2 Replies Latest reply on Mar 17, 2017 4:09 AM by Robert Sterling

    Importing of other Cad Data from Eagle and Altium

    Robert Sterling

      It is quite common to find reference designs on the Web provided by industry such as Atmel, Ti ,ST, Circuitmaker, Ardrino, Octopart etc.

      It would be great if they conformed and provided cad packs in every software version but they normally only provide reference data in the format the design team used to make their demo board.

      So we have to convert it so we can use these files things do go wrong so i have some questions:

       

      1: Is it necessary to have access to the original library parts

      2: How accurately are the schematics matched to the PCB.

      3: Do we need to download demo/free version of the other cad packages to verify the content of the converted files.

      4: Are there any easy ways to do this:

        • Re: Importing of other Cad Data from Eagle and Altium
          Russell Lewandowski

          I have imported Arduino boards and shields as well as Atmel XPlained MCU and extension boards into Solidworks PCB.  My experiences are as follows:

           

          - Arduino UNO R2 boards do not have any separate libraries embedded.  Part schematics and footprints are in the base .sch and .brd files.

          - Various Arduino Shields may or may not have separate libraries embedded.  SWPCB does what is appropriate.

          - Atmel Altium files do not directly import.  I just copy the files into the project directory and 'add existing documents'.  This works for schematics (.SchDoc), schematic libraries (.SchLib) and PCB libraries (.PcbLib).  The PCBs do not open (.PcbDoc) or import.  SWPCB uses a .SWPcbDoc file that is slightly different.  Probably to store addtional ECAD-MCAD parasolid information since it comes with PCB Services ECAD-MCAD bridge.  Not sure if SW is going to provide a converter or make them cross compatible in the future.  I run PCB 2017.2. 

          - Proteus does not import at all.

          - I have not tried others.

           

          For your questions:

           

          1) The library parts should be embedded in whatever vendor supplied files you import/copy.

          2) SCH and PCB match exact for Arduino boards and shields I have imported.  Atmel Altium files do no import .PcbDoc.

          3) I have not downloaded other cad packages to verify.

          4) Easy to import.  Still have to work the BOM to make sure all the parts are available and substitute as needed.  No easy way around that.

           

          Here is my proto board that has Atmel XPlained headers, Arduino shield headers, Grove connectors (I2C, TX, etc), XBee, breadboard, buttons, switches and LEDs.  Only issue was the imported Eagle Arduino headers used ~30th holes and I ordered ~37th pins. 

           

          AtmelArduino.pngAtmelArduinoIRL.png

            • Re: Importing of other Cad Data from Eagle and Altium
              Robert Sterling

              Hi Russell

              I like your Proto Board - Looks like a real fun project!

              I have found that to import Altium files they need to be saved in version 6 format - In Altium they then import into Solidworks with no problem.

              I have also found out that Eagle Version 7 files import the easiest so it pays to download version 7 and save the files with this prior to importing to Solidworks pcb.

              Duplicate rules may be created so look into the rules post import to see if they are correctly setup.

              Pay particular attention to the clearance rule, trace width, via, hole size and polygon connect styles.

              Also single pads identifier should be correctly numbered/named to avoid conflict.

              With Proteus – Use the Eagle software to convert the files to Eagle then convert the eagle to Solidworks PCB – This is a long way round but it works.

              Autodesk 123 file also import but lose some polygon data,

              In all cases make sure you have linked the component links in the pcb to avoid drc errors and compile issues post import.

              I hope I can find the time to write a whole blog on the steps to follow soon.

              Best regards

              rob