----- Original Message -----
From: "Abd ul-Rahman Lomax" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Wednesday, September 03, 2003 4:50 PM
Subject: Re: [PEDA] Joining 2 different nets keeping seperate identifiers?
> At 07:09 AM 9/3/2003, Joe McCauley wrote:
> >I need to have a current return line with 3mm thickness. This line has a
> >identifier of 'Iret'.
> >This line connects to a current sense resistor. I need to take a line
> >this resistor to an amplifier input.
> Here is what I understand from this: this circuit is measuring current by
> measuring the voltage drop across the sense resistor. The current being
> measured is sufficient that a 3 mm trace is required. Presumably the
> temperature rise calculations have been done.... Or the trace is that fat
> so that error due to voltage drop in the trace is minimized.
> >There is no need for this amplifier input line to be 3mm thick, in fact
> >the point of view of routing it would be better if it were not!
> Mr. McCauley writes about one line. Really, there are two, since one is
> measuring the voltage drop across a resistor. Of course, if there is a
> solid enough ground at the ground side of the sense resistor, one might
> assume that the drop in that part of the circuit can be neglected. Or
> perhaps the circuit will be calibrated to account for that additional
> Otherwise one needs *two* sense lines, which will feed a differential
> amplifier of some kind.
> Presumably there will be negligible current in the sense line (the
> "amplifier input line.") At least whatever measures that voltage should be
> designed to minimize the current. So the line can be narrow, really it
> needs to be wide enough to be reliably fabricated.
> > Is there a
> >way of joining 2 different nets in the schematic while keeping seperate
> >identifiers? If there were then I could setup the design rules in PCB to
> >always have the 'Iret' net 3mm thick, while the other one which connects
> >it could be (say) 0.35mm. Am I over complicating things by trying to do
> >this way?
> I don't think so. I'm from the school that thinks that good DRC is very
> important. You can certainly accomplish what you want by setting the
> minimum thickness for Iret at 0.35 mm and the maximum at 3 mm. But this
> won't guarantee that you get 3 mm where it is needed.
> There might be some way to do this with from-tos, as mentioned by another
> designer, but I don't know that. I do notice that From-To Class is one of
> the possible attributes controlling width rules, but I've never
> investigated that rule. Maybe I should read the manual.... Naah, that's
> something I recommend to others, I don't do it myself.... :-)
> As mentioned by Mr. Ross, the so-called "virtual short" will accomplish
> this. Once you have built this footprint, have placed a symbol for it on
> the schematic and have wired it, and have set a design rule for the
> footprint (or component class, if by some chance you had different kinds
> these creatures), it is pretty much set and forget.
> You would have your IRet net, being the return net for your large current.
> Then you would place, on your schematic, the virtual short, which is, for
> schematic purposes, a jumper. One side of the jumper is connected to IRet,
> typically right at the sense resistor pad. The other side of the jumper is
> connected to your sense net that goes to the amplifier. You could actually
> make the jumper structure part of the sense resistor pad, which would
> guarantee that the short is placed in the proper location. In other words,
> you'd build a symbol and footprint for the sense resistor that had two
> extra pads for the sense connections.
> These pads have a gap between them which is below fabrication possibility.
> Properly designed, there will actually be *no* gap on the films, because
> the gap will be well below the gerber resolution. It might be, say 4
> microinches. (Protel can get a tad flaky in the microinch region since
> that's the database resolution, as I recall, otherwise it could be 1
> microinch!) Then a design rule allows pads in that particular footprint to
> be very close to each other, say 2 microinches, without creating a DRC
> violation. By the way, you'll use rectangular pads....
> How do you make the virtual short? I described above the principle for
> using fabrication limits to create a physical short that Protel considers
> as being unconnected. There is at least one other way, which became
> practical and reasonably safe when the CAM Manager was created, allowing
> custom CAM setups for your design. One of the mech layers is dedicated to
> short, that is, a shorting trace is on that mech layer. It is merged with
> the normal layer as part of the CAM definition for the normal layer.
> With the fabrication limit method, you need to create a design rule. It's
> good thing that if you forget to do this, you will get a DRC error, so
> is quite safe. The down side of this method is that if you aren't careful
> about how your CAM pad definitions are created, roundoff can leave a real
> gap on the film and a helpful fabricator will increase it for you, this
> actually happened. The mech layer merge technique will produce a
> bulletproof fab film, but if you forget to create the CAM definition for
> the merge, or it is done incorrectly, there will be no DRC warning.
> Generally, once one has verified that whatever setup you use is working
> *and that there is no gap, i.e, that the gerber pads, as defined, are in
> actual contact (i.e, below 0.1 mil or whatever resolution was chosen for
> the films), it will continue to work, i.e., whenever changes are made to
> the design, DRC will verify that the widths are correct.
> Virtual shorts are useful wherever you want a copper connection with two
> separate nets. Examples would be:
> RF parts, such as inductors, made with traces.
> Separated grounds, such as DGND and AGND, which are connected together but
> which must be controlled to be in two (or more) different nets tied at
> one place.
> And, this application: sense lines used with high-current traces.
> Abd ul-Rahman Lomax
> LOMAX DESIGN ASSOCIATES
> PCB design, consulting, and training
> Protel EDA license resales
> Easthampton, Massachusetts, USA
> (413) 527-3881, efax (419) 730-4777
> [EMAIL PROTECTED]
> 1 Protel 99SE license for sale, $3500 OBO.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
* Forum Guidelines Rules:
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *