Different Net classses on GND?

"Per Green" <per.green@pipeguard.se> wrote in message

news:hjt2bg$qbg$1@cheetah.cadsoft.de...

Example: I have a CPU and power suppy part on my schematic. The CPU is

connected to GND via GND symbol and gets assigned to my own defined net

class GND. The power supply is also connected to GND via GND symbol.

 

Here is the problem: I would like to have a net class with smaller width

on the CPU part GND (8 mil) and wider on the power supply (20 mil).

However, whenever they are connected together the apply to the same net

class.

 

How do I split them to be connected to the same net but have different net

classes?

 

I have solved it temporary by having them separeted in different net GND

and GND_MAIN and then connected together with a resistor (0 ohm). Feels

stupid but I haven't understood how to separete them into different net

classes in any other way...

That is THE way to solve such issues. This way you can also place the 'star'

point of your GND's (if you got more than 2) wisely when it comes to decent

power layout. Normally this point is close to the power connector. Same goes

for shield signal. Shield is just another GND connection where there is no

currents flowing except discharge currents from connectors. If that is

connected to gnd close to the power connector, you can avoid high current

peaks going through the sensitive electronics. Hobbyists normally doesnt

care about this, but pro's do.

Yes the "resistor (0 ohm)" solution is the only available, but not so

elegant.

To route my PCb, I use a script like "auto Wire1; auto Wire2; ...",

obtaining a good PCB, better than EAGLE auto; and also better the

FreeRouting.

The problem of "2 GND traks size" is similar to the "decoupling capacitors

of an IC".

I want a straight track from the capacitor to the IC.

I suggest to the Eagle guys the following implementations:

1- name a segment of wire like mailto:GND@MAIN mailto:GND@CPU

mailto:VSS@PIN21 mailto:VSS@PIN34;

2- class the segments mailto:GND@MAIN mailto:GND@CPU mailto:VSS@PIN21

mailto:VSS@PIN34;

3- auto GND;     if I want to route all GND wire's segment;

4- auto mailto:GND@MAIN; if I want to route the single segment;

amelia

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Per Green wrote on Thu, 28 January 2010 17:16

I have solved it temporary by having them separeted in different net

GND and

GND_MAIN and then connected together with a resistor (0 ohm).

That works, but now you have another part that has to be loaded, bought,

stocked, etc.

I use Eagle devices I call "shorts".  They have two pins and just connect

them together.  For the symbol I make a line just a little wider than a

normal schematic wire.  I have several flavors for connecting only on the

top layer, bottom layer, all layers, etc.

The shorts library and a bunch of other Eagle stuff is in my Eagle tools

release that is available for free from

http://www.embedinc.com/pic/dload.htm.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Hello

I miss the net naming feature too:-) When using an auto router it must

be there.

On 28-01-2010 23:16, Per Green wrote:

Example: I have a CPU and power suppy part on my schematic. The CPU is

connected to GND via GND symbol and gets assigned to my own defined net

class GND. The power supply is also connected to GND via GND symbol.

 

Here is the problem: I would like to have a net class with smaller width on

the CPU part GND (8 mil) and wider on the power supply (20 mil). However,

whenever they are connected together the apply to the same net class.

 

How do I split them to be connected to the same net but have different net

classes?

 

I have solved it temporary by having them separeted in different net GND and

GND_MAIN and then connected together with a resistor (0 ohm). Feels stupid

but I haven't understood how to separete them into different net classes in

any other way...