6 Replies Latest reply on Jun 12, 2018 10:21 AM by lamabrew

    How to use Pad Class?


      I haven't turned up an explanation for this by searching (even in Designer). Apologies if I missed the obvious answer.


      I want to assign a pad class to certain pins of a component so that the PCB tools knows how to connect it to a polygon. In this specific case the connector has multiple ground (shell) pins and I want them directly tied to the GND plane and not with thermal reliefs.


      So far all I have been able to do is manually add the connector pins in PCB Class dialog. What I want to do is attach a Pad Class property to the PCB footprint in the library, or in the pin property for the part (I'm using integrated library and there is a 1:1 symbol to footprint correspondence).


      I thought maybe after setting the pad class in PCB I could back annotate to the schematic and see what it was doing, but CS doesn't see adding a pad class as something that affects the schematic as it tells me there's nothing to do. I tried adding parameter to the pin for the component and updating in the forward direction but again CS says there's nothing to update.


      There doesn't seem to be anything like the Directives->Net Class from the schematic side for setting Pad Class?

        • Re: How to use Pad Class?

          Interesting questions, I'm not sure so will look into finding if there is a solution.

          • Re: How to use Pad Class?

            In my situation, Atium did not connect some ground pads using the thermal relief as I would expect. Direct connect connects them as I want, but I want to keep the relief connect for the rest of the polygon. Here shown are the pads with the relief connect rule:


            I solved this by creating a specific pad class in the Object Class explorer: Design -> Classes -> Right click on Pad Classes -> Add Class


            And manually moved the pads that need the direct connect rule into this class:


            Then I created a new polygon rule with higher priority (leaving the orignal rule that applies relief connect to the whole polygon).


            The new rule uses "InPadClass" on "Where The Second Object Matches"

            The result is that the specified ground pads have been connected using direct connect, but it hasn't affected the relief connect on the rest of the PCB:


            FYI I am using Altium Designer 15.1.

              • Re: How to use Pad Class?

                Hi Catherine, it is possible to use Pad Class rules in CircuitStudio and select specific pads just like with Designer. Unfortunately I still don't think there is a way to have library parts that have pads pre-assigned to a pad class so when loaded into a design they will automatically have the correct rules assigned.

                  • Re: How to use Pad Class?

                    Since this one has bubbled back up and I've been using CS for longer now...


                    I'm kind of surprised that there's no concept of a "pad library," i.e. a pcblib like thing where I can define standard pad info (and associated Pad Class) and then place those in a component PCBLib instead of copy/pasting pads.  Maybe the use case for this doesn't come up that often, but I just spent time tweaking a bunch of parts that all have the same pad; got the Rev 1 boards back and wasn't happy with some solder issues.