To all,
I would tend to agree with Mr. Lomax's version #2 also, this way the DRC is
allowed to do its job.
We used to do this with Cadnetix way back 8-10 years ago. The only thing
with Cadnetix
we could not set a footprint specific rule. We made footprints for each
trace width required which
had two pads touching. Then just swapped footprint to one needed. DRC would
then flag those
footprints but there where usually so few on a design they could easily be
identified and disregarded.
This second way also makes it part of the schematic. Just a little more
documentation friendly.
Bob Wolfe

----- Original Message -----
From: "Abd ul-Rahman Lomax" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Friday, November 23, 2001 2:50 PM
Subject: Re: [PEDA] Is it possible to create "short circuit component"
(sch+pcb)


> At 03:11 PM 11/23/01 +0200, Juha Pajunen wrote:
> >Is it possible to create a design without
> >short circuit error (sch + pcb) where two
> >different nets can be connected together?
> >For example, I need to connect two different ground
> >nets in one point of my PCB design and I do not
> >want to use R0 resistor or jumpers, I need a "wire"
> >that connect those nets.
>
> It is possible, I know three ways.
>
> (1) Set a short circuit rule that allows the two nets to short
> (Design/Rules/Other/Short Circuit Constraint). I do not recommend this
> method because no checking is done that there is only one point of short.
>
> (2) use a virtual short. this is a footprint corresponding to a jumper on
> the schematic; it can be made in many ways, but one simple way would be
two
> pads with 0.004 mil, yes 4 micro-inch, clearance between them. A clearance
> design rule allows this clearance for that footprint only. these pads will
> fabricate as a short. They can be made to look just like a wire....
>
> (3) use a mech layer and set up a special plot file for the copper layer
on
> which the short is to appear, so that the mech layer is merged for that
> plot and that plot only. To be safest, this mech layer short should be
part
> of a footprint, i.e., as with method 2, there is a jumper on the
schematic.
> (this allows moving the short around without leaving a dangerous piece of
> effective copper in some random place.) Or one could add the shorting
piece
> to a footprint manually with Tools/Change/Add selected primitives to
> component footprint....
>
>
>
>
>
> [EMAIL PROTECTED]
> Abdulrahman Lomax
> Easthampton, Massachusetts USA
>

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to