Re: gEDA-user: adding footprints attribute to schematics symbols

[DJ Delorie <dj@xxxxxxxxxxx>]

> I give fottprints attributes for CONN1, CONN2 & CONN3. Are these 
> footprints right?

Only if they match your connectors ;-)

BNC is probably not right for CONN2.  If you want a 2.1mm/5.5mm power
connector, you probably want something that looks like:

http://www.gedasymbols.org/user/vanessa_dannenberg/footprints/DCJ0202%20Power%20Jack.fp

BUT power jacks tend to be of various footprints; you may need to make
your own.  Print out a board and compare the printout with the
physical part and see if they line up.

> I don't know what footprints to add for the rest of the elements.

Depends on the elements.  For through-hole resistor, probably
something in ~resistor or ~generic, like AXIAL_LAY 600.  For surface
mount, use the standard sizes in ~geda like 0603.

You probably want to bring up a copy of PCB while you're running
gattrib, and use pcb's library window to "browse" the footprints.  Put
them on a temporary board, look at them, decide if that's what you
want.  If it is, the text in square brackets (like "... [0603]") is
the footprint attribute you want.

Also, watch out for pin numbering.  For example, confusing a DB-25
male footprint with a DB-25 female footprint will result in a PCB that
looks right, and accepts the part, but is wired wrong.  Trace a few
key signals by hand and verify they end up on the right pin.

> and get WARNINGs for resistors, capacitors, LEDs & optocaplers.

Right.  *Every* part *must* have a footprint (or have graphical=1 to
ignore it) to make a pcb out of it.

The opto is probably a DIP6.

> What is the right way to do this work: to make a PCB for this interface?
> Should I buy first the electronic elements and then add footprints to the 
> elements in schematic?

*I* like to at least download the PDFs for the parts and build the
footprints from those.  However, once I get the physical parts
in-hand, I print out the layout and place the parts on the printout to
verify that I got the footprints right.  I've gotten them wrong before.

Also, having a scrap PCB with holes of various sizes (near an edge is
best) to check what hole sizes you need helps.  Or a cheap dial
indicator for measuring lead diameters; add at least 2 mil for square
pins and 5 mil for round ones for solder clearance.

> How to make a connection to USB port: that is, for what to sold the USB 
> cable on this PC interface?

You probably want one of the USB-B footprints.

Regular: http://www.gedasymbols.org/user/levente_kovacs/footprints/USB_B.fp
Mini: http://www.gedasymbols.org/user/darrell_harmon/footprints/usbminib_hirose_th.fp


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user