart will make assembly a bit easier.

any ideas what specifically i should space apart? 'cause i feel the same way, but there doesnt seem to be quite enough space on the board for me to space certain things apart.

[snow123]

Stitching vias are also generally a good idea to connect your ground planes properly together, be sure though to adjust your DRC settings so they get covered by solder mask (tab Masks > Limit > 14mil or something like that)

what does it mean to stitch vias? and how do i do it?

[snow123]

im assuming i place a couple vias wherever there is missing coverage from the ground plane, and the name those vias "GND". and thats it?

[niektb]

Thicker traces are definitely an improvement! I see you've snugged those resistors (and some capacitors as well) really tight together, even though you don't need to. Spacing them apart will make assembly a bit easier.

any ideas what specifically i should space apart? 'cause i feel the same way, but there doesnt seem to be quite enough space on the board for me to space certain things apart.

For example: R1&R2&R3. C8&C9. R9&R10&R11. But there are more.
You have plently of space sir Doesn't have to be much really. Just 1 (or maybe 2 if you can manage) grid step (assuming you left that on default, that would be 1.27mm) is enough

im assuming i place a couple vias wherever there is missing coverage from the ground plane, and the name those vias "GND". and thats it?

Totally correct! And as tip: place 1 via and rename it, then COPY it to place it elsewhere. Otherwise you have to rename every single via individually