Quoting Ken Zig <kenz...@yahoo.com>:
I am currently working on the EAGLE node 5 front end schematic and
have a few questions. So far I have removed the portions of the SPS
that I do not want to use. I have inserted some of the new SPS
design, and I have inserted the new LPC2368 controller. I have not
yet wired anything to the LPC2368, only moved the existing design
around enough to fit it into the schematic. The file as it stands
has been pushed to avionics-cad/lv2-node5/node5-frontend-rev1.sch so
you can see where I'm at as of now, though I'll still be changing
it throughout the night. As for the questions:
Is there a way to copy and paste from one .sch file to another in
EAGLE? It seems that I may be able to do this by moving one
schematic off to the side and using the diff of the exported script,
but that proved somewhat difficult and resulted in many errors.
Yes. It's odd, but it works well.
-Open the source schematic
-Surround the stuff you wish to copy with the group box
-Click CUT (scissors)
-Click GO (right click mouse) to select group at center
-Open destination schematic
-Position parts and left click to set
Can I surround the new IC with a bus and make every pin go directly
to the bus? I see in the existing .sch that several pins skip the
bus and then run around the page, this seems pointless, but I may be
missing something fundamental here.
Using buses in this way is common in industry, even with other
(better) CAD tools. It may help if you use a few buses with different
purposes, i.e. an analog bus, a digital IO bus, an external parallel
memory bus, etc. as needed by your application. The point is to
connect the nets for your layout, but also to make your schematic
clean so that mistakes are obvious and therefore caught in the review
Can I make the schematic bigger, or is it already a standard size?
Actually, the only reason I can think of to limit the size is so you
can print the schematic. I have borders (frames) drawn to 11x17 size
paper. If you only work with it in electronic form, it can be any
size. That said, remember the comment above about making errors
obvious. You are less likely to miss errors if the whole thing is
clean and on one page. If you cannot cleanly place everything on one
page (with whitespace to separate subcircuits), then a multi-page
scheme with power, digital, analog, clock, etc on separate pages can
help a lot.
If it's already a standard size, should I add new sheets if I run
out of room? In this case it almost seems like there should be a
separate sheet to house the power diagrams leaving the bus to carry
the control signals between sheets and using port symbols for power
connections on the Micro-controller sheet.. (I have not been able to
get EAGLE to let me make a new sheet yet.)
You can't make multiple sheets unless you have the full (not free)
version of Eagle.
Hope this helps.
psas-avionics mailing list