Thrilled with Eagle EDA

[Winston]

So I'm hacking together this little SMT sensor board.
Standard vanilla everything. Two layers 0.063" FR-4.
I stumble across this command 'Polygon' and start fiddling with it.

Before long, I have contiguous GND *and Vcc* planes
underneath my most sensitive amplifier and everything
routes automagically with minimal clean up.

On a *two* layer board, with no drama and no real work.
It's a miracle.


--Winston <-- Now grinning in an unprofessional manner.

 

[Winston]

No drama, no real work, and very likely no actual ground connections to
parts of the polygon.

If you lay out the polygons first, then route your board, Eagle will
happily cut those polygons into multiple, disjoint pieces. Then it'll
route power and ground traces from the islands.

Route the board _first_, then lay down the polygons -- then it'll become
apparent which parts actually connect, and which don't.

I do two-layer boards with "mostly GND fill" by laying down polygons on
the GND net after autorouting, then I go and put in vias as necessary to
reconnect the various islands and isthmuses to the ground plane.

Oops. Good catch.

I phrased that poorly, indicating that I had autorouted over
the planes rather than what I actually did, which was autoroute,
disconnect the Vcc and GND nets and *then* applied both
the Vcc and GND planes.

I was trying to communicate that the 'Vcc' and 'GND' connections
automatically connected themselves to the proper plane (after
'naming' the plane, doing the obligitory 'ratsnest' command and
connecting vias where necessary. There was a little additional
cleanup involved in managing current flow, but I am still
astonished how easy that process can be.

I let my enthusiasm get in the way of clarity there.


--Winston

 

[Grant]

So I'm hacking together this little SMT sensor board.
Standard vanilla everything. Two layers 0.063" FR-4.
I stumble across this command 'Polygon' and start fiddling with it.

Before long, I have contiguous GND *and Vcc* planes
underneath my most sensitive amplifier and everything
routes automagically with minimal clean up.

On a *two* layer board, with no drama and no real work.
It's a miracle.

Sure is, I played with the polygon and nothing useful came out of it, can
you put a demo file up somewhere?

Or describe a command sequence that will let me see it work? I've read
the polygon command is the right one for filling or pouring copper.

Grant.

 

[Winston]

Sure is, I played with the polygon and nothing useful came out of it, can
you put a demo file up somewhere?

This guy did a far better job of it than I could've:
http://www.muzique.com/schem/eagle.htm

The only difference is that in the fifth picture down, I type 'rats'
in the command line box to make the plane visible, because
the solid fill does not appear after 'naming' it, at least for me.
On opening my file for example, I notice that the planes are never
visible until I've typed 'rats'.

Here is a time-saver. When you want to edit your board after having
poured one or more planes, type 'show' and click in the border area
where you first outlined the plane. After one dotted outline
'highlights', type 'rip' and click on that border once more.
The plane will revert to it's 'outline' rather than 'filled'
appearance. Don't panic! You have *not* lost your plane.

Repeat these two steps for each plane on your board.
Note that it is *not necessary _or_desirable* to _delete_ any plane's
outline border if you are happy with the outline geometry.
After editing your board, just type 'rats' again and your planes
will be re-generated *including allowance for your edits*.

It is magical to watch, IMHO.

Let me know if you run into difficulty with this.

--Winston

 

[Winston]

This guy did a far better job of it than I could've:
http://www.muzique.com/schem/eagle.htm

The only difference is that in the fifth picture down, I type 'rats'
in the command line box to make the plane visible, because
the solid fill does not appear after 'naming' it, at least for me.
On opening my file for example, I notice that the planes are never
visible until I've typed 'rats'.

Here is a time-saver. When you want to edit your board after having
poured one or more planes, type 'show' and click in the border area
where you first outlined the plane.

If your plane's dotted outline does not show up, right mouse click
in that border and click on 'next' in the resulting dialog box until
the dotted outline does appear.

After one dotted outline
'highlights', type 'rip' and

click on that border once more.
The plane will revert to it's 'outline' rather than 'filled'
appearance. Don't panic! You have *not* lost your plane.

Repeat these two steps for each plane on your board.
Note that it is *not necessary _or_desirable* to _delete_ any plane's
outline border if you are happy with the outline geometry.
After editing your board, just type 'rats' again and your planes
will be re-generated *including allowance for your edits*.

It is magical to watch, IMHO.

Let me know if you run into difficulty with this.

--Winston ​

​

 

[Winston]

Eagle EDA does have an unattractive feature.
Running the CAM process produces results that has a
random X,Y offset added to the real numbers.

Here is my workaround:

Make sure your entire design is located +X and +Y (above and
to the right of) the little '+' fiducial on your screen.

In your source file, place a 0.001" hole at some obvious
location on your board near the lower left corner.
I shall use X 1.0, Y 1.0 for example.

Run the CAM process to generate your Excellon drill file.
Remember to manually add the '.txt' suffix to your suggested
file name for results and remember to click on the dialog
box *twice* because you are processing both 'pads and vias'
and 'holes'.

Open your Excellon *.txt file and find your 0.001" dia hole
within. Note it's location.

Run the CAM process once more and edit the 'offset' variable
to cancel the offset in the results file. Recently, for
example, I cancelled their error when I plugged in an offset
of X = 0.0010", Y = -0.0151". The 'Y' offset will eventually
show up as a metric value while the 'X' offset will remain
in olde englishe inches. It's a feature.

Run the CAM process again and confirm that your 0.001" hole
is now shown at X = 1.0000, Y = 1.0000 in the Excellon file.

After every few edits, run the CAM process again and adjust
your offset as necessary to bring your 0.001" hole error
back to zero. Make note of the location of a nearby
'real' pad or hole for future reference.

Just prior to generating your real CAM files, delete your
0.001" hole and use the location of your 'real' pad or hole
as a sanity check for your real CAM output.


--Winston

 

[Winston]

[email protected] wrote:

(...)

if you turn of orphans on the plane the unconnected islands will
disappear making
it easy find them

Cool! Thanks.

--Winston