Thanks for your prompt response. The main reason for using one schematic part is that I have created schematics for every component I use i.e. 1 for a 10K Lin pot, 1 for a 10K log pot, one for every value resistor etc. Although a nuisance when creating a schematic (you have to select every value from the database rather than use, say, a `resistor' and then edit its values. the main reason been that I have a defined purchasing code for each component along with a manufacturers code so that when I create BOM's I get all my purchasing requirements available at the same time.
Thus, having created some 20 or 30 schematics for pots, I am not keen to have a another 20 or 30 for the dual-pot version although I am beginning to think this may be the best way. I am surprised that AD doesn't recognise `more than 1 pin with the same designator' and connect them altogether on the same net..... seems a logical thing to do .... but then this IS Altium!!!! Best Regards (Mr) Laurie Biddulph Phone: +61 (0)2 4340 0938 Mobile: 0400 257 645 Elby Designs ABN: 70 022 727 605 http://www.elby-designs.com This e-mail and any files transmitted with it are confidential and intended for the addressee only. If you are not the addressee you may not copy, forward, disclose or otherwise use it, or any part of it, in any form whatsoever. If you have received this e-mail in error please notify the sender and ensure that all copies of this e-mail and any files transmitted with it are deleted. Any views or opinions represented in this e-mail are solely those of the author and do not necessarily represent those of Elby Designs. Although this e-mail and its attachments have been scanned for the presence of computer viruses, Elby Designs will not be liable for any losses as a result of any viruses being passed on. ----- Original Message ----- From: "Geoff Harland" <[EMAIL PROTECTED]> To: "Protel EDA Discussion List" <[email protected]> Sent: Tuesday, December 19, 2006 12:27 PM Subject: Re: [PEDA] Common component pads >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] > ____________________________________________________________ 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]
