Board Layout Skills?

[kolbep]

Hi.
Please take a look at this board I am laying out in Eagle.
It is single layer (the jumpers that are shown as being traces on the bottom layer will just be wire jumpers). I will be doing toner transfer and producing my own PCB. if all goes well, then I will send it to a boardhouse. It will be almost all SMD


Does the layout look reasonable for a beginner to PCB design, or do I need to rip it all up, and do it some other way. I don't like how it looks, but I am really my worst critic.

[fcb]

I'd put decoupling up against the MAX3483. Also i'd probably use a fill for the ground/0V instead of tracking. PIC's are fairly forgiving in layout.

Do an experiment, take a copy of your board and remove the 0V routing from the PCB and then use the ground fill function to route the 0V.

[Monkeh]

You're going to have an exciting time soldering that with no soldermask.

[Fred27]

Home etched doesn't necessarily mean no soldermask. (It probably does though.)

I'm a big fan of Dynamask 5000.

[owiecc]

There is lots of empty space in the middle of the board. You can shift the bottom components 1cm up.
1000uF seems quite big. Do you need so much? Normally 100uF should be fine.
Align the jumpers and connectors in one line. Ideally keep them on 100mil spacing (so it does not look like Arduino connector).
Rotate U2 counterclockwise and move a bit up.
Move C3/C4 closer to U3.
Be careful about spacing around S1. It will be hard to solder. Same goes for U3.
As fcb suggested: pour GND on the bottom. This will free up some space on top layer.

General tip: try keeping traces as short as possible. Move components close together to help with that. Shorten 90deg bends with 45deg ones.

[gman4925]

If your Through Hole parts are on top along with the SMT parts then you will not be able to solder them down if it is a single layer board, as the pads will only be on the top, under the component.
My normal process for doing a board that can be made on one layer is to lay out all the SMT parts on the top layer, with TH parts flipped to the bottom layer, then I flip the entire board, so all tracks are on the bottom layer and TH parts are on top, to envisage how it will look, as generally you will need TH parts on top.
I would suggest you change S1 to be TH so it can be accessed from the top.

Other things, not necessarily in the order they should be handled.
-Watch your trace widths for tracks under D5/S1 (find out what is easily/reliably etchable)
-Watch your spacing (same as above)
-Use 45° corners instead of 90°
-Thicker traces for power/ground
-Flood fill for ground (save time and acid for etching too), leave orphans on if etching.
-Consider using more links to avoid long snaking tracks and then when you get it manufactured get it done in 2 layer
-Use vias that are big enough to fit a wire as the link
-Make it fit in 5x5cm so you can get a cheaper board from somewhere like seeedstudio fusion
-Use ratsnest and the DRC (traces around R5 are too close)
-Make traces enter pads at 45°/90° (looking at -ve of C1) to avoid acute angles of copper where acid can form a bubble and eat a disproportionate amount of the trace.
-Looks like your first board, if it is and you have not yet purchased acid/toner transfer paper etc (and can wait 2-3 weeks) consider just getting it made at seeedstudio its about US$10 for 10 boards and DHL is about $25 so chinapost will be a lot cheaper, I get boards in under 2 weeks when shipping by DHL from them, that should come in under the cost of diy materials, but your respin time will be longer if you need to fix any errors.
-Getting it manufactured will save lots of headache trying to solder that PIC without soldermask
-Smash the components, then resize the texts so they are not all different sizes (relevant if you get it manufactured).
-Add some holes so you can mount it with screws.
-Add a board outline

[kolbep]

Ok, I have taken your suggestions, and here is my respin of the design.
The reason for the blank space at the right is for the Optotriacs, and Triacs with snubbers,etc. Still have to get to that part though.

The Poly Fill is connected to VSS, with clearance of 10, and Isolation turned on.

I can Smash the components, but when I try to change the writing size, I cannot, It just does not do anything. Still have to figure that part out.

I only have 2 Jumpers going across the back of the board. So if double sided is not too much more expensive than single sided, then maybe I can put the SMD opto-triacs and SMD Triacs on the back of the board, and that way save on real-estate...

Hows it looking now? Better than before?

[xgmr|anti]

Miter all those 90s.

[mzzj]

Ok, I have taken your suggestions, and here is my respin of the design.
The reason for the blank space at the right is for the Optotriacs, and Triacs with snubbers,etc. Still have to get to that part though.

The Poly Fill is connected to VSS, with clearance of 10, and Isolation turned on.

I can Smash the components, but when I try to change the writing size, I cannot, It just does not do anything. Still have to figure that part out.

I only have 2 Jumpers going across the back of the board. So if double sided is not too much more expensive than single sided, then maybe I can put the SMD opto-triacs and SMD Triacs on the back of the board, and that way save on real-estate...

Hows it looking now? Better than before?

It looks like you forgot the attachment 

[kolbep]

OOPS, Indeed I have.
Let me know what you think of this, and then when I correct any suggestions, I will also go and Mitre the 90's as advised...

[mzzj]

Definitely much better!

few improvements:
-for home made board you probably better of with lot more clearance between ground poly fill and traces to ease soldering.
-C4 supply decoupling capacitor traces makes a big loop to complete the current path to your microcontroller.
Placing your supply decoupling caps close to the chip doesn't do any good if the current has to make huuuge roundtrip around the board. Move C4 closer to the controller and route the vcc trace up to C2 from the left side or something like that ( or route between C5 and C2)

For your use the layout between D1- US2 and C1 probably works just fine but it looks kind of wrong. For best filtering results run separate trace from C1 to US1

[fcb]

Looking much much better.

I would suggest you look up "acid traps" on PCB's (although I'm not sure this quite the problem these days), this might explain some of the theory behind mitres on corners.  I've always liked the ideas of electrons over shooting on 90's like Scalectrix slot cars..

Also, the non orthogonal tracks (near & to JP4) look ugly.

All in, I reckon that's fine to send for mfr.

[DanielS]

I would rotate the diode bridge clockwise 90 degrees to have straighter traces, rotate R1 and ZD1 CCW 90 degrees aligned with R2 so everything is on one straight line to the jumper, move JP4 up, rotate the switch clockwise 90 degrees, rotate JP5 180 degrees and move it down.

That should clear up the layout a fair bit further after straightening everything up.

[sleemanj]

The trace squeezing through the corner of the PIC going to a wire jumper (top side trace) - if you move R4/5 and their leds down, and S1 down a bit too, then you can make some space to bring that trace out the front of the pin and get rid of the jumper totally.   You couls also get rid of that jumper from the MAX to the PIC, if you don't mind a bit of a long trace.

For home etch, give yourself more clearance between the copper pour and traces.  In general too, if you can give more space between traces (or make traces larger), no reason not to, and it makes your home-etch easier.

Get yourself some zero-ohm 1206 size surface mount "resistors", they come in very handy for single side boards when you want to jump a single trace, just drop down a 0R, saves drilling holes, bending wires, stripping wires...  Just remember that they are not of course 0 ohm, they do have a very small resistance (a few tens of milliohm perhaps), so bear that in mind.

[Dave]

Another problem I spotted: Soldering that C1 capacitor is going to be difficult, because home made holes probably won't be plated and therefore soldering it from the bottom won't be enough to make a connection to the traces on the top side. I'd opt for an SMD cap.

[DanielS]

Another problem I spotted: Soldering that C1 capacitor is going to be difficult, because home made holes probably won't be plated and therefore soldering it from the bottom won't be enough to make a connection to the traces on the top side. I'd opt for an SMD cap.

Not a problem if you put the cap under the board but that would require some adjustments to enclosure plans.

The same thing applies to all those (presumed) 0.1" headers too: difficult to solder the pins if the plastic spacer is flush against the board.

[xgmr|anti]

Here's a quick example of what I meant by miter.

[sleemanj]

The same thing applies to all those (presumed) 0.1" headers too: difficult to solder the pins if the plastic spacer is flush against the board.

Soldering .1" male headers from the top is not too hard, put them in, solder the bottom, then grab your curved tip smd tweezers and lever the plastic up a couple mm, solder the top sparingly, and push the plastic back down.  Of course doesn't work with female ones.

For electrolytic caps, just solder them a bit off the board so you can access the top pad, it's only a prototype after all, a bit of hot glue will stop it moving around if necessary.

[Smokey]

I'm going to take a different route here.... You've done a good job so far... but....
Instead of making it one layer of routing and home etching the board, take the jump and go with some professionally made 2 layer boards.  You don't say where you are from, but shipped to California Itead got me 10 5cm x 5cm 2 layer boards in 2 weeks earlier this month.  That's 10 boards for 12USD in two weeks.  Even if it takes them longer, its still worth it.  And there are faster places for not much more now.

Real two layer boards are easier to route, will look professional, will solder better with fewer solder shorts because of the mask, will have better signal integrity since you don't have to snake them all over the board, you can use all SMD parts and not worry about through hole stuff to jump traces, and you can have very good confidence that out of 10 PCBs you will have 10 working boards.  Out of 10 home etch boards you might get 4 or 5 with that QFP.

If you absolutely have to home etch just for the experience (which sucks) make your through hole pads bigger by as much as you can.  It will make drilling easier since you can use a bigger drill bit and won't have to worry about missing the middle as much.  For that matter, the bigger you make all your traces where you can the better chance you will have of not over-etching and having open traces all over the place.  And watch out for the fiberglass drill dust which can itch like crazy.  Oh home etching..... 1 million down sides, 0.5 benefits. 

[kolbep]

Thanks Smokey.
Yesterday I actually decided that I would just get a board house to make the board for me.
That way it is 2 sided, easier to route, and will look a lot neater.
And, If there are any mistakes, that is why you got bodge wires, and a knife to cut tracks...

Do you think it will be ok to have something like (as much as possible) horizontal tracks on the top layer, and vertical tracks on the bottom layer, and the ground fill the rest of the Top and Bottom layers (stiching together the polygons), or does that sound like a bad idea?

P

[tautech]

 kolbep, I've been watching this thread and the posted replies with interest.
I feel as you have not given us the full layout, it has been hard to steer you in the right direction.
 
A nice PCB is a beautiful thing and the "feel" to make one takes some time and study to develop.
Hopefully you can find some guidance in these links:
From our Dave: http://www.alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf

You can also learn a lot from some of the critique requests on the forum:
https://www.eevblog.com/forum/projects/first-pcb-design-critique-welcome/msg509347/#top

Search for more PCB review/critique's, there are many.
Study as the tread progresses the changes and why.

If you think you want to have a go at etching by all means do, especially until you have done a few PCB's and learnt the traps and pitfalls to avoid.

The favorite saying of the DR. EE that guided me was "god awful", and I knew I was almost there when he stopped using that phrase. 
Hang in there, it takes time.

[kolbep]

as you have not given us the full layout

This was not done intentionally. I was mainly wanting to get the first part of the board right before I add the other parts, or else the Ratsnest would be a real mess. I did have the other parts on the schematic, but it got too busy. All that is missing is the Opto-Triacs, Triacs, Snubber Cap and 3 resistors per channel (looking at 4 channel for now).

Then I got to thinking, I might just have a seperate board to contain the Opto Triacs, Etc. That way it is easier to swap out during the gig, if one Triac blows, just swap out that specific PCB. Instead of having to solder a new triac in.

The project is a DMX Controlled Light Dimmer system.
 

A nice PCB is a beautiful thing and the "feel" to make one takes some time and study to develop.
If you think you want to have a go at etching by all means do, especially until you have done a few PCB's and learnt the traps and pitfalls to avoid.

I have etched a few of my own boards before, but they were all basic Through-Hole Boards (E.g. EPE Magazines PIC Tutorial Board. As well as a 3 channel light chaser using a 555->LM317->Moc3021->Triacs). These were done Toner Transfer and did not look the best.
That is why I was thinking of Etching this one, and then if it works ok, then going the Boardhouse route. But after this thread, I am getting confident that I should be able to get proper boards made straight. I mean the Itead that was mentioned further up is fairly cheap, and will cost $8 standard post.
That also means I do not have to worry about solder bridges or over/under etching on the TQFP pack (as that is a lot of pins for my first venture into Surface mount).

This weekend I will get into relaying out the board again. Work comes first...

[marshallh]

Another tip: get your hands on any/every pcb you can find. Look at them, understand them and pick specific things about them that you like.
On each pcb you do, try to incorporate a couple of these things. So you are continously adapting and improving.

[kolbep]

Well, I have done it.
Spent this afternoon relaying my board, making decent use of both sides. 5cm x 5cm is a tiny board size for so much stuff. But I got it to fit.

I have also designed a seperate board with the optos, triacs and snubbers. I managed to squeeze 2 channels on these  boards. So basically I can have 1 cpu board, and 3 triac boards, to make a 6 channel dmx dimmer / switch.

Worked out to about 280zar for 10 of each board, including slow postage. I am trying Itead as recommended above.

While I wait for that, and the other parts, I can get down to finishing the code...

[kolbep]

Will keep you posted when I get the boards.
btw, who is a cheap supplier for a syringe of solder paste in South Africa...

P