How to have connected signals without connected wires on schematic?

nigelmercier wrote on Wed, 24 February 2010 07:45

How do you get the pin names on the uC to span two lines?

Huh?  What "lines"?

--

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

"Olin Lathrop" <eagle@embedinc.com> wrote in message

news:hlplqg$cbb$1@cheetah.cadsoft.de...

I have attached a snippet of a such a schematic...

How do you get the pin names on the uC to span two lines?

Mike R wrote on Sat, 20 February 2010 15:21

It seems a nice and efficient way to organize a schematic.  I know that

on 

the supply symbols like GND and VCC they will be connected together,

but 

is there a generic symbol that I can give a name to, and anything 

connected to that symbol will be connected on the board?

You don't need a symbol at all.  Having a symbol there is more likely a

artifact of the software used to make the schematic.  It is certainly not a

necessity, and Eagle doesn't force you to use one.  As User said, net names

are global, so all net lines of the same name are considered connected.

However, you need to document the connectivity, not merely explain it to

Eagle.  Use DRAW LABEL to show the net name on the schematic.  It's

important to use that instead of explicit text because that way it is

guaranteed to show the net name even if you change it later.  You may also

occasionally discover the net isn't named what you thought it was.

I have attached a snippet of a such a schematic.  All the names you see are

net names drawn with DRAW LABEL.  On the left side they document air wires.

Some on the right side are not really necessary since the net line on that

page goes to everything that net is connected to.  Inside the PIC code I

give names to pins, and it's helpful to have those names listed on the

schematic.

The arrows showing the direction of information flow are also useful in

helping demystify what is connected to a pin and how that pin is used.

Note that this has nothing to do with current flow, but rather signal flow.

--

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

Attachments:

Mike R schrieb:

I have noticed when I view professional schematics, they will have a 

microcontroller (as an example) and maybe some inputs may be labeled, with 

a short wire extending from the pin on the device, and then going to a 

symbol labeled maybe "temp_in".

 

Then elsewhere on the schematic, there will be a circuit with an output 

which goes to a symbol also labeled "temp_in".

 

It seems a nice and efficient way to organize a schematic.  I know that on 

the supply symbols like GND and VCC they will be connected together, but 

is there a generic symbol that I can give a name to, and anything 

connected to that symbol will be connected on the board?

 

I am sure it exists, just didn't find it browsing through the libraries.

You don't need some special symbol or device. Net names are global. As

soon as you define two nets the same NAME, they are connected (result in

a single SIGNAL in the board). You can place LABELs to show the names,

but for the connection this isn't even necessary.

You might also have a look at the PORT and XREF symbol-only devices,

they might come handy for documentation (though personally, I prefer

pure LABELs).

Tilmann