Unable to change pad signal name connected to polygon

Jeff rockel schrieb:

I am designing surface mount proto-boards. (I will upload my library once

done.) I am working ONLY in Board for this project. In my package library,

I created parts with SMD pads and through-hole pads.

 

I used "Signal" to name and connect some pads GND. I also have a polygon

on the solder side named GND.

 

I am unable to rename any of the pads that connect to GND. If I unroute

the polygon, no air-wires appear to the pads. If I use "Name" and click on

a pad, I select the nearest routed signal, not the pad. If I add a signal

from one of the pads to another net (such as VCC) I am asked to select a

name for the "combined" net. Even if I delete the polygon, I get the same

results.

 

In the attached file, please note the 4 holes on the top and bottom edge

of the board as examples.

 

Jeff Rockel

WI, USA

A layout without schematic will not generate a netlist, ergo no

airwires. If you plan to upload your library later on, I think most

users wouldn't find it very helpful if it is packages "only".

Since packages are the most difficult thing to design, the symbols are

most easy. Just a few lines and pins, or take symbols from a different

library.

So why don't you "paint" a symbol to your package and make it a device.

With a device you can draw a schematic and most of the problems are solved.

--

Gruß / regards

Joern

Joern,

Vielen dank. Yes I can do as you suggest. I have airwires for signals

connected to non-polygon net names. My issue appears to be an eagle

limitation when working in Board only.

I chose to work in Board only because the proto-board is intended to be

generic. My design is based on a board I used many years ago. It had no

through holes for connectors and was simple to make without any plating

process. The solid ground plane on the bottom is the key to good, working

prototypes.

I will take another pass and paint some symbols.

Wieder einmal, vielen dank.

Jeff Rockel

WI, USA

--

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

On 07/14/09 22:37, Jeff rockel wrote:

I am designing surface mount proto-boards. (I will upload my library once

done.) I am working ONLY in Board for this project. In my package library,

I created parts with SMD pads and through-hole pads.

 

I used "Signal" to name and connect some pads GND. I also have a polygon

on the solder side named GND.

 

I am unable to rename any of the pads that connect to GND. If I unroute

the polygon, no air-wires appear to the pads. If I use "Name" and click on

a pad, I select the nearest routed signal, not the pad. If I add a signal

from one of the pads to another net (such as VCC) I am asked to select a

name for the "combined" net. Even if I delete the polygon, I get the same

results.

 

In the attached file, please note the 4 holes on the top and bottom edge

of the board as examples.

What exactly do I have to do in that example to see the problem?

Klaus Schmidinger

--

_______________________________________________________________

Klaus Schmidinger                       Phone: +49-8635-6989-10

CadSoft Computer GmbH                   Fax:   +49-8635-6989-40

Hofmark 2                               Email:   kls@cadsoft.de

D-84568 Pleiskirchen, Germany           URL:     www.cadsoft.de

_______________________________________________________________

Klaus,

SHOW GND;

Then try and rename a drilled pad that is highlighted.

If you are able to rename the drilled pad (which is part of a package) then my experience was a fluke.

Thanks for the effort.

--

Jeff Rockel

WI, USA

--

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

On 07/30/09 22:26, Jeff rockel wrote:

Klaus,

 

SHOW GND; Then try and rename a drilled pad that is highlighted.

 

If you are able to rename the drilled pad (which is part of a package)

then my experience was a fluke.

The problem you're having is that the GND polygon prevents airwires

from being generated between the GND pads. That's because these pads

are already connected by the (calculated) polygon.

Normally you would rename the net that the respective pin is connected

to in the schematic, and the associated pad would be automatically

removed from the GND signal.

What you can do if you have only a board is to temporarily rename

the GND polygon to, say, GND1, and then do RATSNEST. Now you get

actual airwires attached to the GND pads. Delete whatever airwires

are necessary to isolate the pad in question from the rest of GND,

and then rename the polygon back to GND.

Klaus Schmidinger

--

_______________________________________________________________

Klaus Schmidinger                       Phone: +49-8635-6989-10

CadSoft Computer GmbH                   Fax:   +49-8635-6989-40

Hofmark 2                               Email:   kls@cadsoft.de

D-84568 Pleiskirchen, Germany           URL:     www.cadsoft.de

_______________________________________________________________

Klaus,

Many thanks to you and the others who contribute to this forum. I read all the posts to learn "fixes" before I encounter the "problem".

Eagle has so much embedded power, yet is so simple on the surface. The underlying design is so elegant as compared to the Orcads and Altiums of the CAD world.

Your support (and now my support, as well) will encourage more use and the continued success of Eagle and Cadsoft.

Vielen dank!

Jeff

--

Jeff Rockel

WI, USA

--

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