1 2 First Previous 16 Replies Latest reply on Sep 2, 2016 3:12 AM by robert_davies

    Alternate symbols in DxDesigner


      How does DxD handle alternate symbols, such as a vertical capacitor symbol and a horizontal capacitor symbol for the same capacitor part number? 

      In PADS Logic I set up 'CAE Decal 1' and 'CAE Decal 2' under the Gates tab in the Part Editor.  Then I can hit <ctrl><tab> or <right-click><alternate> to cycle through the decal choices.  Does DxD have something like that? 



      John D

        • 1. Re: Alternate symbols in DxDesigner

          To ask this another way... Can I have multiple Symbols for one Device, such as Logic has for one Part-Type? 

          • 2. Re: Alternate symbols in DxDesigner

            This is not a complete answer as I am just getting into this myself too.

            But looking at supplied libraries there are 4 capacitor symbols withing the one symbol for diff rotations.

            they are cap.1, cap.2 cap.3 & cap.4 in the symbol preview they come up just like excel as tabs on bottom to pick which one you want to use.

            When editing the symbol these tabs are on top.

            Just not sure yet on details of copying etc to create the other symbols. Because when you look at the symbol in xDM Lib Tool

            you only see "cap", yet each of these you see within the symbol cap, cap.1 cap.2 etc can be opened and saved separately so not

            really there yet as to what is going on, need to do a little more reading and playing.

            So yes there is the capability like Logic just how the details work, not there yet.

            1 of 1 people found this helpful
            • 3. Re: Alternate symbols in DxDesigner

              Thanks.  I just stumbled across the .1, .2 suffix too.  The open question is where is the 'Part Type' info defined in DxD? 

              • 4. Re: Alternate symbols in DxDesigner

                I am still having no luck finding any more info on this.

                If you go to a schematic and dxdatabook to place a part, you get the choice of the 4 symbols, .1 thru .4

                however if you go and edit a part that uses hat symbol, in the CAE Decal section ONLY cap shows up.

                So how this all ties together is still not very clear to me & struggling to find more related info.

                • 5. Re: Alternate symbols in DxDesigner

                  A quick look in the corporate.mdb database provided with the evaluation shows the symbol listed without the suffix.  Maybe DxD is smart enough to offer all suffixes.  So it appears the Part-Types are defined in the database. 

                  • 6. Re: Alternate symbols in DxDesigner

                    A handy tip from the starter design library from Optimum Design Associates ("Mentor_PADS95_PADS_Net_List_Library_Guidelines_Rev1a.pdf"):



                    REQUIRED: The value of this field determines the symbol that will be used when the device is selected from DxDatabook for placement on the schematic. The exclusion of a file extension (.1, .2, etc.) in the symbol name allows the use of any of the multiple symbols with the same name. For example, cap.1, cap.2, cap.3, or cap.4 can all be selected from DxDatabook for any device that has ‘cap’ as the symbol name. This allows for different rotations and views of the symbol to be selected for placement.  And asterix character at the end of the symbol name allows for all symbols in a Hetero set to become available for placement on the schematic i.e. xc7vx415t-ff1927* "


                    Mentor's "DxDataBook Setup (Beginners)" is a good reference too:  https://supportnet.mentor.com/portal?do=reference.tutorial&id=MG576734


                    I'm still trying to figure out where DxDatabook finds its symbols...

                    • 7. Re: Alternate symbols in DxDesigner

                      I found where symbols are pulled from.  You use <Setup><Settings...>(Symbol Libraries) and define a path to a folder ABOVE the folder with the symbols for a Table in the database ('.\my_library\Diodes' for example).  You then need a folder in that folder called SYM ('.\my_library\Diodes\SYM') and then the symbols need to be located in that folder ('.\my_library\Diodes\SYM\1n4001.1', etc.). 


                      A couple handy commands from the DxDatabook window are:


                      <right-click><Configure>(Rescan Symbol Libraries) and

                      <right-click><Configure><Edit Configuration>(Update All)

                      • 8. Re: Alternate symbols in DxDesigner

                        Interesting in some reading too I found similar info that led me to settings, but I think the only way you see "Symbol Libraries" if you are using netlist flow,

                        if you are using Integrated flow that won't be there? Which is how we are running. However I did see those commands Rescan & Configuration.

                        Did not try that till I did a little more reading. But I did get a little further if you rt click in search pain of DxDatabook, you do see menu to get to edit configuration where all the parameters are controlled.

                        • 9. Re: Alternate symbols in DxDesigner

                          I believe that is correct.  "Symbol Libraries' are for the Netlist flow (PADS Standard).  The Central Library is for the Expedition flow (PADS StandardPlus/Pro).  The 'Use symbol data from Central Library' checkbox in the DxDatabook configuration window is grayed out if you only have a Netlist flow license.

                          • 10. Re: Alternate symbols in DxDesigner

                            I don't think so exactly, whether you have std, std plus or Pro, there are two flows you can use Integrated which uses the central library scheme

                            and netlist flow which I think you get all the same functionality & can use a central library (maybe not DxDatabook?), just an extra step in getting data to layout. At least I believe that is the way it was explained to me. Could be wrong on netlist flow?

                            • 11. Re: Alternate symbols in DxDesigner

                              Support explained to me that my Central LIbrary is grayed out because I only have a Standard (ES) License.  Or maybe because I'm still running V9.5? 

                              • 12. Re: Alternate symbols in DxDesigner

                                Oh interesting, I was under the impression all the new license schemes std/stdplus/pro had that?

                                If it was still under old ES licensing maybe not, but you might be right about v9.5 I think you need to be on VX releases to

                                take advantage of any Central Library functionality?

                                • 13. Re: Alternate symbols in DxDesigner

                                  You are correct.  When I run VX1.2 I have the Central Library.  When I run 9.5 the Central Library is unavailable.  Now back to 9.5 before my designs get upgraded and can't go back... 

                                  • 14. Re: Alternate symbols in DxDesigner

                                    In VX.2 you will not need to use alternate symbols to manage rotations, all rotation data will be stored in a single file (by default the *.1) Alternate symbols, those with different graphics, for example ANSI or IEC can be stored as a *.2 etc and it too will have the rotations stored there. For an example, if you have VX.1.2 then look at the resistor in the StarterLibrary (added by default to a project created using the 'PADS' template) and you will see an ANSI resistor, the .1 and an IEC resistor, the .2. Both carry rotational information so that they look correct when rotated, mirrored and flipped. In VX.1.2 you cannot edit these rotational views, but you will be able to in VX.2. Keep a look out for documentation on 'Compound Symbol' in the VX.2 release for an explanation.

                                    1 2 First Previous