Eagle imposible routing

[guidoilieff]

Hi, I've been months with this project. Its a video signal generator that audio can be applied to modulate the signal.

The problem arose when trying to route everything with 0.8/0.6mm tracks. The autorouter can do 100% of the job but there is no way I can make a toner transfer with the default traces thickness.
I know everything is practice and already tried screaming and crying at the design but nothing seems to work. No even with jumpers.


What is the solution here? Should I make separate modules and connect them with wires? Is there a procedure for beginners? I read a bunch of articles on the web but it doesn't seems to tackle my problem.


Its my first "complex" schematic and I know its a mess. Ill post pictures of the schem I did and the autorouted pcb with default options.








Thanks for your time, sorry for my english.

[vigilante397]

Auto-routing technology has come a long way, but is still nowhere near perfect. Regardless of the complexity of the design, I don't trust it. I would recommend doing it yourself. Also, as a bit of bad news, some complex projects require the use of multi-layer circuit boards, and there's no way around it.

All that being said, you should be able to change the settings for the autorouter and set thicker traces and wider spacing to make sure you can get results that you can transfer and etch.

Good luck!

[diffeq]

Breaking things down helps a little bit. I tried to route a phaser once and it was a very hard thing to do with just one layer and a quad opamp, TL074. I broke it down to single channel ICs and it became more or less manageable after that.

The way I see it, any circuit is simply a set of entangled connections and one either untangles it on a double-sided board, making mounting a breeze, or untangling it off-board with jumpers and messy wiring, making mounting/wiring a pain. Try to identify the knots in your circuit and work from there. 4093 is one, that VGA is another. You can tear that VGA into solitary pads and place them around the whole thing, then wiring them to a socket with wire.

Just my 2 cents.

EDIT: don't route GND connections, use polygon pour for that - http://dangerousprototypes.com/blog/2012/07/18/eagle-polygons/

[reddesert]

I'm no Eagle expert but there are several separate issues here:

- You should go into the "Design Rules" section and change the default track width and clearance to something much wider, if you're going to do toner transfer and etch. Maybe 16 or 24 mils.  The Eagle default of 8 mils is for sending PCB designs out to be fabbed, not for home production.
- Autorouters aren't up to the task and you should try to route it yourself. Try moving the components around until the airwires are relatively not tangled, then start drawing traces. It's an art form and you may want to try first on a simple circuit.
- As others said, a ground pour with a polygon is better. It also makes routing much easier because it connects all the ground pins.

There are several Eagle tutorial videos by JMK of JMKpcbs that are linked on the Madbean forum that I found helpful.

[guidoilieff]

Breaking things down helps a little bit. I tried to route a phaser once and it was a very hard thing to do with just one layer and a quad opamp, TL074. I broke it down to single channel ICs and it became more or less manageable after that.

The way I see it, any circuit is simply a set of entangled connections and one either untangles it on a double-sided board, making mounting a breeze, or untangling it off-board with jumpers and messy wiring, making mounting/wiring a pain. Try to identify the knots in your circuit and work from there. 4093 is one, that VGA is another. You can tear that VGA into solitary pads and place them around the whole thing, then wiring them to a socket with wire.

Just my 2 cents.

EDIT: don't route GND connections, use polygon pour for that - http://dangerousprototypes.com/blog/2012/07/18/eagle-polygons/

Have you ever done homemade double sided boards? I know about keeping a register. If I make vias as big as through holes I then can just solder scrap resistors/capacitors legs and make the connections of the traces on both sides. Is that weird? Any advice? I just think that'll make things neater.

[guidoilieff]

I think I've done it, the awfulest pcb design in the world... but in theory it should work... right?

[diffeq]

Your polygon pour is not connected to any signal, it's floating. It should connect with some pads cross-like, like on a picture here https://en.wikipedia.org/wiki/Copper_pour  . Try naming polygon pour as "GND". The design is not bad at all, though.

Double-sided boards are much harder to do at home. Personally, I've never done this but I've seen DIYers printing decals side-by-side and folding over the double-sided copper board, aligning free ends together.

[temol]

I've made couple of double-sided boards at home. The main problem is lack of metalized holes. Sometimes it makes soldering very hard or almost impossible, especially when soldering under component which is touching the board. You can always use jumpers on single-sided board.

T.

[guidoilieff]

Your polygon pour is not connected to any signal, it's floating. It should connect with some pads cross-like, like on a picture here https://en.wikipedia.org/wiki/Copper_pour  . Try naming polygon pour as "GND". The design is not bad at all, though.

Double-sided boards are much harder to do at home. Personally, I've never done this but I've seen DIYers printing decals side-by-side and folding over the double-sided copper board, aligning free ends together.

woa, you're right. I named it GND, I don't know what happened. Thanks!


I didn't get the folding thing though...

[diffeq]

Basically, like this:

(except that he staples it first, which is better than folding it like a postcard, I think)

[R O Tiree]

When faced with a track that "just won't go" without some very roundabout routing, there's nothing wrong at all in using a resistor lead cut-off to make a jumper to go on the top (component) side of the board... a poor-man's double-sided board, then.  Place a solder pad at each end of your jumper, then bend the wire to length, solder it in - simples!

[guidoilieff]

Basically, like this:

(except that he staples it first, which is better than folding it like a postcard, I think)

Mother of god, he's a genius... I'll try that.


I also made a double sided board with no vias. I just have a ground plane not connected but will make it manually with a wire.

[diffeq]

Nice! I can see that keepout around grounded pads is small as it should be, maybe check design rules settings, should be something about pouring and thermal pads to tweak around.

One trick about polygon pours is that you have to watch out for dead zones created by track-component loops (islands and bays, so to speak). The red (upper?) pour around 744066N IC goes to D-sub middle row and then hits the dead end. If you move that vertical track next R3 and R5 a little to the left, you'll let main part of pour spill in the dead end, thus connecting it.

Completely unrelated to routing topic, but you have two gates of 4093 unused. Leaving logic gates in unknown like that can lead to oscillation as inputs accumulate charges. Might not be the case with Schmitt trigger, but it's generally considered a good idea to connect unused inputs of logic to a defined state (HIGH or LOW).

[R.G.]

Some fundamental concepts:
1. Placement is king. Placement of parts can make routing trivial or impossible.
2. Good placement relies on placing parts that are most heavily interconnected as near one another as possible. The idea of having connection "rubber band" connections was concocted to make people think that connections actually had pull on the parts they connected, so that the circuit would contract on the pull of the connections to the most closely connected placement, or very near it.
3. Minimum cut-set. IF you have a set of connections, as in IC1-pin2 to IC4-pin7; R3-pin1 to IC3-pin3 (and on for all of the hundreds of connections), a minimum cut-set of two means you only have to cut two connections to separate the circuit into two independent sections. A cut-set of three only needs three connections cut to separate it into distinct parts. Placement can be based on minimum cut-set, then increasing cut sets, to literally sort the interconnections out, for further rubber band placement.
4. Scorable nets. Auto routers sometimes use a polynomial to calculate the "goodness" of placement, then routing. Things like shortest total length of all traces combined, smallest PCB area, smallest number of layers, etc. go into this calculation. People found early on that you don't need to score all the nets to figure out a good layout. For instance, you can usually ignore ground, not because it doesn't matter, but because it has to go EVERYWHERE so it doesn't make a difference in the scoring. Similar for power, bias nets, etc. that go lots of places. You're looking at the differences in connections, not the sameness of connections.

But all this sophistication is to arrive at good placement. Placement is king.

[Fender3D]

^^
Yes,
positioning is the most time-consuming stage...
after that, is like sudoku

[ElectricDruid]

I think everyone has covered it pretty much, but I'll summarise:

1) Go back and change the schematic to make all unused logic inputs are tied to ground or +V. Don't leave them floating.

2) There look to still be some errors. I can't see any power supply connections for IC4. You've got no supply greater than +5V, and the TL074 won't run effectively at such a low voltage. Your 5V regulator connects to Vcc, but all your 5V chips connect to 5V. These should be the same.

3) Don't be afraid of jumpers. Yeah, sure, we're all trying to *avoid* them, but if you've got a neat board that uses a couple, what's the problem? It's much better than a bad board that uses up much more PCB area and doesn't use them.

4) If you're going double-sided, think about what you put on each side. I usually route power rails on the top layer, and use the rest for a ground plane. Occasionally this scheme really isn't suitable, in which case, an alternative approach is to route horizontal connections on one layer and vertical connections on the other. Obviously most connections are a bit of both (H+V), and this is where the human skill comes into the equation and the autorouters starts to look a bit hopeless.

5) Break it up into pieces. You can route just a chip and the components that go with it and the once you've got the various functional elements sorted out, you can start organising them on the board. For me, this process is usually a bit of forwards-and-backwards; I'll route some basic elements, and then that will make it obvious which wires between the units I'm going to have trouble with, so then I'll reorganise the overall placement of the elements, and so on...

Your board has several chips on it, with their associated components. I'd start by getting the relevant components close to each chip. You then need to think about the power routing between the chips, and the overall signal flow from one block to another. Can you arrange the chips on the board so the signal flow makes sense? Remember one gate on a chip is the same as another, and one op-amp in a package is the same as another. This is the point that I find myself going back to the schematic and swapping op-amp 3 and op-amp 1 in a quad package over, for example, because it makes more sense on the board layout. The same thing happens with logic chips. Using a gate on one or the other side of the chip might make life a lot easier, and it doesn't matter where the unused gates finish up.

6) To do a nice job takes time and practice. Don't beat yourself up if your first attempt isn't the greatest. If you get it working, that's a win for starters!

HTH,
Tom

[R.G.]

6) To do a nice job takes time and practice. Don't beat yourself up if your first attempt isn't the greatest. If you get it working, that's a win for starters!

Let me re-emphasize that. I did my first crude board layouts in 1971. I've been learning and trying to get better ever since. I can never go back to an earlier layout - even one from last week - without seeing something I should have done better, or at least differently. There is always one more thing to improve on.

But make no mistake - like some other Big Steps in life, there will never be another feeling like the first time it all works.    

[guidoilieff]

I think everyone has covered it pretty much, but I'll summarise:

1) Go back and change the schematic to make all unused logic inputs are tied to ground or +V. Don't leave them floating.

2) There look to still be some errors. I can't see any power supply connections for IC4. You've got no supply greater than +5V, and the TL074 won't run effectively at such a low voltage. Your 5V regulator connects to Vcc, but all your 5V chips connect to 5V. These should be the same.

3) Don't be afraid of jumpers. Yeah, sure, we're all trying to *avoid* them, but if you've got a neat board that uses a couple, what's the problem? It's much better than a bad board that uses up much more PCB area and doesn't use them.

4) If you're going double-sided, think about what you put on each side. I usually route power rails on the top layer, and use the rest for a ground plane. Occasionally this scheme really isn't suitable, in which case, an alternative approach is to route horizontal connections on one layer and vertical connections on the other. Obviously most connections are a bit of both (H+V), and this is where the human skill comes into the equation and the autorouters starts to look a bit hopeless.

5) Break it up into pieces. You can route just a chip and the components that go with it and the once you've got the various functional elements sorted out, you can start organising them on the board. For me, this process is usually a bit of forwards-and-backwards; I'll route some basic elements, and then that will make it obvious which wires between the units I'm going to have trouble with, so then I'll reorganise the overall placement of the elements, and so on...

Your board has several chips on it, with their associated components. I'd start by getting the relevant components close to each chip. You then need to think about the power routing between the chips, and the overall signal flow from one block to another. Can you arrange the chips on the board so the signal flow makes sense? Remember one gate on a chip is the same as another, and one op-amp in a package is the same as another. This is the point that I find myself going back to the schematic and swapping op-amp 3 and op-amp 1 in a quad package over, for example, because it makes more sense on the board layout. The same thing happens with logic chips. Using a gate on one or the other side of the chip might make life a lot easier, and it doesn't matter where the unused gates finish up.

6) To do a nice job takes time and practice. Don't beat yourself up if your first attempt isn't the greatest. If you get it working, that's a win for starters!

HTH,
Tom

Thanks, you gave me advice I hadn't found anywhere on the web, brought my hope back on this design and more problems to fix before disappointing myself with a useless populated pcb.

[guidoilieff]

6) To do a nice job takes time and practice. Don't beat yourself up if your first attempt isn't the greatest. If you get it working, that's a win for starters!

Let me re-emphasize that. I did my first crude board layouts in 1971. I've been learning and trying to get better ever since. I can never go back to an earlier layout - even one from last week - without seeing something I should have done better, or at least differently. There is always one more thing to improve on.

But make no mistake - like some other Big Steps in life, there will never be another feeling like the first time it all works.   

I would love to have the ability to design pcbs by hand... I mean, i've done it with markers but having that professional look would be awesome to me. 

[287m]

i always with basic from RG, or Jack AMZ? i forgot
start from left is input, and right is output
its easiest to draw. And Runoffgroove teach me the simple way

im lazy too etched, so perf its the fastest way
then, i jealous with perf wizard like Rick freqcental, Jon midwayfair and Russ Cozy, their layout is amazing
convert perf to pcb is easy

because the trouble in perf is mood to build, and hard to modify
move on to pcb, madbean have some good tutorial to make pcb. i follow

in the end, found unreal style like Jack Deville, look at his delay
or OCD-ish like bugg, how they can layout like that? amazing art

i must mention some 1590A builder, ex pickdropper, thomasha
their own layout is unreal too

the best lesson is from local store owner
want make your own layout?
imagine first, draw some variant, then decide what suit you
but please, no autorouter. Kill your creativity