----- 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 net > >identifier of 'Iret'. > >This line connects to a current sense resistor. I need to take a line from > >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 from > >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 drop. > 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 only > 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 to > >it could be (say) 0.35mm. Am I over complicating things by trying to do it > >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 of > 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 a > 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 a > good thing that if you forget to do this, you will get a DRC error, so this > 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 has > 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 only > 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: * 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
