Hi Ted,
Thanks for the rundown on the multi part ICs. I recall drawing 7400
series gates into schematics with Orcad that way. I haven't come to it
in Eagle.
I'm still wanting to get rid of the offset I mentioned being in my
design. Seems that although the "positive coordinate" option switch
gets rid of the objectionable offset, DeskPCB doesn't like it! So I'm
stuck getting the border aligned better. I shrunk my board outline to
fit 3" x 4", and lost my corner holes (for now). The origin is now on
the LL corner, I'm hoping I've solved the problem.
When I last tried to convert Gerber to DXF and overlay the component,
solder and silks, they don't line up (offset somewhere).
One thing that would help is the registration marks for the board. I
wanted to use the four corner holes I initially designed into the board,
but I can't get them into the 3 x 4" Eagle envelope. I haven't found
the symbol to put on the silk layer yet. Maybe that will help the
alignment. I want to make the layers correct for a board house to
produce eventually.
73's,
Alan KM6VV
kilocycles wrote:
> 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,
>>