Jeez, you guys do things the hard way, I just use a zero-ohm resistor, it's
a standard part available from multiple sources in any size from 0201 up to
2512. This works especially well for maintaining multiple grounds with a
single point tie. 

> -----Original Message-----
> From: Abd ul-Rahman Lomax [mailto:[EMAIL PROTECTED]]
> Sent: Thursday, February 21, 2002 13:08
> To: Protel EDA Forum
> Subject: Re: [PEDA] Tie compoents(Ex: RF footprints)
> 
> 
> At 01:10 PM 2/21/2002 +1100, Ian Wilson wrote:
> >There are a few workarounds.  The one that I think is most 
> documentable 
> >but sometimes subject to Gerbering issues is the Lomax Virtual Short.
> 
> Note that Lomax himself now considers as at least equally 
> satisfactory the 
> use of mech layer shorts merged in the gerbers through CAM Manager 
> definitions (which can be named, helping with documentation 
> for future 
> generations), the shorts being part of a special jumper 
> component, just as 
> with the virtual short.
> 
> Note that Schematic control of the short is a very important 
> part of any 
> solution. Schemes which do not automatically create and separate nets 
> except at one point, the visible and controllable short 
> between nets, do 
> not satisfy this criterion; specifically this would be an 
> argument against 
> the modification of split planes as some have used.
> 
> >Basic method: make a really small gap between two small pads 
> (0.1 mil), 
> >give each pad a name and then create a special clearance 
> design rule to 
> >allow such a small gap between these pads.  Issues to watch 
> for are gerber 
> >rounding and aperture matching.  So set a tight apt matching 
> tolerance and 
> >set gerber to include more than the standard 3 decimal figures.
> 
> It is best if the pads in question are part of a jumper which 
> appears on 
> the schematic; the whole process becomes automatic at that 
> point. Want a 
> single-point ground? Put a single-point ground jumper on the 
> schematic. 
> With the virtual short you will need to set a design rule 
> allowing the pads 
> of that component to be so close to each other; with the mech layer 
> solution, you still need to set up a special gerber definition and, 
> preferably, to name the mech layer or layers used appropriately.
> 
> The gap should be smaller than 0.1 mil in my opinion. I've 
> used 0.002 or 
> 0.004 mil. Protel can get a little flaky in the sub-mil 
> region, so one may 
> need to experiment (examples have been given in the past of sizes and 
> definitions known to work).
> 
> PCAD has tienet polygons. I consider that solution, as far as 
> I understand 
> it, as inferior to either of the workarounds we have at present.
> 
> I've described in the past various alternatives, I think, as 
> to how Protel 
> could make this a directly accessible feature, instead of merely a 
> workaround. Instead of going down that road again, I'll just 
> state what I 
> consider desireable.
> 
> I want to place a symbol on a schematic; it may have any 
> number of pins, 
> and these pins will be kept separate for netlist generation. 
> However, the 
> footprint which is associated with this symbol may have pads 
> which are 
> shorted together without creating any DRC error.
> 
> This, I think, would actually be quite simple to implement, 
> it is really 
> only a little jiggering with the DRC routines. Perhaps the 
> routines would 
> recognize something about the name of the symbol, in the type field 
> perhaps, since that is fixed to be generated from the symbol 
> name, which 
> allows shorts between the nets of the pads to take place 
> within the pad 
> areas, whether by the pads themselves shorting or by track 
> connected to the 
> pads (provided that they only short within the pad area, not anywhere 
> else). No special rule should be needed, because it is extra 
> work to create 
> such a rule and errors may take place during that. More than one name 
> should be possible for this symbol, so perhaps the name would have a 
> controlled prefix, such as PCBSHORT.
> 
> Protel support is distinct from Protel engineering. While we 
> would wish 
> that support personnel would read and be familiar with this 
> list, I don't 
> think that they are at this time. I might be wrong about 
> that, at least 
> with regard to some. I've many times said that it is 
> completely natural and 
> to be expected that this list can provide better support than 
> Protel; I 
> would suggest, in fact, that Protel abandon much of its 
> direct support and 
> direct the funds freed up by this to software maintenance and 
> development. 
> Basically, issues that were not resolved quickly on this list 
> would then be 
> referred to support personnel, who would be very closely connected to 
> engineering.
> 
> This list generally answers questions more quickly than 
> Protel support 
> could possibly manage unless they were to throw a *lot* of 
> money into the 
> effort. And that would be silly.
> 
> [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