> -----Original Message-----
> From: Rene Tschaggelar [mailto:[EMAIL PROTECTED] 
> Sent: Saturday, December 06, 2003 4:51 PM
> To: Protel EDA Forum
> Subject: Re: [PEDA] double pins
> 
> 
> Thanks a lot John,
> (both your posts reached me at almost the same time)
> I had a very quick look before going to dinner.
> The point appears to be that the second row of pads
> is named with an 'A' attached. So '1' and '1A', '2'
> and '2A', and so on.

Rene

You will see from the example board I uploaded, both methods,
1,1,2,2,3,3.... And 1,1a,2,2a,3,3a  work fine at first import to the
PCB. Only drawback with the latter is that you need a second part to the
SCH symbol and must draw/wire it on the SCH. 

But as you have all the pins named differently, you have more control
over connectivity while making it still to be 'readable' in some sense
as the pin number only has a suffix.

But if you use the 1,1,2,2,3,3... Method then do some things like update
the footprint, or otherwise update the net list from within the PCB then
the net list used by the DRC seems to get corrupted.

I always use the 1,1A method which never fails.

John


> John A. Ross [Design] wrote:
> 
> >>-----Original Message-----
> >>From: Rene Tschaggelar [mailto:[EMAIL PROTECTED]
> >>Sent: Saturday, December 06, 2003 2:18 PM
> >>To: Protel EDA Forum
> >>Subject: Re: [PEDA] double pins
> >>
> >>I'm usually coming from the Update design, update footprint,
> >>... This time I also tried to create and load a netlist 
> >>manually. It didn't work as it didn't assing a net to both, 
> >>just one. I also found the soldermask to be negative. How do 
> >>I cover something that is blank copper ?
> > 
> > 
> > Rene
> > 
> > I assume you are meaning a pad, in which case you could add 
> a negative 
> > clearance value to the pad which is enough to cover the pad 
> completely 
> > . If this is to be a permanent changes, then do this at footprint 
> > library level, as any time you update from the PCB library, users 
> > changes will be over written.
> > 
> > I also suspect you may have done a footprint update on the 
> part after 
> > loading the original netlist.
> > 
> > This is not that reliable when using the same number' 
> methodology, it 
> > does work, but only reliably at first import when no primitives are 
> > connected to the pads. If you make any footprint updates 
> then you can 
> > expect issues. Trying to re-import the netlist using 
> netlist load or 
> > update PCB sometimes just does not work.
> > 
> > I uploaded a sample design for you to 
> > http://www.proteluser.com/download/same_pinno/ which is a 
> recreation 
> > of what I seen happening. It is almost exactly like your 
> example here.
> > 
> > I avoid using this same number method for connecting rows in 
> > preference for two part symbols with 1,1A type naming conventions, 
> > wherever I can, especially if the footprint is not mature 
> and is being 
> > updated.
> > 
> > Hope that test board makes sense to you, I opened it up and checked 
> > all was Ok before uploading it (it is old)
> > 
> [snip]
> 
> 
> 



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to