Stats

  • Locked Locked
  • Replies 18
  • Subscribers 165
  • Views 29539
  • 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

Assigning a Net to an Unassigned Shape

melview1

I am using Allegro PCB Editor 16.2.

I have a symbol (dra file) that has 8 top-layer shapes in it.  These shapes are not connected to eachother.  Within each shape, I placed a pin which I would like to be electrically connected to its respective net and the shape to be connected to the pin's net (in this case all are connected to ground).  I get a DRC error regarding spacing between the pin and the shape on the same layer in the symbol file.  I assume I'm not assigning something properly.

If I put this symbol into my design (albeit with the symbol's DRC errors), the pins connect to their assigned nets just fine, but all 8 shapes are assigned to a "dummy net" and are not electrically connected to their pins or ground.  They, of course, have the same DRC error as in the symbol file. 

If I choose Display-->Status, and click on the box next to "Unassigned Shaps" I can get a "Shape Without Nets" report and it tells me how to suprpres these messages in this report for a particular shape, but these are problems in my design and I would like to fix them rather than suppress them.

I would like to know how to do the following:

1.  Properly connect the pin to the shape in the symbol, so that there are no DRCs in the symbol or brd fiile and the shapes are connected to the proper pin and net.

and

2.  Once in the brd file, I would like to be able to reassign the "dummy net" shape to the ground net, i.e. choose the shape and assign it to a net.  If I accomplish #1, I shouldn't need #2, but knowing how to do #2 would come in handy as I've ran across this issue while doing other things in layout.

 

 --Mark

 

 

If I choose Display-->Status I see that I have 8 Unassigned Shapes.  If I click on the yellow box next to it, I get a "Shapes Without Nets" report.

  • Cadpro2K

    1) SHAPE; select SHAPE

    2) make sure SHAPE is enabled in the elements filter

    2) RMB, Assign net (click on a pin containing the net name you desire)

    3) Done

    I'm not sure why this isn't connecting properly from the symbol (it seems you've done it right), but heh, somethings I never figure out.  :)

    Good day. Mitch

  • Bennigin

    You could create a pin using a shape for the top layer pad. Create a "Shape Symbol" and then you can use that as a pad when designing your pad stack. I have attached an image of an example I have used.

     

  • melview1

    Cadpro2k~

    - I select the "Shapes" checkbox in the "Design Object Find Filter" so I can select a shape

    - I select the shape that is in question

    - I right-click and get a menu that does not include "Assign Net".  This is exactly what I was originally looking for, but didn't see it, that's why I thought I was doing something wrong.  My options are:  Quick Utilities, Move, Copy, Delete, Spin, Change to Layer, Add Connect, Fix, Property Edit, Show Element, Application Mode, Super Filter, Customize, Selection Set.

    Thoughts?

     

    --Mark

  • steve

    Ensure that the centre of the pin is covered by the shape on etch - top. You cannot get rid of the DRC's in the dra file but when you import the logic in your brd file the shapes then take on the net name of the pins.

  • melview1

    I ended up taking bennigan's advice and creating a custom shape for the pad and that's the only way I was able to get it to work.  The other ways the shape would never take on the net name and would cause a DRC and I couldn't figure out how to reassign it to the proper net.

    My issue is "resolved", however I'd still like to know how to reassign a shape to a different net, but perhaps that'll be added to the list of things I'll never figure out in Allegro  :).

    Thanks for everyone's help.

     

    --Mark

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.