9 Replies Latest reply on Mar 14, 2011 7:16 PM by Nightwish

    Reuse Block Symbol

    Nightwish

      Hi All,

       

      I am trying to crreate a Logical-Physical reuse block in the Library. After I created this RB and verified it, I opened my Dxdesigner to place the reuse block in my design. But the Place Symbol window only shows a symbol border without pins. See picture below:

       

      RB.JPG

       

      I have defined the IN and/or OUT pins in the root design, but they don't show up in the generated Reuse Block Symbol. If I edit the Reuse Block Symbol from within Library Manager, when I package the design and there are some errors. Can any give me some advice on this? Also when place the Reuse Block Symbol into Dxdesigner, it will merge some nets like GND or VCC as Global nets. Is there a way to set the Global nets manually? Many thanks!

       

      Regards,

       

      Nightwish

        • 1. Re: Reuse Block Symbol
          robert_davies

          In order to understand the problems can you provide some more details about how you have generated the block symbol, from where and the steps and settings you used. How is the symbol editor configured for pin length, pin spacing etc.

          On the globals issue, how have you defined the global signals in the source (re-use block design), what are globals are used in the host design etc.

          Also look at the process guides for Logical Physical reuse in the on-line help.

          1 of 1 people found this helpful
          • 2. Re: Reuse Block Symbol
            Nightwish

            I first created a root design in Dxdesigner and then I packaged the schematic and forward annotate to Expedition. After that I  open Reusable Block Editor in Library Manager and new a L-P Reuse Block follow the wizard. And then I verified the newly created RB and place it on a design in DxD. But the symbol just has no pins defined. I checked my root design and I have defined the IN and OUT port. Also the design and the RB are all link to the same Library.

            • 3. Re: Reuse Block Symbol
              robert_davies

              Do you add hierarchical ports to the signals of the Reuse block design such that all of the connections traverse up to a 'non-existant' external parent block. The symbol generation relies on the signals being hierarchical rather than flat and uses the port symbols to generate the pins. For example, if the block was a parent you would not expect 'port' symbols for the I/O, more likely physical connectors, but this would generate a block symbol with no pins. If you have defined the I/O of the RB with physical pins replace these with hierarchical ports.

              If you still have no success give customer support a call so they can work through the problem with you.

              Rob

              1 of 1 people found this helpful
              • 4. Re: Reuse Block Symbol
                Nightwish

                Hi Rob,

                 

                Thank you very much for your help. You are right and I need to use the hierarchical ports in my schematic. I have called the local Mentor AE and there is also something wrong with my ports in library. Now I have successfully created the reuse block.

                 

                 

                RB.JPG

                 

                Have a nice day!

                 

                Nightwish

                • 5. Re: Reuse Block Symbol
                  snguyen

                  Hi Rob,

                  Can you explain the difference between ports and hierarchical ports?

                  In DxD, there are 2 kinds of symbol for each direction such portin.1 and portin_hier.1, any significant different?

                  I've been using the regular ports for all of my hierarchical blocks.

                   

                  Thanks

                  • 6. Re: Reuse Block Symbol
                    robert_davies

                    There is no difference between ports and hierarchical ports, or at least we should state that 'port' means a connection that passes through hierarchy via a block symbol. We should however distinguish between three kinds of 'connector' used in DxDesigner, physical connectors, those that are a component in the PCB and are represented by 'module' type symbols in the editor. These may be single pin symbols or multi-pin symbols and have a corresponding cell (decal) in PCB layout just as any other physical component. Then we have two virtual connectors that represent information for the designer, ports (or hierarchical ports) that represent connections traversing the hierarchy through block symbols, these are represented by 'Pin' type symbols in DxDesigner, they do not have physical cell on the PCB but they drive the connectivity through the hierarchy and are checked in DRC for elecrical correctness. The second virtual pin type is used for documentation and cross-referencing, these are represented by 'annotate' type symbols and do not influence connectivity but are used for annotation and 'linking' between schematic sheets. You will find these listed under the 'Links' node in the latest versions of DxDesigner. Again they do not have a physical cell in layout.

                    Now for each virtual pin type you may have more than one symbols to represent different drawing styles or requirements, in your case you have a portin.1 and a portin_hier.1, provided these are both 'Pin' type symbols (check in the symbol editor) then they are just alternative representations of the same type of connection. If on the other hand one of them is an 'annotate' type symbol then it would be used for documentation purposes only and should only appear in the 'links' menu in DxDesigner. It is possible that when designs are migrated from earlier versions of DxDesigner such as 2005.x, 2004.x then the wrong types of symbols appear under the port connections or links menus as they were not consistently handled in the earlier versions of the software.

                    • 7. Re: Reuse Block Symbol
                      snguyen

                      First of all, thanks a lot for you response, Rob.

                      Secondly, the type of symbol that you mentioned as "annotate" seems to me is the on/off-page symbols (>>-- or --<<), am I right?

                      • 8. Re: Reuse Block Symbol
                        robert_davies

                        You are correct in your assumption, annotate = on/off sheet. Now referred to as links.

                        Rob

                        • 9. Re: Reuse Block Symbol
                          Nightwish

                          Here I have another question about the Reuse Block properties. When creating the RB I type in the Reuse block description but when I place the symbol onto schematic, the description doesn't show up. Please see picture below for the detail, Is there a way to show the description in the Dxd? I don't find a setting about this. I can add the info when editing the symbol within library manager but I hope there can be other ways. Can someone help me about this?

                           

                          RB Properties.JPG

                          Thanks,

                           

                          Nightwish