Mail Archives: geda-user/2015/08/18/07:48:24
Matt Rhys-Roberts (matt DOT rhys-roberts AT envinsci DOT co DOT uk) [via
geda-user AT delorie DOT com] schreef op di 18-08-2015 om 11:21 [+0100]:
...
> > The pads are indeed numbered in order of creation. In my experience, you
> > can simply renumber the pads in the footprint file. Just make a note of
> > how the numbers should change from what you see in PCB beforehand.
>
> Hi Richard. Ok, thanks
>
> > The best approach is to number pads during creation. Each line that is
> > to become a pad can be assigned a number by pressing N while hovering
> > over it; just enter a number as the Line Name.
>
> Oh dear, have I messed up here? I created my very specifically sized
> pads using rectangles on the top layer. I have seen that some ready-made
> elements break down into round-ended top-layer lines, which can be
> squared afterwards... Am I breaking the rules by trying to use
> rectangles instead in the first place?
Well, I'd say that the rules are that you can do anything that works for
you :-)
I always use lines for creating pads, because rectangles can't be
numbered. Then again, rectangles are easier to dimension correctly than
lines.
I draw lines of the required lengt minus the required width (since this
width will be added to the rounded ends again), and then set the width
using the :ChangeSize command. After converting the footprint to an
element, I use Q to convert rounded pads into rectangles (and pressing Q
while not hovering over a pad will toggle rectangle/round for all pads).
And yes, if you use rectangles to define pads, then convert the
footprint to an element, and then break it apart again, the rectangles
are converted to lines, not rectangles. So that tells me that using
lines is the expected way to go about it. But if you find it more
convenient to use rectangles and subsequent renumbering the footprint
file, that seems OK as well.
And of course it's always a good idea to double check pad/pin numbers
and dimensions by drawing a simple test schematic, importing this in
PCB, and also printing it to see if the part actually fits. Especially
with connectors, manufacturers' drawings are sometimes a real pain to
translate into a properly dimensioned (and numbered!) footprint, and
I've had several embarrassing moments when things wouldn't fit on a PCB
I ordered.
> > When dealing with structural metal parts such as mounting tabs and pins
> > on connectors, I usually assign these the number 0 (zero) -- although
> > the gschem symbol should have a corresponding pin if these parts are to
> > be connected to a circuit net (usually GND). Perhaps other people use a
> > different approach here?
>
> I too have several pads that all connect to a connector's shield ground;
> it would be nice if I could call them by same name. I've been numbering
> them uniquely, pending a better strategy :D
I think it's sensible to give them all the same pad number (I use 0), as
this reflects the fact that all pads of a shield ground are usually
connected through the connector.
Using a separate numbering for each pad makes things unnecessarily
complicated -- unless of course you actually have isolated metal parts
that you want to connect to different nets. But I'm curious what others
may have come up with.
Best regards,
Richard
- Raw text -