What:
This is the recipe for adding more sheets or re-ordering your existing
sheets for a project after you've already completed or done some layout.
Motivation:
I completed my first project that was faily complex with about 200
components and a torturous layout with nasty board dimensions. Being an
Eagle noob I did it all on one schematic sheet. On my second project, that
had even more components, I realized that printing out multiple sheets and
patch working them together sux, so I figured out Eagle's multi-page aspect
and am quite pleased with it and the results.
But, looking back at the first third of the job I was disgusted with the
unprofessional single schematic page and decided to break it into multiple
pages.
As you know with Eagle's automatic updating of the layout, whenever things
change on the schematic - they change on the layout. This process can be
highly destructive to an existing layout. It will rip up traces or
re-number parts.
Couple the cross annotation with the auto part numbering and havoc can
follow.
To pull this off successfully you need to follow this recipe.
Recipe:
1) Make one or two backups of your existing schematic and the board files.
Something like: ExistingNameHACK1 and ExistingNameHACK2. Using "Save as"
2) After 1) above, you should be sitting on: "ExistingNameHACK2".
3) Close the existing board: "ExistingNameHACK2.brd". This suspends the
the automatic updating, freezing your layout.
4) In the schematic you want to FILE>EXPORT>Partslist to
"ExistingNameHACK2.partslist" Note where it lands.
5) Open "ExistingNameHACK2.partslist" in your favored editor.
6) Starting at the top of the partslist look at the "Part" column. You
will see for instance C1,C2,C3...... If there are less than about 10 of a
type part, check them for all values being there - NONE can be missing. If
there are none missing move on down to the next type of "Part". If there
is one part in the sequence missing then go onto the schematic and copy any
same-type part that you see to add another one. This will fill in the
missing values.
Go down the partslist until these are all taken care of. If there are more
than 10 values of a type of part, DO NOT trust your eye. Just copy a
same-part adding it to the schematic. Do this until you see the next added
part is numbered higher than the highest numbered one of the same type in
partslist. Once you get one higher, UNDO and move down partslist to the
next Part. Typically Resistors and Capacitors would certainly get the
blind - add treatment. If the first add is a number higher than the
highest on partslist just UNDO and move on.
7) Now you likely have a little group of added parts on the schematic up it
some corner from 6). Good, leave them there, never to mingle with the
rest.
8) Add as many pages as you think you'll need. DRAW>FRAME putting in
frames, if you desire, on each of the new pages. I start them exactly on
the new page's X and run them out to half an inch of my printer's page size
Ex: (16.5" x 10.5"). This shows how much room you have to keep all the new
page's circuitry in your printer's paper size.
9) Look at your one page schematic and decide how you want to break it up
into a logical several pages. Since this is just to fix a single page
situation don't knock off a nasty chunk that requires a bunch of signals
moving to multiple pages as it will be horribly tedious and easy to screw
up.
For example, you may want to move the displays to a new page and the power
supply to yet another page.
Move these areas into groups that you can hack out when you're ready. Now
use the label command to label each signal that will span from the first
page to one of the new pages. Typically you will have a signal called, for
example, "N$37". On the same net add another label - it will be the same.
Cut the net somewhere convenient between the two labels. Now, using the
"NAME" function rename both sides something descriptive like "CLK".
10) Repeat 9) until all nets that will be severed, to break up the monster
page, are done.
11) Now using Eagle's psychotic cut and paste method, GROUP>CUT>rightclick
on screen to save the sub-area we're moving into the paste buffer. Now
'pick' the DELETE button and right click to delete the same GROUPed parts.
pffft! They're gone - existing only in the paste buffer. Those preventing
renumbering of these parts when they're PASTEd.
12) Go to the new page and PASTE. You now have the moved circuitry on the
new page - with no renumbering.
13) Repeat 9) thru 12) until you're satisfied with your newly broken-up
schematic.
14) Go back to the first page and blitz all the components you had to add
to fill the Part listings. This prevented ANY renumbering.
15) This is a good time to SAVE.
16) Open up "ExistingNameHACK2.brd". There will be squawking about "No
Annotation because their are inconsistencies!!!" Fear not this is
expected.
17) What has happened is that traces on the board were all previously named
from the net names on the schematic. Recall that we just put useful names
on the nets we had to cut to 'multi' the schematic. The inconsistency is
that now the existing traces don't match the new names we just assigned.
On the schematic page run the ERC, the Electrical Rule Checker. You will
get a bunch of pretty lavender Consistency Errors. You will immediately
see the new names you assigned paired up with the old net names still
residing on the layout's traces. "N$37", etc.,etc.
Minimize the schematic somewhere and move the ERC window to the side. Click
on an Inconsistency. This boxes one pin on a contested trace on the board.
Again using NAME select the the PIN or Trace. Looking at the ERC list
reNAME the trace to the name you recently gave the net on the schematic.
18) Repeat 17) until you've done all the inconsistencies. If they're
listed twice you can ignore the second complaint. Once you've reNAMEd them
all run the ERC again. There should be none! If there is, just address
them. Do this until there are none left.
19) Save.
20) Examine your layout. You should see no changes from the original. If
this is the case you've been successful. P A R T Y T I M E!
You can Save as back to the original name or the original name with some
minor addition. "Multi" or *ms".
Caveat. There is some aspect about Eagle and gates spread around different
sheets. I am too much a noob to know what ramifications this would have
with the above process. Perhaps someone can add that.
--
Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.
