7 Replies Latest reply on Jan 24, 2013 5:13 AM by robert_davies

    Is it possible to do a Hierarchical Schematic using DxDesigner?

    v.anisoveca

      Is it possible to do a Hierarchical Schematic using DxDesigner?

      I have already done simple schematic. But now my boss asked me to make a block diagram on the first page of schematic project. It is first time I hear about this feature. How can I do this step by step? Is there any tutorial on this theme??

       

      Thank you in advance!

        • 1. Re: Is it possible to do a Hierarchical Schematic using DxDesigner?
          michal_ferdek

          Hello,

           

          Please take a look at the video attached to this tutorial available at http://supportnet.mentor.com/reference/tutorials/index.cfm?id=MG576731.

           

          I hope it helps.

          Thank you,

          Michal

          • 2. Re: Is it possible to do a Hierarchical Schematic using DxDesigner?
            Jackie_D

            Hi,

             

            If you go to the SupportNet page for DxDesigner, you will find tutorials for both Expedition and Pads flows.

            If you do not yet have a SupportNet login, please go to to http://www.mentor.com then select the Support section, and request a SupportNet login by filling in the details requested.

            You could also contact your local office to enquire about training classes.

             

            Regards,

            Jackie

            • 3. Re: Is it possible to do a Hierarchical Schematic using DxDesigner?
              veronika.anisoveca

              I had a look on the tutorial. But as I understood these blocks are created instead of the part of my schematic and the content of this block appears on another sheet.. But is it possible to leave the existing schematic as it is and to create the blocks on the new sheet? I would not like to make any changes in existing schematic design..

              • 4. Re: Is it possible to do a Hierarchical Schematic using DxDesigner?
                robert_davies

                Hierarchical blocks can be created on any sheet and at any level in the hierarchy, so a hierarchical block can exist inside another hierarchical block, it is just a way of partitioning your design into functional areas. You can even create a hierarchical block from an existing piece or circuitry. To do this select the Add Block Command and tick the Extract SChematic option.  But be careful using this command, you need to ensure that you intersect nets at an appropriate point in the design so that each net becomes a pin on the newly created block and the action is not easily undone.

                • 5. Re: Is it possible to do a Hierarchical Schematic using DxDesigner?
                  v.anisoveca

                  The thing I do not like is that instead of the detailed schematic the empty block appears. I would like for schematic to look like it was before the "Add Block".

                  In your video the detailed schematic moves to another sheet, but I would like for empty block to move to another sheet while the detailed schematic remains on its' place.

                  Am I clear?

                  • 6. Re: Is it possible to do a Hierarchical Schematic using DxDesigner?
                    v.anisoveca

                    So I just want to add a separate sheet where the Block Diagram will be represented, while the circuit diagram remains as it is.

                    • 7. Re: Is it possible to do a Hierarchical Schematic using DxDesigner?
                      robert_davies

                      I don't fully understand what you are trying to achieve or whether you fully understand the concept of hierarchy. But maybe what you are trying to do is generate a block symbol for the existing schematic and then use that elsewhere in your design. If that is the case then you need to ensure that all nets that are external to this schematic, that is go up the hierarchy to the sheet above, where this block will finally appear, have hierarchical port connectors attached. Once all external nets have such connections use the Tools - Generate Block Symbol command to generate the hierarchical block representation of the sheet. Once this is done you will see the block appear in the navigator under the blocks node. Now create a new schematic and add this block from the DxDataBook - CL View - Symbol View - Local Symbols node. When the block symbol is placed on this new schematic you will be able to select it and use the 'Push' command to open the child schematic (your original schematic). Finally, in the navigator set the new schematic you created as the root of the design so that it is the top block. To do this select the block in the navigator blocks section (by default it will be the Schematic2 block) and use the Set as Root from the context menu on the right mouse button. You should see that the Board view now has Schematic2 as the root and the original block (schematic1 unless you renamed it) as a child node. You can make the plain block symbol more informative by adding additional graphical elements to it if you so desire, but I would wait until the design is complete before doing so.

                      If this doesn't help then  perhaps you might consider some training where these concepts are taught.