At 04:36 PM 6/8/01 -0500, Tim Hutcheson wrote:
>Anybody know how to back annotate
As far as I know, Protel does not support automatic back-annotation for
gate swapping (and resistor pin reassignments are a variation on gate
swapping.) Swapping requires symbol level definitions of what can be
swapped. For example, the two inputs of a NAND gate can be interchanged,
and any NAND gate in a 7400 package can be interchanged with any of the
other three. But a different part will have different allowed swaps. The
intelligence is simply not built into the parts.
When I have needed to reassign simple parts, I've done it manually. It's
not at all difficult and errors, of course, fall out in the wash (i.e., the
final DRC).
For complex swapping, I've made dummy parts. I took a large gate array once
and made a pile of single pin components that were numbered (refdes)
according to the array pin numbers. As I routed the array, I picked up the
individual parts and rearranged them for good routability. At this point I
made a list of the final part sequence around the array and manually
transferred this information to the schematic. But I could have renumbered
them and used back-annotation. How I dealt with the schematic I don't
recall. I may have made a special symbol, or I may have rerouted the wires
or rearranged signal names.
For pullups, using dummy parts, one part per pullup pin, would work pretty
well. (using dummy parts both on the schematic and on the PCB). When one is
done, finalizing the schematic would involve changing, for example,
RP13_8-X (a single pin part with refdes RP13_8 and pin name X -- arbitrary
--) to RP13 part 8 (which might be actual pin number 9, but it is the part
number which will be used when replacing the parts with real multipart
symbols).
It sounds more complicated than it is.
To manipulate the dummy pins, the real footprint for the multipin part can
have its pads moved to a mech layer. They can then be used to snap the
single pin parts.
However, I don't do nearly as much swapping as I used to. Unless a design
is very dense or has other special requirements, it can be more trouble
than it is worth, it being simpler to draw the schematic and then route the
board where it falls.
As to the future, the ability to swap parts would indeed be valuable. Even
better would be swapping built into the autorouter (or, more accurately,
probably, into autoplace since the kind of intelligence needed is similar
to what an autoplacer needs to apply). It could be assumed that any part
with the same footprint and same type and value could be swapped with any
other such part; within parts the two ends of non-polarized two pin parts
can always be swapped; and then other more complex kinds of swaps would
need definition. Such definitions would probably be made at the schematic
library level, but the information would need to be accessible to PCB.
Further, in both the schematic and PCB documents, "swapping allowed" would
be a part parameter.
I might or might not be able to swap the address lines of an EEPROM, for
example. If it is programmed in-circuit, swapping should be fine, but if it
is programmed in another device, it could be quite confusing.
That none of these parameters exist -- at least I haven't seen any sign of
them -- is a pretty good clue that it is not supported, not to mention that
there is no mention of swapping in the manual.
[EMAIL PROTECTED]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
