> 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 [email protected] http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
