<snip> GH> > > Or have I "grabbed the wrong end of the stick" in this instance, GH> > > and you actually want just two of the four corners to be GH> > > rounded instead? > > DS> > yes this is what i had wanted > > DS> > these sorts of shapes can be very handy at times, chokes, buttons, DS> > dual footprint compromises that customers always demand > > DS> > ideally i would like to be able to define a completely arbitrary pad DS> > shape, e.g. a polygon with differing radiused corners > > DS> > failing that then the current rounded rectangle but with 4 (or 2) DS> > settable corner radii > > DS> > failing both of those then also acceptable would be piling up a bunch DS> > of junk (tracks, fills, regions, other pads) BUT without the current DS> > nuisance of having to update free primitives all the time > GH> I thought that there had been improvements in updating the Net GH> properties of (non-pad) primitives in relatively recent times. (Or was GH> that an instance of an "overly optimistic" item within the release notes GH> provided for one of the SPs released for AD6?) > GH> And would defining an union of the primitives of interest be helpful at GH> all in such circumstances? (Originally each union consisted of a set of GH> components, but I gather that at some stage the concept was extended GH> to enable users to "group" *any* set of objects.) > DS> > these primitives when part of a component and when touching a pad and DS> > when on an electrical layer should simply become children of the pad, DS> > sort of like a nested sub component and any child pads should lose DS> > most of their electrical properties such as designator so that that DS> > ambiguity would also be solved DS> > solder mask and paste could be offered as a calculation of the DS> > boundary of the finished composite object (sort of a 'SUPER-PAD') or DS> > simply drawn or pasted from the conglomerate mess > GH> I am pretty sure that P-CAD provides the ability for users to define GH> shapes of their own choosing for each layer of a pad (including Paste GH> Mask andSolder Mask layers, and P-CAD's equivalent of Power Plane GH> layers), and has done so for a number of major versions; there is also a GH> "default" option available for the Solder Mask layers in which the GH> details on those layers are derived from the details on the appropriate GH> external copper layer in conjunction with a "Solder Mask Expansion" GH> setting. (I'm not sure whether a similar feature is also provided for GH> the Paste Mask layers, but perhaps there is.) > GH> I don't know whether that functionality will ever be provided within AD GH> as well, but if P-CAD users are not going to lose any of the GH> functionality which is currently provided to them, it would need to be GH> implemented at some stage (though perhaps in a following major version GH> of AD, rather than within AD6). <snip>
Something else which I have since recalled is that there have been various times when I have wanted to effectively implement pads with customised shapes, and while it would be untrue to say that I have never used non-pad objects to implement such shapes at such times, I have still always regarded it as desirable to use *just* pad objects at such times. The reason for that preference is that there is normally a lot less hassle in implementing the appropriate details on the Solder Mask and Paste Mask layers. (And if there is any reason for subsequently changing the value of the Solder Mask Expansion and/or Paste Mask Expansion property for the "pad" concerned, I usually don't have to edit any objects on any of those layers.) To avoid synchronisation-related issues, it is highly desirable to also provide additional corresponding pins within the associated schematic file(s), and in such cases I customarily "overlay" each additional pin required in exactly the same location as the "nominal" pin. Only the original "nominal" pin has its Designator and/or Name properties displayed, while *both* of those properties are concealed for any additional pins which are subsequently added to the relevant part. It has been claimed on at least one occasion in the past that a netlist-related issue involving different pads/pins having the same Name/Designator property has been rectified, but my experience has been that regardless of whether any changes have been made to the source code, that claim needs to be taken with a grain of salt. As such, I ensure that every pin within each (schematic) component continues to have an unique Designator property, and similarly, every pad within every (PCB) component continues to have an unique Name property. So as one example, if a pad with a customised shape is to be assigned a Name property of 2, a "second" (supplementary) pad would be designated as 2A, while a "third" pad, if required, would be designated as 2B, etc. And similarly for the pins for the corresponding part within the corresponding schematic file. I would be the first to agree that there is some additional work involved in doing all this, and that that approach wouldn't necessarily always be the best approach in some circumstances. That said, I think that that approach still has something going for it in at least some situations, though it would of course be even better to have the P-CAD feature provided in which customised shapes can be specified on each layer as required. Regards, Geoff Harland. ____________________________________________________________ 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]
