5 Replies Latest reply on May 10, 2012 9:00 AM by eng.same.tan

    How to export/import parts placement?


      I would like to export some parts placement from Project A to Project B with reference point at x=0, y=0.

      Can I do this and how?


      Can I just export for those I selected parts before I export from Project A?

      So I can import for those I needed only parts to be placed in Project B.

      I need some advice and guide, thanks in advance.

        • 1. Re: How to export/import parts placement?



          I would recommend to use "Circuit Move and Copy" within Expedition PCB.

          Other option ist to use keyin command "pr -file=<dir>/<filename> {-x}" , write all part to a file and delet not needed ones in the file.

          Then import file with keyin command again.




          • 2. Re: How to export/import parts placement?

            I would use IDF import export functionality.

            File - Export - IDF to output an *.emn and *.emp file.

            File - Import - IDF tot import the created *.emn file.


            EMN files wil also contain the board outline, keep-out areas and more. The file is easy to read, and you can remove those lines from the file before importing it in layout.

            If you want to exclude parts form the emn file. You can remove the components first from the original layout and don't save the layout. Or you can edit the emn file and remove the lines with those parts from the emn file.

            • 3. Re: How about TRACE / VIA ?

              @ m.maenhout,

              Noted, I will try this.



              @ Andreas.Schaefer,

              Thanks for the tips, I tried and it is really work.

              But filtering (deleted) for those unused / unwanted parts are a bit wasting times.



              How about export/import traces/via?

              Is only CIRCUIT MOVE & COPY function to use?

              Can I just copy trace and via into other design by ignore all the netname?

              Need some guide on this.


              • 4. Re: How about TRACE / VIA ?


                When you intend to copy vias and traces, you need to have a netlist in the background.

                Otherwise you would get everything on (net0) and then reassign it to correct net manually. A silly idea.


                So when needing a netlist, you will also have a schematic with connectivity, creating this netlist.

                When you copy traces, it would only make sense when you assign some nets to them too.


                CM&C can do this within the wizard appearing at the paste process.


                So just select teh traces with CM&C in source design an paste it in target design.


                When connectivity of source and target do not differ much, it will work.


                If you are using complete different connectivity in source and target (for what reason ever)

                I would try the following:

                • in source fix all desired traces and vias
                • in source schematic delete the circuit
                • Forward annotate into expedition with option not to delete hangers.
                  So after FA all fixed traces shoud be still there and connected to (net0)
                • Then use CM&C and you will be able to copy teh (net0) traces



                kind regards,


                • 5. Re: How about TRACE / VIA ?

                  Thanks for your detail guide, I got your point there.

                  By the way, I don't know why mentor need to by same netname only can copy over.

                  It should be sllow us to copy what ever we selected (trace, via, shape, line, polygon, text...etc) and just copy & paste to other design directly,


                  For trace & via, after copied, then we only decide want to set the netname or just leave it there (maybe as a reference or whatever) and allow us to set a reference point when copy or export to a file.

                  then can use the same reference point when we want to import.