Actions
Forum Thread Details
  • State Verified Answer
  • Replies 12 replies
  • Answers 1 answer
  • Subscribers 191 subscribers
  • Views 2427 views
  • Users 0 members are here
Related

Tidy schematic after pinswap

alberthall

I am working on a design using a microcontroller using analogue inputs and digital I/O.   The analogue pins can be swapped and the digital pins can be swapped at will (with commensurate changes in the firmware).  I have set the swap levels on the part to allow this.  I put short wires on each pin and named them and did likewise with the parts they connected to.  The parts on the board layout are connected correctly but the layout would be better if some pins were swapped.   So, on the schematic I swap some pins and the board layout correctly reflects the changes.   The problem is that the schematic is now a mess wire wires draped all over the microcontroller.  I tried using Bus/Net but the result is similar.

 

Is there a way of using pinswap without making a mess of the schematic?

Parents
  • 0

    Hey all,

     

       I came across this question and almost lost hope based on the comments.  HOWEVER, there is a work around that will allow for modularity in schematics without changing PCB pad design.  What i wanted was a schematic symbol that I can physically alter the pin arrangement so i don't have a schematics rats nest, all while maintaining the pin-to-pad linking that was there in the first place.

     

       The Solution I have:

      

    1. Create a symbol level pin for the library you are working in.
      1. This is a simple as simply placing a pin and saving it as a generic PIN1
      2. Note: If you want to be able to PIN SWAP STILL you will need to produce a number of pins equal to the number of swappable pins on your final schematic part (i.e. if you expect 36 swappable pins on a part, then that library can have PIN1 -PIN36 defined).  This is because pinswap will not occur if the pins have the same symbol name for a component part.
    2. Create the symbol for the package SANS pins.
      1. This takes a little bit of work on your part to make sure the package is the right size for the size pins you created.
    3. Create a Device
      1. Choose the Package you already have designated for the part you will use
      2. Go to Change-> Add Level (Always), means that every component you add will be placed immediately.  You can look at the other levels if you are interesting in more interesting device placements.
      3. In order to do a gateswap, change the swap level to non-0 in the device creation manager.  Note, this is different than the swap level of the individual PINS you will be adding in regards to pin swapping.
      4. Add+ :
        1. Your Strictly Symbolic Package Body
        2. Each Pin the body should have
          1. Place them according to how you would have if designing the symbol as a single package.  (You can place PIN 1 for all of them if you don't care about pinswapping, or can add different pin symbols for swappability in the future)
          2. Change the NAME of each pin to the PIN number you expect (i.e. 1,2,3, etc.)
      5. Connect the Pins on the Package to the Pins on the Device; the pins will have format {NAME.SchematicPinName}.
    4. In your schematic you may now Place the Device.
      1. Caveats:
        1. Each Pin and the body are now moveable on their own.  To do operations or rotations, use group select and group move or rotate.
        2. If you have not Net connected any pins, a quick way to swap pin orientation is to use GATE SWAP.  Warning:  If you have Connect Pin1 to Vin and Pin 3 to D+, GATE Swap on Pin 1 and 3 will swap the pins on the schematic, but will not maintain the routed connection (i.e. Pin 3 now goes to Vin, and Pin 1 now goes to D+)
        3. If you want to maintain the already routed net, then individually select the pins and reposition them in the schematic.

     

    I hope this helps.  While there are some caveats, this beats having to version name every single pin change if you want to have a nice schematic and useable device!

     

    Let me know if this fails in any ways!

Reply
  • 0

    Hey all,

     

       I came across this question and almost lost hope based on the comments.  HOWEVER, there is a work around that will allow for modularity in schematics without changing PCB pad design.  What i wanted was a schematic symbol that I can physically alter the pin arrangement so i don't have a schematics rats nest, all while maintaining the pin-to-pad linking that was there in the first place.

     

       The Solution I have:

      

    1. Create a symbol level pin for the library you are working in.
      1. This is a simple as simply placing a pin and saving it as a generic PIN1
      2. Note: If you want to be able to PIN SWAP STILL you will need to produce a number of pins equal to the number of swappable pins on your final schematic part (i.e. if you expect 36 swappable pins on a part, then that library can have PIN1 -PIN36 defined).  This is because pinswap will not occur if the pins have the same symbol name for a component part.
    2. Create the symbol for the package SANS pins.
      1. This takes a little bit of work on your part to make sure the package is the right size for the size pins you created.
    3. Create a Device
      1. Choose the Package you already have designated for the part you will use
      2. Go to Change-> Add Level (Always), means that every component you add will be placed immediately.  You can look at the other levels if you are interesting in more interesting device placements.
      3. In order to do a gateswap, change the swap level to non-0 in the device creation manager.  Note, this is different than the swap level of the individual PINS you will be adding in regards to pin swapping.
      4. Add+ :
        1. Your Strictly Symbolic Package Body
        2. Each Pin the body should have
          1. Place them according to how you would have if designing the symbol as a single package.  (You can place PIN 1 for all of them if you don't care about pinswapping, or can add different pin symbols for swappability in the future)
          2. Change the NAME of each pin to the PIN number you expect (i.e. 1,2,3, etc.)
      5. Connect the Pins on the Package to the Pins on the Device; the pins will have format {NAME.SchematicPinName}.
    4. In your schematic you may now Place the Device.
      1. Caveats:
        1. Each Pin and the body are now moveable on their own.  To do operations or rotations, use group select and group move or rotate.
        2. If you have not Net connected any pins, a quick way to swap pin orientation is to use GATE SWAP.  Warning:  If you have Connect Pin1 to Vin and Pin 3 to D+, GATE Swap on Pin 1 and 3 will swap the pins on the schematic, but will not maintain the routed connection (i.e. Pin 3 now goes to Vin, and Pin 1 now goes to D+)
        3. If you want to maintain the already routed net, then individually select the pins and reposition them in the schematic.

     

    I hope this helps.  While there are some caveats, this beats having to version name every single pin change if you want to have a nice schematic and useable device!

     

    Let me know if this fails in any ways!

Children
No Data