2 Replies Latest reply on Apr 17, 2012 11:29 PM by kbak

    Multiple footprint decals for same library part? How to use?

    dmeeks

      The library editor allows selecting more than one decal for a part. But I can't seem to change the decal in either the schematic or the layout, once the part is placed.

      The extra decal shows up under the part's properties, and I can select it (in schematic only), but then that change doesn't seem to ECO over to the layout.

      How are these alternate decals supposed to work?

       

      Thank you

      Dan

        • 1. Re: Multiple footprint decals for same library part? How to use?
          RLS2004

          Depends somewhat on the schematic capture software are you using.

          DxD can output a netlist in this format:

          C1 CAPC@CC1206

          C1 is the refdes, CAPC  is the part type and CC1206 is one of several optional footprints (Decal).

          As you've already noted, you can select them in Layout as well.

          My personal preference is to have a 1:1 relation between Part Type and the footprint (Decal).

          RLS

          • 2. Re: Multiple footprint decals for same library part? How to use?
            kbak

            There are two ways of using the alternate decals.

             

            1) Controlled directly in Layout (my preferred way)

            • Select the part in layout.
            • RMB and select properties
            • In the middle of the "Component Properties" dialog there's a "Decal:" drop-down box.
              See attached picture "Alternate_Decal_In_Layout.png".
            • In there you can select one of the assigned PCB-Decals.
            • Click "OK"

            • Be aware - that DRC Prevent setting can prevent you from changing the decal.
              In such case temporarily turn DRC off.

             

             

            2) Controlled from PADS Logic

            • Select the part
            • RMB and select Properties
            • Click the PCB Decals icon
            • Select one of the PCB Decals in the "Alternates in Library" window.
            • Click "Assign"
            • Click "OK"
            • Click "Close"
            • Send ECO to PCB*

             

                 *Important - you must have the "Compare PCB Decal Assignments" enabled in the "PADS Layout Link".
                 Otherwise the Decal information is not sent to PADS Layout.

                 See attached picture "Compare_PCB_Decal.png"

             

                 But be aware that enabling this can have unexpected results if you manually modify just some of the similar named PCB Decals directly in layout.
                 You can risk that these modification will be cleared by an "ECO to PCB".
                 That's why I prefer the first method.

             

            ******************************

             

            Please note:

            The first time you send information from Logic to Layout (sending the netlist), the PCB-Decal information is always sent.

             

            regards

            Klaus