Stats

  • Locked Locked
  • Replies 3
  • Subscribers 164
  • Views 13665
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Getting a static shape in part symbol to connect to a net

Mattski

I have a board with a lot of RF connectors, and 5 different ground nets for different board sections.  The footprint for the RF connector has 2 ground pads, and one signal pad, and also some static shapes connected to the ground pads that will make the signal pin coplanar waveguide.  I have defined those shapes seperately because it needs to be a precise width, and the spacing is a precise amount that I don't want defined by the constraint manager.

For most of my board it recognizes these static shapes as belonging to the ground nets where it is physically connected to the connector ground pins, and thus it properly connects it to the ground pour that I have on the top layer.  On some sections of my board, it is only showing up as belonging to the Dummy Net on Etch/Top, and thus the ground pour is not being fully connected to this static shape - it is using the shape-shape spacing rules to put a void in between. This is still the case when I have a ground via connecting this static shape to the ground plane beneath it.

I have tried re-netlisting the design,refreshing the symbol drawing, updating shapes to smooth, checking shape outlines in DB Doctor, derive connectivity, and save-exit-reopening, but it is staying as Dummy Net. I know that I could redraw the symbol drawing and create a pad which I draw to be this irregular shape.  I would prefer not to do that since it takes quite a bit longer, and the static shapes have worked properly at least in some sections of my board - I just don't know why yet.

 What do I do to get these static shapes to show up with the net of the pin that they are overlapping?

  • redwire

     Sounds like you're doing it right so without seeing the board  I don't know what's wrong.
    For the time being select the shape manually and assign the net.  Should clear up.

  • mcatramb91

    I am assuming that the static shapes have been defined inside of the RF connector symbol.  If this is the case then the only time that these static shapes will assume the net name of the pins that are connected to (flooded on top) is when they are placed in the design.  If you copy the RF connector symbol around the board the static shapes will assume Dummy Net and will remain that until you manually reassign the static shape to GND.  Doing a Netlist import or symbol refresh has not effect on these static shapes, as you found, because you only have one shot of automatically assigning these static shapes to the nets of the pins that are flooded on top of is when the are placed on the board.

    My suggestion is to generate a placement file of the design using File > Export > Placement, deleted the RF Connectors with the Dummy Net static shapes and reload the placement file using File > Import > Placement.  This will replace the RF Connectors and in doing this the static shapes will associate to the Pins they are flooded on top of in the connector symbol

    Hope this helps,
    Mike Catrambone
    UTStarcom, Inc.

  • Mattski

     Thanks Mike, the trick with exporting and importing the placement worked!

     It is interesting to note that all of these connectors were placed before I updated the part symbol to include this additional shape.  However, some of them had the proper net, and some did not.  Sometimes there were two shapes in the same part symbol, one which assumed the net, and one which didn't.  

    Also it is useful to note for others reading this thread that this import/export trick only worked for the connectors that had this static shape already connected to the appropriate ground net.  It is not inheriting the net from the pin that it is connected to.  In fact, by placing a shape with a different net altogether on top of the static shape that is in the part symbol, it will inhert that net rather than the net of the ground pad (with ground net) that it is also connected to.

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.