[PCB_FORUM] Re: net-shorts

The NET_SHORT property

 

This property lets you connect two nets, like GND and AGND, to common
pin or vias, without a DRC error.

 

This property allows contact between two planes that have different net
names without a DRC error being

flagged or reported.

 

A DRC is reported if any connect lines other than the net of the actual
pin, touch the origin point of the actual

pin. The actual pin (or via) does not report a DRC for any logic objects
that touch it

.

Use the Edit > Property command to attach the property in the standard
manner to the pin and via are the only

active database element in the Allegro Find Filter.

 

The syntax of the NET_SHORT property is: <net 1>:<net 2>:....

 

For example: NET_SHORT = GND1 : GND2 : GND3

 

Method to Make Connection

 

Let's say you have two nets defined on the schematic: AGND and DGND. If
you want to tie two segments of a

split plane together at one point:

 

1. First define the split plane, and assign the nets AGND and DGND to
the appropriate segments of the

plane.

 

2. You can make this connection in multiple ways: using two vias, using
one via and one pin, or connecting

directly between two pins. No matter which method you choose, one pin or
via must have the

NET_SHORT property added to it.

 

3. If you chose to use two vias, place one via into the AGND shape and
one into the DGND shape by

selecting the Route > Connect command from the pull-down menu.

 

A. Click on the AGND plane to start a route.

 

B. Immediately click either your right mouse button, then select Add Via
from the pop-up menu, or

double click the left mouse button to place the via.

 

Gerry Meier, Sr. PCB Designer

Freedom CAD Services. Inc

Email:gerry.meier@xxxxxxxxxxxxxx

visit us at http://www.freedomcad.com

 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Ed Caldwell
Sent: Thursday, November 08, 2007 6:14 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: net-shorts

 


Legally you can short around the cap or res in the schematic with a
wire.  This is safe and design driven. 

Illegally you can add a shape/trace to a graphic (user defined) layer
and include that layer in the artwork generation but this can be
dangerous especially in future spins. 

Ed
http://www.eds-pcb.com




"Tmi Systems PCB Design - Amin Aslan" <amin@xxxxxxxxx> 
Sent by: icu-pcb-forum-bounce@xxxxxxxxxxxxx 

11/08/2007 03:57 AM 

Please respond to
icu-pcb-forum@xxxxxxxxxxxxx

To

<icu-pcb-forum@xxxxxxxxxxxxx> 

cc

 

Subject

[PCB_FORUM] net-shorts

 

 

 




is there a way to short a res or cap without creating drc ???   just
like  0 ohm resistor thanks 
  
may be inside the dra  if possible 

________________________________

Other related posts: