6 Replies Latest reply on Jan 31, 2012 5:25 AM by zeke41

    Layout and Schematic Library Management


      In order to avoid duplicate footprints in layout, I would like to use one library for footprints. Schematic parts would need to refer to footprints in that library.

      However, it looks like unless there is a schematic part in that library, it is not shown in the list of libraries when I try to select the PCB decal in the component editor.

      Is that correct?


      This is the way I have always used PCad and Orcad, which is what I am moving from. If there is another way to manage the footprints so that there are no duplicates, please let me know. I like to keep a library of all of my SMT footprints, and a separate one for THT (no reason to separate other than to keep the sizes smaller).




        • 1. Re: Layout and Schematic Library Management

          I created a new library and imported 4 PCB Decals into it.  I added that library into my Lib List in Logic and opened a random Part Type in a different library.  When I set the Pin Count to a value that matched a PCB Decal in my new library I was able to see the PCB Decal in the preview window.


          If this is not working for you please submit a Service Request and attach the library for review.

          • 2. Re: Layout and Schematic Library Management


            if you are still looking for an answer to your question I suggest you restate it


            your problem may be as simple as selecting (All Libraries) in the Library drop down list rather than a specific library


            but it is not exactly clear to me what you are asking or trying to accomplish

            • 3. Re: Layout and Schematic Library Management

              Thanks but -


              What I am trying to do is to use one library to hold almost all of my layout footprints (decals). That library doesn't have any part types or schematic symbols in it - only footprints.


              But this seems to be  a problem. In Layout, it looks like it will not use any library that does not have a part definition in it. My library that is full of layout footprints doesn't even show up in the Libraries... list.


              I am trying to avoid having duplicate footprints. For example, a SOT23 footprint would exist in several different libraries (resistors, ICs, diodes, transistors, etc). Having the same footprint in every library where a part definition exist would force me to remember where they all are and to update them all if I happen to make a change. It is much better to have a single footprint.


              What am I missing here? Can this be done, or not? Is there some other way to manage the libraries to accomplish this?




              • 4. Re: Layout and Schematic Library Management

                Hi Dan


                I have been using the same library setup as you for many years without any problems.

                I have footprints in one library (called SMD) and the parttypes are located in multiple different libraries such as Res, Cap, Dio and similar.


                I think it may be a problem with your library lists.

                Are the available libraries the same in both Logic and Layout?




                • 5. Re: Layout and Schematic Library Management

                  Putting the PCB Decals in a separate library should work fine if everything is set up correctly.


                  1. Be sure all four of the library files for this library are in the same folder.  You need all four files even if three of them are empty.

                  2. Add this library to the Lib List in both Layout and Logic.


                  The library should appear in the Lib List and the PCB Decals should be visible in the PCB Decal preview window in the Part Type.

                  • 6. Re: Layout and Schematic Library Management

                    Hi Dan,


                    Each component in PADS uses 3 Items : Part, Symbol and Decal. And each library can contains this 3 Items.


                    When you add a component you use its Part.

                    The Part calls the first Symbol that the name is matched in the first library. In the same way when you add a component in PCB

                    the Part calls the first Decal that the name is matched in the first library.


                    Suppose that you have that libraries in your system:


                    (In MyPart you have only Parts, MySym2/MySym1 only Symbols and MyDecal2/MyDecal1 only Decals)


                    MyPart:      Parts
                    MySym2:   Symbols
                    MySym1:   Symbols
                    MyDecal2: Decals
                    MyDecal1: Decals


                    Suppose now that you have the 7400 part in the MyPart Part library.
                    This 7400 Part uses the NAND2 symbol and uses the DIP14 Decal.


                    However you can have the NAND2 symbol in MySym1 and MySym2 and DIP14 in MyDecal2 and in MyDecal1 like that:


                    MyPart:    7400
                    MySym2 : NAND2
                    MySym1 : NAND2
                    MyDecal2: DIP14
                    MyDecal1: DIP14


                    When you add the 7400 part in a schema PADS calls the NAND2 symbol found in MySym2 because this library is set before MySym1 in the library List.
                    PADS do not purpose you the second NAND2 symbol.

                    In the same case for Decal.


                    Zeke Cmos