4 Replies Latest reply on Nov 22, 2013 12:49 AM by Janice

    Import from Altium to Pads

    Janice

      Hi,

      I have a few questions regards to PADs Layout :

      1) Can i connect 2 split plane(eg. AGND , GND) with a track directly and preserve their net name?

      2) How to preserve reference designator when merge 2 design in a Layout?

      3) What is the function of COMBINE, when to use?

      4) Can we use REUSE on a design instead of using copy and paste to merge 2 designs together?

      Thank you.

        • 1. Re: Import from Altium to Pads
          David Ricketts

          1. Yes. Draw a copper shape where you want the tie, check the "copper bridge" box in the properties box, and follow the prompts.

           

          2. You can't have duplicate ref. des. If they're all different, you'll have no problem. Otherwise, see answer to 4.

           

          3. Combine is for creating a single object out of many 2D lines and text. Useful for objects like logos, drawing outline templates, etc.

           

          4. You can use Reuse for merging two databases. Select one of them, and save it all as a file with Reuse. Open the other database, go into ECO mode, and select Add Reuse. This will let you do an intelligent merge, combining and/or renaming parts and nets in several different ways. They both need to have the same number of layers.

          • 2. Re: Import from Altium to Pads
            Janice

            Hi David,

            Thank you for your reply.

             

            As for the 4th questions.

             

            4. You can use Reuse for merging two databases. Select one of them, and save it all as a file with Reuse. Open the other database, go into ECO mode, and select Add Reuse. This will let you do an intelligent merge, combining and/or renaming parts and nets in several different ways. They both need to have the same number of layers.

             

            I tried doing it, but the Make Reuse do not include the board outline (even i choose the board outline in the Edit-Filter), therefore I select all and click Combine,  followed by the rest of your instruction, and it works.

             

             

            Another question:

            1) There are 2 type of importing other CAD tools design : PADs Layout/Schematic Translator and Import. What is the difference?

             

            Thank you again.

            • 3. Re: Import from Altium to Pads
              David Ricketts

              I forgot about the board outline part. For this purpose, the workaround is you're able to select the shape, then change it to a 2d  line before creating the reuse.

               

              Another restriction of PADs is you're only allowed one board outline. That's because it's a special entity used in calculating errors and clearances. If you're trying to put more than one board on a panel, then you need to get creative with how you define the separate boards. I put all the board outlines on the Drill Drawing layer, and expand the system board outline to definae all of the outer edges, and encompass all the boards. This will allow you to run DRC correctly.

               

              I don't think there is a difference between Import and the translators, maybe the controls are different, but you might be better served asking that question over in the "Ask the Pads Team" community.

              1 of 1 people found this helpful
              • 4. Re: Import from Altium to Pads
                Janice

                Hi David,

                Thank you for your reply.