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
PCB design, consulting, and training
Protel EDA license resales
Easthampton, Massachusetts, USA
(413) 527-3881, efax (419) 730-4777

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: *[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to