Wanted: Eagle advice

[pinkmouse]

OK, I'm playing around with a balanced input active crossover design in Eagle. It is a double sided board, and I want to run a ground plane on the top for all the chip bypass caps, with seperate earth star runs for the signal on the bottom. At the moment, all the grounds are on the same net, linking back to a single through hole that joins the two layers. I have run all my signal grounds back on the bottom, and now I want to copper pur the top, but Eagle doesn't seem to want to let me seperate the two layers, and refuses to let me connect the polygon to my ground net.

Am I just stupid? I have been banging my head on this for a couple of hours now, and the only solution I can see is to ripup everything I have done so far, and split the ground net into two.

HELP! Can anyone save my sanity?

[Bricolo]

If I understood correctly, you wand a groundfill on a layer, and a star ground on the other. And a simple connection between the two, with a through hole at the star's center?

I think it's possible with eagle.
-don't connect the cap's ground to anything at first
-route all the grounds on the bottom layer, in a star scheme
-place a via at the star's center
-place a polygon on the top layer. in the command line hit "name" (without the quotes) and hit enter. Then, click on your polygon. Enter "GND" for the name (still without the quotes) it asks you if you want to call it "GND" or "Net xx", choose "GND".
-Click on the "Ratsnet" button.


It should be ok.

I can try to fix it if you want, you can send me the eagle files via mail.


Alex

[JochenH]

Hi,

is this a SMD design with the components placed on the bottom side? Otherwise the TOP ground plane would (usually) connect to the pins which you do not want as i suppose.
What do you mean when you say that Eagle doesn't let you seperate the layers?

Jochen

[pinkmouse]

Bricolo

Thanks for the offer to fix the board, but this is only a practice run, to get to know eagle, it's not that mission critical!

I suspect that I have just gone too far into the project, and not thought ahead enough to do this properly. I will give your ideas a try on a new version. Practise makes perfect!

Jochen

No it's just a conventional through hole design. I am just trying different things to increase my knowledge of Eagle, it may not have much real use as a design technique in the real world.

Basically the problem I have is that because my earth net is on two layers, I think it gets confused when I try to attach a polygon to it, it seems to want to include the rats nest conections on the bottom layer.

[JochenH]

There is no way to seperate nets by layers, a net GND is valid on all layers. Thats why it connects a polygon with thermals to the through-hole pins if possible, regardless if you routed these pins by hand. This would be easier with SMDs in your case.
One solution is not to connect the polygon (by the NAME command) to the net but use a 0 ohm resistor to connect the nets. I don't know if Eagle supports "Jumpers", i have to check.

Jochen

[jackinnj]

there are a couple newsgroups on usenet -- under
news.cadsoft.de look for eagle.userchat.eng

[Bricolo]

Oh I see what you think, I just tried your "dual ground" on a project.

Even if you route a star ground on the bottom; it still connects all those pins to the groundplane on the top.

Not so problematic if it's for a self etched PCB, simply ripp of some copper arond the lead, and don't solder it to the groundplane.
For industrial made pcbs, it's more dificult :/

Strange, indeed

[jacco vermeulen]

Pinkster,

make frequent backups of your design while you are working on it. Better even to have two backups.

I had to make a ships hull design with a 3-D software package, one click on the wrong button and the whole thing turned psycho on me . After three months sweating at it starting fresh on a monday morning the entire file on the university main frame had dissapeared. At the second attempt i had backups on a floppy disc, thats when the file on the disc dissapeared, fortunately the server still had it. After that i had the file on the main frame, on three different files on a Zip disc, and on two floppy discs.
Paranoid, me ? It drove me completely bonkers !

[JochenH]

You could create a special "jumper"-part consisting of 2 SMD pads touching each other. In the schematics, one side is connected to "GND", the other to "GNDPLANE" net for example. In PCB name the polygon also "GNDPLANE" and put the jumper part on your via. See attachment.

Jochen

[pinkmouse]

OK, stupid mistake No. 1.

I was using the rectangle tool rather than the polygon... Doh

Now to see if I can get your other suggestions working. Cheers guys!