Homebrew PCBs

Alan,
I'm not quite sure what you mean when you say recenter the border.  On
a few occasions, I've manage to lose one of the border lines on my
board, on-screen anyway.  I don't know how, I just accidentally
deleted it, probably while deleting a polygon.

You can recenter or otherwise move the whole layout, or a part of the
layout, in effect changing the distance to the border or edge of the
board,  by grouping and moving it.  The Group icon is the larger of
the two open/closed brackets-looking things on the left.  Select that,
then turn on all of your normal layers, and draw a rectangle around
all the components you need to group and move.  They will turn red and
black highlghted on-screen.  Then click the Move icon, and use
RIGHT-CLICK to drag the layout to wherever you want it.

By the way, I figured out how to make multipart ICs yesterday.  I was
working on a 74HC4053 MUX/DEMUX (actually, three single pole double
throw switches with 5V logic control lines).  I wanted each switch
section to appear where it needed to be in the schematic, rather than
having all net wires coming in to a 16-pin symbol.  Op amps are done
the same way.  I drew each switch section symbol with its pins and
saved it under a name, beginning with 74HC4053A (note-I changed the
pin names to the actual pin numbers of the DIP package).  The next
section was then 74HC4053B, etc.  The last section was the ground,
supply, and two other pins that are usually tied to ground.  The
kicker is to assign the first symbols pins as swap level 0, the second
swaplevel 1, etc (that's a drop-down box).

When creating the 74HC4053 device, import first the 74HC4053A symbol,
and look at the drop-down boxes at the upper left.  Keep this one at
swaplevel 0, and make sure addlevel is "Next".  Then, import the next
symbol with its set of pins, and set swaplevel to 1, and addlevel to
"next".  Just put the second symbol right on top of the first.  The
third switch section will be swaplevel 2, addlevel "next".  The 4th
section is the power section, and it's swaplevel 3, but assign
addlevel or "Always" if you want it to always be shown on the diagram.
 If you want it to show only when you type "Invoke" to show power
sections on the diagram, set addlevel to "Must". (I used always).  Put
it somewhere beside the pile of 3 switch section symbols on the screen.

Then create the device by clicking on "New" to bring up the package, a
16-pin DIP.  Then "Connect" to synchronize the symbol pins with the
actual pad numbers one by one.  That's easy if you've changed the pin
names to match.  Finish the device by assigning a default designator,
U or IC or whatever, add a description, and save the library.

When you call the part into the schematic, the first switch section
will appear, along with the power section.  Click again, and the
second section will appear, again, and the third will appear.  Now, if
you're using the device to switch between two LC filter sections, one
narrow and one wide band, for example, you can drag one section to the
input, and drag one to the output.  You can mirror one of the sections
so it's facing the filters in the correct orientation. The schematic
looks a lot cleaner and easier to read.

By the way, this IC draws only 4 uA, as opposed to the 16 to 50 mA or
more of a sensitive relay.  Steve Weber, KD1JV used the device to do
the bidirectional mixer switching in his Minimalisist SSB transceiver.
 I've been using it in my designs ever since. 

Ted
--- In Homebrew_PCBs@yahoogroups.com, "Alan Marconett" <KM6VV@...> wrote:
>
> HI Ted,
> 
> Thanks for the kind words!
> 
> Yes, I'm fascinated with the simple, elegant steam engine designs of the
> past.  Not so much on the RR's, but that may develop later...
> 
> I have a little QRP paddle, and I've drawn it up.  I've also taken a
GOOD
> look at some of the really nice keys out there.  I believe I could
design
> and build a reasonable hand key.  Just too many other interesting
things to
> do!
> 
> I have a few small CW transmitters in the closet that I intend to
restore.
> A Johnston and a Heathkit.
> 
> For now, I intend to get going on PCB's.  And there's the PCB router
parts
> that are taking up space and not being useable... yet.
> 
> I'm still making minor improvements in my board layout, and in the
parts I
> incorporated into my design.  Seems they don't look equally well when it
> comes to exporting Gerber files from Eagle.  Outlines which must be
on the
> wrong layers, funny pad sizes/shapes.  And now it appears that I'm a
"little
> too big" in my layout (pushing the envelope), I've lost part of my
board!
> 
> I'm using DeskPCB to do generate the isolation toolpaths, and export
in DXF.
> This allows me to import into Vector CAD/CAM and examine it thoroughly. 
> 
> Can I re-center the border on my board?  Just erase and redraw it?
> 
> 73's,
> 
> Alan  KM6VV
---snip---