a few PCB design questions (expressPCB)

[EnnPeeEff]

Hi guys, just two quick PCB design questions...

-What sizes are appropriate for ground, power, and signal traces?  On the expressPCB site they list how much current a given thickness can handle but I really don't know how much juice is flowing through a standard 9v stomp box.  The pedal I'm doing the design for isn't anything fancy, 4 transistors and some caps.

-Does anyone know what the hole size is on perfboard that smallbear sells?

Thanks so much!

[a soBer Newt]

A boss Boss PSA-120S is 150mA.  I would flood your ground then you don't have to worry about it.

[EnnPeeEff]

A boss Boss PSA-120S is 150mA.

That's a good way to think about it, thanks. 

I would flood your ground then you don't have to worry about it.

On a two layer board how would you set that up?  Ground on one side power and signal on another?  I've used plenty of boards with ground planes, but never though about how to implement it.

[a soBer Newt]

On a two layer board how would you set that up?  Ground on one side power and signal on another?  I've used plenty of boards with ground planes, but never though about how to implement it.

Yeah that is how you want to do it try to keep all your signal and power on the top layer and only go to the second layer if you have to don't want to be cutting up your ground plane. What are you laying out?  Who are you going to get your boards made by?

[Processaurus]

I run 30 mil traces for ground and power, unless there is a layout problem and they have to neck down.  It's less about current handling (analog effects take so little) as having a lower resistance path for those nets.  It's generally nice to have big fat traces for ground, in particular.  A ground plane counts.

[bhill]

A boss Boss PSA-120S is 150mA.  I would flood your ground then you don't have to worry about it.

And has nothing to do with how much the pedal draws. A four transistor circuit (Big Muff, huh?)  running off 9vdc probably only draws around 10-15 ma at maximum. Usually the indicator led is the highest draw in the circuit. The current rating on a power supply only indicates how much current that supply will source at maximum, but it will only source as much current as the circuit draws.

[EnnPeeEff]

What are you laying out?  Who are you going to get your boards made by?

ExpressPCB, Sorry, I don't mean to be opaque but it is for someone else's commercial project.  Despite it being a tiny project, it's not my place to talk details, but suffice to say it's a distortion pedal. 

Insert Quote
I run 30 mil traces for ground and power, unless there is a layout problem and they have to neck down.

Wow, that's pretty thick, but it makes sense what you're saying.

And has nothing to do with how much the pedal draws. A four transistor circuit (Big Muff, huh?)  running off 9vdc probably only draws around 10-15 ma at maximum. Usually the indicator led is the highest draw in the circuit. The current rating on a power supply only indicates how much current that supply will source at maximum, but it will only source as much current as the circuit draws.

Of course, I'll admit I'm being lazy not looking up the data sheets, but it's more fun to talk it out here.

[R O Tiree]

I've customised my installation of ExpressPCB quite a bit...

I've fattened up all the pads on all through-hole components to 56 mil with 29 mil holes.
Pads for pots, etc, I use 80 mil with a 35 mil hole.
Traces are generally 50 mil. On a 100 mil grid, this also gives me 50 mil spacing between traces. so parasitic capacitance is tiny. Very occasionally, I'll have to neck down to 30 mil.
That will still leave a fair amount of copper to be etched away, so I then fatten up the ground and power traces to eat up as much slack space as they can. Any spare space on the board and I fatten up other traces by just drawing squares, triangles, etc with 50 mil traces.
Any component pad ends up in the middle of a big fat area of copper and I'll usually "hollow out" the shape I've made and fill it again with a small copper-plane. Once I've done that, I set the pad proprerty to "thermal to filled plane".  You also have to make any traces joining or bounding that copper-plane able to join to that plane without any clearance (right-click, set trace properties, set 0 clearance, OK).

If you just draw a ground plane occupying your entire board area, you'll end up with a default 12 mil clearance around every trace and pad (except the ones you need to connect to GND, obviously, which needs to be done by hand). With ExpressPCB, you can alter the clearance around traces, but not around pads - that's set in stone and it's a bit of a pain.  The other drawback about it is, if your printed artwork is at all spotty, or your photo-sensitised board is of less than stellar quality, this kind of "isolation routing" will be hit and miss, at best.

OK, what about EAGLE? Personally, I don't like it. It has a much steeper and higher learning curve, it is less intuitive than ExpressPCB and it takes me much longer to do anything. I've tried, believe me, because I recently moved on to solder masks, which are dead easy to print out in EAGLE, but cannot be printed out at all in ExpressPCB. A useful workaround is to draw fat circles in the other copper layer... 0.040 line width, 0.015 radius will give you a spot that is slightly bigger than a 0.056 pad. Save your file and then drop a circle on every round hole on the OTHER side of the board from the traces (you can do something similar for square pads with very thin traces). Delete all the components off the board and delete all the traces - you should be left with just the dots and squares on the other side. Highlight them all, switch them to the other layer and then save the file as the same name + "mask". Say your first file was "Squeezer.pcb" then the mask file gets named "Squeezer_mask.pcb".

I use those names, here, because the Orange Squeezer is a simple circuit that I used to try to get to grips with EAGLE. First off, I did the design in ExpressSCH and -PCB, optimised it, and did the solder mask with this work-around. Then I did the same thing in EAGLE... "NO! Not round there... through THAT gap, dummy! Oh for Heaven's sake, I'll route it myself... See, it DOES pass your Design Rules Check! Why couldn't you have done that in the first place?" Maybe I'm doin' it wrong, but every time I moved a component to snuggle it up a bit closer and then hit the button to re-route, it kept on trying to route around instead of through and I could not get the board as small as the ExpressPCB one. In the end, I ripped it all up, made a direct copy of my Express board in EAGLE and then ran DRC... passed first time! Deleted all the wires and told EAGLE to auto-route... yup, you guessed it, a rats nest of roundabout routings again... Ho hum.

[EnnPeeEff]

Wow!  That's really great advice, I think I'll do a total redesign based on the advice here. 

I really haven't gotten anywhere with Eagle, the component library is totally overwhelming.  ExpressPCB has been great so far, really not much harder to use than "DIY layout"

[swinginguitar]

I've customised my installation of ExpressPCB quite a bit...

I've fattened up all the pads on all through-hole components to 56 mil with 29 mil holes.
Pads for pots, etc, I use 80 mil with a 35 mil hole.
Traces are generally 50 mil. On a 100 mil grid, this also gives me 50 mil spacing between traces. so parasitic capacitance is tiny. Very occasionally, I'll have to neck down to 30 mil.
That will still leave a fair amount of copper to be etched away, so I then fatten up the ground and power traces to eat up as much slack space as they can. Any spare space on the board and I fatten up other traces by just drawing squares, triangles, etc with 50 mil traces.
Any component pad ends up in the middle of a big fat area of copper and I'll usually "hollow out" the shape I've made and fill it again with a small copper-plane. Once I've done that, I set the pad proprerty to "thermal to filled plane".  You also have to make any traces joining or bounding that copper-plane able to join to that plane without any clearance (right-click, set trace properties, set 0 clearance, OK).

If you just draw a ground plane occupying your entire board area, you'll end up with a default 12 mil clearance around every trace and pad (except the ones you need to connect to GND, obviously, which needs to be done by hand). With ExpressPCB, you can alter the clearance around traces, but not around pads - that's set in stone and it's a bit of a pain.  The other drawback about it is, if your printed artwork is at all spotty, or your photo-sensitised board is of less than stellar quality, this kind of "isolation routing" will be hit and miss, at best.

OK, what about EAGLE? Personally, I don't like it. It has a much steeper and higher learning curve, it is less intuitive than ExpressPCB and it takes me much longer to do anything. I've tried, believe me, because I recently moved on to solder masks, which are dead easy to print out in EAGLE, but cannot be printed out at all in ExpressPCB. A useful workaround is to draw fat circles in the other copper layer... 0.040 line width, 0.015 radius will give you a spot that is slightly bigger than a 0.056 pad. Save your file and then drop a circle on every round hole on the OTHER side of the board from the traces (you can do something similar for square pads with very thin traces). Delete all the components off the board and delete all the traces - you should be left with just the dots and squares on the other side. Highlight them all, switch them to the other layer and then save the file as the same name + "mask". Say your first file was "Squeezer.pcb" then the mask file gets named "Squeezer_mask.pcb".

I use those names, here, because the Orange Squeezer is a simple circuit that I used to try to get to grips with EAGLE. First off, I did the design in ExpressSCH and -PCB, optimised it, and did the solder mask with this work-around. Then I did the same thing in EAGLE... "NO! Not round there... through THAT gap, dummy! Oh for Heaven's sake, I'll route it myself... See, it DOES pass your Design Rules Check! Why couldn't you have done that in the first place?" Maybe I'm doin' it wrong, but every time I moved a component to snuggle it up a bit closer and then hit the button to re-route, it kept on trying to route around instead of through and I could not get the board as small as the ExpressPCB one. In the end, I ripped it all up, made a direct copy of my Express board in EAGLE and then ran DRC... passed first time! Deleted all the wires and told EAGLE to auto-route... yup, you guessed it, a rats nest of roundabout routings again... Ho hum.

Well said, my friend!

Glad I'm not the only one who finally vacated EAGLE for ExpressPCB...(I'm a software veteran, and EAGLE just frustrates the snot outta me.....kinda like trying to use iTunes)

now if i could just figure out how to layout PCBs properly....

Do u guys often do double sided (for density)?

[R O Tiree]

Double-sided... never had the need for it, I guess. I tend to get the packing density fairly high, so there's not a lot of room on the top side for traces. The snag with double-sided is that you have to (generally) put vias in to transfer signals from one side to the other. You can either invest (thousands) in a plating machine, or you can insert little tiny rivets (cheap). Fiddly, though. There's also the issue of registration... you have to get the artwork for the top side precisely located relative to the bottom artwork. There are lots of videos on youTube from people who have developed workable systems.

The most I've ever needed is a couple of jumpers, and I use cut-offs from resistor wires for those.

All that said, my next step will be into SMD, so double-sided will be pretty much a requirement.