4 Replies Latest reply on Aug 18, 2011 6:32 AM by cleon

    Help sending mass ref. designator change to Layout...

    cleon

      I used a script to change almost all of the reference designators in Logic (after the board had already been laid out) and everytime I try to "ECO to PCB" and "NETLIST TO PCB", the parts lose their association and revert to the origin of layout (I understand that this is not a bug). Is there a way to make is so the ref. designators are just changed while preserving the layout side of the board? For example, if I change R1 to R1A, is there any way to have the Layout update to R1A while preserving the position on the board (keeping its association)?

        • 1. Re: Help sending mass ref. designator change to Layout...
          Vern_Wnek

          In my 30+ years in this industry, I have heard this question many times from Engineers...

           

          With every PCB Design system I have used (and there are many), If you change the Ref Des on the schematic, expect that the Part on the PCB will be ripped up. Although it seems simple, it is not. The schematic drives the board, so if a Ref Des changes, the board sees it as No Longer There - and removes it.

           

          Some suggestions I have made in the past to engineers to help this issue...

           

          1. Never change Ref Des on Schematics on a board respin

          2. Never reuse a Ref Des on a board. IE) If you replace P1 with a different type of part, keep it P1. But, if you remove P1 from the design and add a New Part somewhere else - do not call it P1.

          3. If you Ref Des by Schematic Sheet, and you need to add or remove sheets - Do not change the Ref Des if the circuit are to stay on the board. Add Blank Sheets to your schematic - New Sheets are Cheap compared to the time to replace a circuit that was being reused.

          4. If you need to change Ref Des on your schematic, do it from the PCB side and Back Annotate to keep everything intact and in sync.

           

          There are some exceptions to these rules - Like Formal Reuse Circuits, but unless you are using them, this is the way EDA tools work.

           

          Good Luck,

          Vern Wnek

          • 2. Re: Help sending mass ref. designator change to Layout...
            David Ricketts

            Of course there is, but you need to control the process. You can't use the Layout Link. The procedure below is tailored specifically for your stated situation. It's long because I'm trying to be thorough, but it's not as hard as it might seem, especially if it works the first time.

             

            1. From the Logic Tools menu, use Layout Netlist to create a netlist.
            2. Only the "Include Subsheets" checkbox need to be checked, and that's only if you're using them.
            3. Start Layout with your PCB loaded.
            4. From the Layout Tools menu, select Compare/ECO. You will start on the "Documents" tab.
            5. For the "Original Design to Compare and Update" box, check "Use Current PCB Design".
            6. For the "New Design with Changes" box, use browse and select the netlist (<schematic filename>.asc) you just created.
            7. For the "Output Options" box, check "Generate ECO File" .
            8. Go to the Comparison tab.
            9. For the "Comparison Options" checkboxes, what you select this depends on your design standards. For this case, you probably should just check "Compare only ECO Registered parts".
            10. Here's the payoff. For "Name Comparison options", select "Compare Connectivity and Topology (not names). Rename as necessary". This option is designed just for your situation.
            11. Leave the "Attribute and Design Rule Comparison Level" boxes unchecked.
            12. Go to the Update tab.
            13. For Update Options, check both "Update Original Design" and "Pause before Updating" boxes. You ALWAYS want to review the ECO file before continuing.
            14. You can leave the Library options unchecked.
            15. Click on Run.
            16. You will get a Process Status dialog box. Click on" Show Report".
            17. If the SCH and PCB databases were in perfect sync before the schematic was renamed, you should only be seeing Rename (*RENPART*) commands.
            18. If that's the case, press Continue. Your PCB should now match the schematic, and no parts will get moved.
            19. If that's not the case, examine the ECO commands to figure out what the differences are. If there are *DELPIN*, *PART*, *CHGPART*, *DELPART* or any NET commands, then you might have more parts on one database than the other, or the nets are different too. If that is the case, then you need to might need to manually make the these changes for rename process to work.
            20. Another option is to delete all of the ECO commands that aren't *RENPART* and save the ECO file. Now, when you press Continue, you'll get a partial update.
            21. With a partial update, rerun Comparison. Since the databases are now closer in sync, you should get more accurate ECO changes.

             

            Hope this helps.

            • 3. Re: Help sending mass ref. designator change to Layout...
              Vern_Wnek

              David,

               

              Very Nice. I completely forgot about the ECO *RENPART* in Pads, that's my bad.

               

              You are correct though, you need to use the ECO Compare capability, and not the Normal Layout load.

               

              Thanks for the Outline, I'll have to keep this around

               

              Thanks,

              Vern Wnek

              • 4. Re: Help sending mass ref. designator change to Layout...
                cleon

                Thank you very much.

                 

                In your step 13, my "Update Original Design" and "Pause before Updating" boxes are grayed out. Does this mean I do not have the proper license or am I just doing something by mistake?

                 

                edit: Nevermind, it was my mistake. I neglected to follow step 5. Thanks again!!!

                 

                edit 2: I actually ended up need to do "Compare names and reference designators. Rename as necessary". I think some of my nets had also changed when I changed my schematic, requiring more than just the third option you had told me. It did work, however. I can't thank you enough. Even though I may have been able to re-layout the entire board in the time it took me to find an answer, it's worth it in the long run