I wouldn't personally be inclined to use the same schematic part for both "dual footprint" and "standard footprint" (PCB) components, but if you really wanted to do that, there are two ways by which you could conceivably accomplish it.
First method (which I would *not* recommend though): As you are using Altium Designer 2004, the schematic part could incorporate just three pins in the "Standard" Mode, and 5 pins in the "Alternate 1" Mode. Then select the former mode for TH or SMD components, and the latter mode for "dual footprint" components. (I have an idea that if you tried doing that though, then you would get errors, or at least warnings, whenever you compiled your schematic files, because of the different sets of pins for each of the modes concerned.) Second method: Provide additional pads within the "standard footprint" (PCB) components, so that pad 1A is totally encompassed within pad 1, etc. Doing that will result in Gerber files which will be larger than otherwise (but probably not by much), but which still shouldn't be problematic. As I alluded to before though, I still wouldn't personally want to resort to either of those methods, unless there was a truly compelling reason for using the same schematic part in all circumstances. Regards, Geoff Harland. > Hi, > > How do you then accommodate a component where you only have the one > set of pins? > i.e. on some boards I need to use the dual-footprint with its 5-pins but > most other times I need to use only a 3-pin footprint. I need to use the one > schematic item for either the single or double pcb footprint. > > Best Regards > > (Mr) Laurie Biddulph > > > > What I do in such circumstances is define pins 1, 1A, 2, 3, and 3A in the > > schematic component, and similar pads in the PCB component. And pins 1A > > and 3A (in the schematic component) should each have both their Name > > and Designator strings hidden, and be placed in the same locations as pins 1 > > and 3 (respectively). > > > > When you connect a wire to pins 1 and 1A (or to pins 3 and 3A) a junction > > will be depicted (as that wire is joining two different pins), and that > > acts as an alert that there is actually more than one pin residing at the > > location concerned. > > > > I have found that this method works very well, and to give credit where it > > is due, I first heard of it from Abd ulRaham Lomax. (a number of years > > ago, and on this mailing list). > > > > Regards, > > Geoff Harland. > > > > > >> Hi, > >> > >> I have created a simple footprint for a component that supports 2 > >> different physical packages ( a pcb-mount pot, 1 on 0.1" pitch the > >> other on 0.2" pitch). The centre leg of both devices are common > >> while the 2 pads on one side are common to each other as are the > >> 2 on the other end. So the footprint has 5 pads, 1 common and 2 > >> pairs. > >> > >> How do I create/define these pads such that Altium Designer DXP 2004 > >> automatically associates the appropriate netlist to each pair of pads? At > >> the moment, if the pads are designated 1, 1, 2, 3, 3, it only picks one 1 > >> and one 3 meaning I have to go to every component using this footprint > >> and assign nets to the empty pads. Which is fine until I do an update. > >> > >> The schematic for the component only has 3 pins (1, 2, 3) because there > >> are only 3 pins on the physical device. > >> > >> A similar situation occurs where it would be nice to have an extra pad > >> on, say, a radial footprint to allow for a 0.1" or a 0.2" capacitor to > >> be fitted. Again, 1 pair of pads needs to be common. > >> > >> Best Regards > >> > >> (Mr) Laurie Biddulph ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
