Your post is more relevant to the PADS Layout and Routing community, so I've moved it here so that more people will see it.
Are you asking if you can have more than one pin with the same pin number (for example, the four ouside pins of an SMA connector)? if that's what you're asking, then the answer is no. PADS is set up to do one pin per connection. Your schematc symbol should show all connections.
You CAN use ECO mode to tie unconnected pins together, but the "extra" connections would be lost the next time you sync to a schematic or ECO-in a new net list.
Thanks for the answer.
Actually there is a way to do it if you think outside the box a little.
In your schematic, remove all the pins that are ganged together except one. In your decal, remove the same pins. Now add a copper shape to layer 1 that duplicates the pads of all the missing ganged pins and associate the copper to the remaining pin.
What happens is the schematic and the layout only "see" one pin but the copper SHAPE mimics the pin pads for the actual part, which makes the part itself happy, and there will be no errors.
Give this a shot and let me know if it works for you.
Good for SMD pins ... but how about TH pins ?
Put a small dot or X at the center of the TH pin in the decal and delete all the pins but one in the decal and in the schematic symbol. Form the copper the same way as the SM component duplicating the pin locations and associate it to the remaining pin. Create a via equal to the size of the TH for the part, then place the via on the copper using the dot or X as center points. Change the vias to stitching vias and I suspect they will act the same way as Epad stitching vias; i.e., no errors. Oh, yeah, be sure to add the correct shapes to your soldermask and (for SMT) paste masks and associate them to the pin as well.
Both of these methods should work, but to be honest I just thought them up now as a response to your question and I haven't tried them. They are compatible with what I know about Pads anyway. Personally I usually just ignore this type of error since I know what causes them. Let me know how it works for you.
There is another way, that I forgot about, because I never use it because it's too easy to introduce probems, unless you're VERY strict and conscientious about how parts are built and used, and how schematics are done (or at least have more than a little control over how schematics are done), including what signal names are used for what, at least for GND and PWR signal names, which is where theses multiple-pin s going to one signal usually are..
You can assign implicit pins to schematic symbols, they will be tied to a specific signal. I'm not 100% sure about how to do this, as I haven't done it in years. But you can look it up in Supportnet and/or Help. Also, I think some of the Parts in the supplied libraries may have implicit pins used. But, except for the most basic stuff (i.e., pins), I don't use the supplied libraries. so I'm not 100% sure on that.
Anyway, using an SMA as an example, you could then show just one of the common pins, with the other three as implicits.
You can use Signal Pins in Logic for the global nets like GND. But you still need a terminal in the PCB Decal for every pin on the schematic part including signal pins. If the schematic part has one pin that is visible and wired to a net on the schematic and also has three signal pins assigned to GND in the Part Type the PCB Decal needs to have four terminals. The netlist will not read into the board without errors if there is any pin number mismatch.
I know this, hence my statement "In your schematic, remove all the pins that are ganged together except one." then match the decal pin to the same number as the schematic one. The original question was how to eliminate all the decal errors when the decal has copper covering more than one pin. The solution is you trick Pads AND Logic into thinking there is only one pin even when the device labels a common copper area as multiple pins.
This idea will work assuming you have permissions either to modify the schematic yourself or ask the hardware engineer to do it for you. Personally I find it easier to simply verify the errors then ignore them but other people may have different thoughts or requirements.
One thing I haven't mentioned in my answers. I simply insist (when I have that option), or ask very nicely (when I don't), that ALL pins on a part be shown in a schematic, even the NC and PWR/GND pins.
It makes some parts, like spade lugs, SMAs, and some other parts with multiple pins all tied to the same signal look a bit clunky, but there is no confusion and it makes sure all pins get tied to whatever signal they need to tie to. And makes sure that those that are supposed to not have a connection don't accidentally get one.