5 Replies Latest reply on Jul 10, 2015 1:20 AM by robert_davies

    Change implicit power supply definitions on schematic level


      I downloaded the ODA starter library to begin playing around with xDX Designer in PADS VX.0 and noticed that most ICs consisting of multiple gates define the power supply and ground pins implicitly (e.g., a dual op-amp package like the LM393AN has the supply voltages defined as "V+" on pin 8 and "V-" on pin 4, or on a 74xx quad logic gate, Vcc and GND on their respective pins.) See below, for example:


      The bottom two properties designate pin 4 and 8 as the negative and positive supply voltages, respectively. However, if I change the property value to match the name of my net for one of the nets (e.g., if I change "V-;4" to "-10V,4") then the property field for the other signal pin disappears. I am then unable to add another "Signal" property field as that is not one of the options that pops up when adding a new field. See below:

      This leads me to believe that this is either a bug with the part library and/or DXDesigner, or that this is not the proper way to change the signal pin definition (and I am leaning towards the latter.) It may be that it is simply not best-practice in circuit design to have circuits that have different supply voltages for op-amps or other ICs, however this is the case for several of our legacy designs where we have some op-amps getting +/-15V and others getting +/-10V for example, and the particular design and components necessitate it.


      Without editing the library part, is there a way to manually select the net that the signal pins connect to for individual symbols in a schematic/block? (See above for example, where one instance of an op-amp must have V+ and V- mapped to +/- 10V respectively, and the other to +/- 15V)

        • 1. Re: Change implicit power supply definitions on schematic level

          It's a bug, in the property definition file Signal is set as a single entry you need to change this to multiple. Open the Central Library from the toolbar and in there open the Property Definition Editor. Find Signal and expand the dialog by pressing the Advanced button and modify the Instances Allowed from Single to Multiple.

          Close the Library tools and run Tools - Update Libraries to refresh the property list. You should then be able to modify both strings without them disappearing.


          If the Tools - Update Libraries doesn't work just close and re-open xDX Designer.

          • 2. Re: Change implicit power supply definitions on schematic level

            To add to your general comments, you can create parts with the power pins defined explicitly on the symbol and you connect up to them with the required nets. These can be created in a number of ways, one is known as a Hetero Type 2 where one symbol shows the power pins and another doesn't. Or you could simply show the power on all symbols and connect them to the correct supply. To group them together use the PKG_GRP property with the same value (any alphanumeric).

            An example of the hetero 2 is shown in the picture (also look it up in the on-line help and/or SupportNet).

            • 3. Re: Change implicit power supply definitions on schematic level

              If you use simulation, the easiest method to apply a model is to show the power pins on all fractures and connect them to the correct supply.

              • 4. Re: Change implicit power supply definitions on schematic level

                Thanks for all the helpful responses. Changing the Instances Allowed to multiple let me view and modify all of the signal values within the schematic, and I was able to use Hetero Type 2 symbols to show those pins. The other workaround I found is to use the Supply Rename property to manually reassign supply pins to the proper nets (e.g., Supply Rename = V+=+10V V-=-10V where I've already made nets named +10V and -10V)

                • 5. Re: Change implicit power supply definitions on schematic level

                  It seems you have a hybrid setup based on the ODA parts. If you are using the Integrated flow with a Central Library then the Supply Rename is used to override power/ground pins defined implicitly in the mapping and the Signal property shouldn't be on the pins at all. These are used for a netlist project using the PCB Interface to annotate back and forth.

                  If using Hetero type 2 then the picture I showed you is for the netlist flow, the same set-up can be created in the Central Library without the need for many of the properties.

                  It is good to know however that either method works in your case (renaming the Signal property and Supply Rename), but personally I would figure out which mechanism I'd prefer and create my components accordingly.