7 Replies Latest reply on Dec 21, 2015 2:45 PM by john15

    Schematic net missing from pin in layout


      Using PADS VX.0 Flow
      Schematic: xDxDesigner

      Layout: PADS VX.0 (July 8 2014 23:35:32)


      I am using a heirarchical schematic.


      I have a fuse holder that uses four through hole pins - two per side of the fuse.  The fuse is used in various places throughout the design. The following problem description affects every instance of the fuse in the design.


      Because PADS effectively requires a separate terminal for each through hole, I created a decal and associated schematic symbol with four terminals/pins. Pins 1 and 2 are the same net and

      pins 3 and 4 are the same net. In the schematic, I can generate a list of connected nets for any fuse and I will see that all four pins have an associated net. The duplicated net names are are paired to the pins correctly. When forwarded to the layout, every instance of the fuse leaves pin 3 without its assocaited net. In PADS, I can see in the project explorer that the net which should be connected to pin three only shows that it should be connected to pin 4 (half of the required pair). The report generated when forwarding from the schematic to layout does not mention any conflict or reason for removing the associaton.


      I can ECO the net association to pin 3. When I attempt to push the change back to the schematic, I get the following notes in pcb.err
      pcb: Warning 6051: 50388 pin $16I613\$1I1418.3: Duplicate pin number
      pcb: Warning 6051: 50388 pin $16I640\$1I1620.3: Duplicate pin number
      pcb: Warning 6051: 50388 pin $16I640\$2I1437.3: Duplicate pin number
      pcb: Warning 6051: 50388 pin $16I640\$2I1459.3: Duplicate pin number
      pcb: Warning 6051: 50388 pin $16I640\$2I1479.3: Duplicate pin number
      pcb: Warning 6051: 50388 pin $16I640\$2I1499.3: Duplicate pin number
      pcb: Warning 6051: 50388 pin $16I640\$2I1519.3: Duplicate pin number


      Each one of those identifiers is an instance of the fuse. The schematic does not not change in any way that I can tell, and pushing back to the PCB for any reason will clear the net assignment I made with the ECO. If I search for the identifiers listed I see that the identification numbers are unique in the design. I do not see any duplication of pin 3  in any of the part definition files. I have exported and used notepad to inspect *.p, *.d files from PADS; they look reasonable. The text behind the xDxDesigner symbol file is beyond my understanding but also seems okay.


      What's the deal?

        • 1. Re: Schematic net missing from pin in layout

          Hi John. I've moved your question to the PADS Schematic Design sub-community where it should get a quicker response. -Cathy

          • 2. Re: Schematic net missing from pin in layout

            On the PADS side the part was designed for swapping pins, but the PINSWAP on the schematic symbol was missing preventing pin swaps on back annotation.  I have attached an updated symbol.

            pinswap.png !


            Verify your pin numbers by selecting each schematic pin, and compare the Block pin numbers match the Symbol pin numbers.  In my example, pin 1 and 2 don't and are visible because I have swapped them.


            It's important to note, that the PINSWAP command works on the name of the pin, and not the pin number, which happens to be the same in the symbol you provided.

            • 3. Re: Schematic net missing from pin in layout

              I updated all of my schematic symbols and saw that the pin swap properties from your screenshot were visible. I used the xDx "PCB Interface" and PADS "xDx Designer Link" tools to attempt a push and pull of the changes to the PCB. No improvement that I can see.


              I reverted to my schematic symbol and removed the pin swap settings in PADS Part definition (set all terminals to swap=0). That also did not solve the issue.


              Regarding the pin swap, it would have been nice that the paired pins were swappable and that the pairs themselves were swappable. That is logically correct for the component to be mounted. The swapping of terminal pairs is exactly equal to rotating the part 180° so although PADS does not seem to support that kind of swapping it's value is pretty minimal. For this particular project it turns out the swap settings overall are a "don't care".


              As a sanity check I have used the cross probing feature to show that when I highlight parts in PADS they are highlighted/focused in xDx Designer. The converse is also true.

              • 4. Re: Schematic net missing from pin in layout

                click on pin 3 in the schematic, what are the values for the #= property?

                • 5. Re: Schematic net missing from pin in layout

                  There are no symbols in the schematic that allow me to highlight individual pins directly. I can add and remove net connections readily, but no resistor, IC, power or ground tap, connector, etc. etc. has a pin that is separately clickable. I can cross-probe to schematic pins from PADS, though, which is interesting. If I have PADS set to click "anything" and I touch a pin on the decal xDx will highlight a pin and show me the properties you requested. That doesn't seem to jive with your assumption so I'm guessing something is broken or some tick box is unchecked somewhere.


                  I learned some things and did some things without solving the problem. Process looked like this:

                  When I probe pins in PADS I see that PADS and xDx disagree about the fuse. Pins 1 and 4 are on the left side (should be 1 and 2). Pin 2 is clickable but Pin 3 is disassociated. No highlight or properties show up in xDx whatsoever. Following that I:

                       1. Found and removed an incomplete PADS CAE gate that incorrectly specified 2 pins only. I should now only have an xDx to PADS Layout relationship possible.
                       2. I clicked "Define pin mapping of Part Type pin numbers to PCB Decal". This results in a warning and won't save the setting. Seems okay though
                                 "Warning: Pin Mapping is no longer needed - all pin numbers in part type and decal are equivalent."
                       3. I re-ordered the pin sequence in the xDx library editor. If I clicked the around in the editor the pins were identified correctly but I moved pins around and renumbered my list so they are sequential in the symbol editor. It is still true that 1 and 2 are "left" pins and 3 and 4 are "right" pins.
                       4. I verified that the sequential list in the PADS part definition is no longer used. All entries are blank.
                       5. I updated the schematic symbol
                       6. I updated the fuse part and decal from the new library definition
                       7. I forwarded to the PCB using the annotation tool from both applications


                  The process had zero effect on my results. Pins 1 and 2 still cross probe on opposite sides of the schematic symbol and pin 3 is still logically missing. No properties for pin 3 show up.



                  Ran "Check Design against PADS Decal Pin Numbers" tool. Result was "No errors were found for this design"

                  Ran xDx diagnostics. All 17 of the default scripts passed which includes tests for

                       empty labels

                       duplicate internal ids

                       net connections

                       component graphical data

                  • 6. Re: Schematic net missing from pin in layout

                    Using the selection filter, you can select pins directly, and then view the pin numbers in the property window.


                    Using the symbol I sent you, I have pin 2 on the schematic selected, but on the symbol this is pin 1, because the pin numbers have been swapped.

                    From the error, I am guessing you have multiple pin 3 at the block level, perhaps because once placed on the schematic, pin numbers are not automatically updated if changed on the symbol.



                    If you continue to have an issue, call support to setup a web session and review the error.

                    • 7. Re: Schematic net missing from pin in layout

                      The solution was to copy the schematic library symbol to another name. I used the library editor to copy my part definition in PADS to match. Suddenly my net connection worked. I reverted the name change without changing anything about the symbol/part/decal definitions and I still get to keep my net. That's a pretty insidious bug. Clearly, the software previously noticed changes and was able to update parts, silk, etc. but did not push everything. My only clue was a warning when annotating in a particular direction as described above.


                      If a "duplicate" pin (which I couldn't make intentionally if I tried) can result in the software choosing to make netlist edits it should really be a full stop error, not a warning. The software should not guess the intent of a designer for the same reason compilers don't throw away code. If it knows you're wrong, fine. Stop working and give a useful response. If a compiler generated executables with chunks of libraries thrown out because of a warning level event there would be outrage and brimstone.


                      Selection filter> [x] Objects - got it. Thanks for the help.