findbuddha is routing the BLM board...

[findbuddha]

More noob PCB meanderings:

I've gone back to separate Scalar PCB.....

I manually routed the 'long' connection between J1 -> shift registors -> J2, then let the autorouter do the rest.

Any suggestions?

:)

[nILS]

Any suggestions?

Yes. Don't use the autorouter. Ever. Unless you are one of the 3 people who tamed it. Until you have: Don't use the auto router. Have I mentioned not to use the autorouter? Oh and one last thing - don't use the auto router.

[findbuddha]

oh....

Could you briefly tell me why? freerouting.net seems (to my eye) to do a nice job of connecting everything, then optimizing it.

What should I be doing to route this design that an autorouter can't?

Thanks!

*edit*

I re-did it with GND and +5V planes, and it looks a bit neater.....

Edited August 15, 2010 by findbuddha

[nILS]

Unless you really know how to tame the autorouter (correct net functions, DRC per net, etc) it'll always be worse than what you manually do. Some random things: 90° bends on HF lines are horribly bad, cause they lead to reflections. Generally more copper is better - 10mil traces around areas that are exposed to physical pain caused by pads being constantly hammered down on them is probably not the best thing to do. Overall, you (should) know more about the PCB and what does what than the autorouter. You can make sure HF lines aren't going all over the board just to save one via, ... Last and least - autorouted stuff is a pain to look at.

Also, as opposed to ground planes, power planes aren't all that common. I personally dislike them cause a single, small scratch pretty much always exposes V+. And in my imagination, it basically turns the entire board into a capacitor :yes:

[Wilba]

nILS, you need to talk down to us Aussies... maybe use the local vernacular... like...

Autorouters are about as useful as tits on a bull. They put tracks all over the place like a mad woman's shit. Even blind Freddy could do a better job. I'm not pissing in your pocket mate!

[seppoman]

+1 for don't touch the autorouter :no:

Also, as opposed to ground planes, power planes aren't all that common. I personally dislike them cause a single, small scratch pretty much always exposes V+.

agreed - plus a VCC plane doesn't have important positive effects - GND planes provide improved GND impedance which is a good thing, but with VCC this doesn't really matter.

And in my imagination, it basically turns the entire board into a capacitor :yes:

That's right, alhough on multilayer PCBs, this is an intended effect, it works just like an additional smoothing capacitor and is completely free of charge (pun intended :D)

S

[findbuddha]

nILS, you need to talk down to us Aussies... maybe use the local vernacular... like...

Autorouters are about as useful as tits on a bull. They put tracks all over the place like a mad woman's shit. Even blind Freddy could do a better job. I'm not pissing in your pocket mate!

Tits on a bull????? :frantics:

OK, thanks for all the auto-router info.

I've gone and layed out the components more intelligently :thumbsup: , and routed it manually (still using Freerouting.net).

Any more tips?

Ta :)

[nILS]

Which DRC did *that* pass? Your tracks are way too thin, way too close to pins and other tracks and have way too many 90° bends.

- Try routing with 16 mil traces

- Look at the spacing between the ground plane and the pins - there's a reason for that

- Delete that layout. Start over - best way to learn.

- Oh and, make a new thread for PCB design questions.

[findbuddha]

Which DRC did *that* pass? Your tracks are way too thin, way too close to pins and other tracks and have way too many 90° bends.

- Try routing with 16 mil traces

- Look at the spacing between the ground plane and the pins - there's a reason for that

- Delete that layout. Start over - best way to learn.

- Oh and, make a new thread for PCB design questions.

It passed Kicad's DRC.....

Tracks too thin? Ok, I will try 16 mil traces....

Too close to pins? Do you mean for manufacturing, or electrical interference? I have used 10mil minimum clearance: the two manufacturers I might use specify 8mil (PCBCart ) and 7mil (Gold Phoenix).

Delete that layout? :shocked: Can you please suggest a better layout? I've already spent many hours deleting and starting over :sorcerer:

I just looked at TK's protoboard layout http://midibox.org/forums/index.php?app=gallery&module=images&section=viewimage&img=277

Seems to have IC1 a long way from IC2 - I didn't realise such long SC/RC lines would be acceptable???

Thanks for your help :)

[findbuddha]

Here it is, redone with 16mil traces, 10mil clearance. Passes kicad DRC. These are direct screenshots from kicad, instead of the poorly layered render I did last time.

I've attached one with GND plane, one without.

Am I getting closer? (Still a few components need moving a little, mostly caps)

Thanks :)

[nILS]

- Vias in between pins are bad juju

- Unneeded vias are bad juju as well (bottom right corner IC, pin 11)

- breaking up the ground plane more than necessary is bad juju as well

- 10mil spacing may lead to errors depending on where you get the boards fabbed. I'd try to stay at or better yet above 12mil. On the last run of gm5x5x5 I used 12 mil clearance and roughly 5% of the boards were "fixed" by PCBcart due to errors. Read: "passes DRC" != "will actually work"

- there's no mount holes

Seems to have IC1 a long way from IC2 - I didn't realise such long SC/RC lines would be acceptable???

Zoom back out - how big is the entire board again? ;)

[findbuddha]

I appreciate your help :)

I think I'm getting closer:

- 12mil spacing

- 16mil traces except for a couple of 14mil that go between some pads.

- ground plane seems a little better utilised.

[findbuddha]

Complete redo, for various reasons..... Based on TK's veroboard layout. Bigger traces than before, 12mil clearance.

Any ideas?

:)

[findbuddha]

Well, scratch that last post. I've gone back to a slightly more compact version of my original layout, as it's easier to layout the button board.

This layout should be usable for both 'horizontally compact' and 'SEQ CS aligned' options, with a simple drag of components. There's a footprint for standard 6mm tactile, as well as ALPS SKPG switches (quiet action, tactile feel: http://www.alps.com/.../SKPG_list.html).

Comments please? :frantics: (I know I haven't added mounting holes to the button board yet - there's space between the buttons)

[findbuddha]

Moving right along.....:sorcerer:

[ilmenator]

The DIL headers seem to be a little too close? At least if you prefer the kind of connectors that hold the plug tightly, like these:

(Disregard that this particular one has a 2mm grid.)

[findbuddha]

:thumbsup:

Thanks for picking that up. I should have created the proper footprints for them.

I'll have to use the 'bare' board stacking style headers that take up less space. Any idea how easily they wiggle loose? We're talking 2x 2x8 headers holding up each ~5cmx5cm board.

[ilmenator]

On the stacking works quite well, but then the headers go around all of the 25cm x 25cm boards. In your case I would probably add mounding holes (one should do if space is an issue) that could be used to fix the boards to each other with a long enough M3 or so screw.

[findbuddha]

Cheers.

As space is tight, I've added a single solder pad near each set of headers. A cut resistor leg between boards should be plenty to hold them together, and not be too difficult to remove if needed.

[ilmenator]

Now, that's a smart idea :thumbsup: