4 Replies Latest reply on Nov 15, 2013 7:30 AM by mcrist

    Selecting the pin name in DxDesigner

    mcrist

      When  we translate our designs into Expedition, sometimes the text comes in at a different size and font.  I'd like to select all of the net names, components properties and pin names and change the font size and face to our current standards.  I've managed to change the net names and component properties, but can't figure out how to select the pin names.  I'm trying to change the purple text in the screen shot below, which is a pin name.Pin_name.PNG

       

      How do I select pin names?

        • 1. Re: Selecting the pin name in DxDesigner
          Satoru

          Hi mcrist-san,

           

          Can't be edited on DxDesigner, because Pin Name is the property which the symbol has.

           

          Regards,

          Satoru

          • 2. Re: Selecting the pin name in DxDesigner
            mcrist

            By setting my selection filter to  Property, I am able to select this pin text and change the font color and size manually:

             

            Change_Property.PNG

             

            This is a zoomed in shot of the same pins.  This isn't changing the symbol in the library, just the local design instance.  I think I was unclear in my first message, I am trying to programatically  change the font size of a property of a pin on a symbol.  But I can't find how to access that property.

            • 3. Re: Selecting the pin name in DxDesigner
              Satoru

              Hi mcrist,

               

              I think that the property is a user property.

              If a property that can be selected, Automation can get it.

               

              Please select a symbol and run the following code.

              Automation will get the size and the color of property "PIN_ID".

               

              ===============================================================================

                  Dim cmp

                  Dim conect

                  Dim cPin

                  Dim attr

                  Dim temp

               

                  For Each cmp In dxdView.Query(VDM_COMP, VD_SELECTED)

                      temp = "REFDES=" & cmp.Refdes & vbCrLf

                      For Each conect In cmp.GetConnections

                          Set cPin = conect.CompPin

                          If Not cPin Is Nothing Then

                              Set attr = cPin.FindAttribute("PIN_ID")

                              If Not attr Is Nothing Then

                                  temp = temp & "[" & cPin.Number & "]" & vbCrLf & _

                                         "    Size=" & attr.size & vbCrLf & _

                                         "    ColorR=" & attr.GetObjectColor.r & vbCrLf & _

                                         "    ColorG=" & attr.GetObjectColor.g & vbCrLf & _

                                         "    ColorB=" & attr.GetObjectColor.b & vbCrLf

                              End If

                          End If

                      Next

                      MsgBox temp

                  Next

              ===============================================================================

              • 4. Re: Selecting the pin name in DxDesigner
                mcrist

                That's it!  Thank you.