Stats

  • Replies 4
  • Subscribers 66
  • Views 14238
  • Members are here 0
More Content

PCB Footprint question

OPC74

Hi,

I am trying to design a land pad like the image below... In PADS I used to be able to add all my pins and then a copper area and that would tie all the pins together, there where no errors because all the pins where tied to the same net... Now in Cadence when I create a land pad like this I have to make a shape, then export that shape as a sub drawing, then modify a library pad and insert said sub drawing as the pad shape...


The problem this causes is the schematic shapes, and pcb decal now don't match the customer drawing on pin count... 1 vs 4 pins.  So is there a way to get all my pins on Cadence instead of just 1 large one?  I have tried the adding copper shape and it's suppose to associate with the pads that it comes into contact with, but I get proximity errors... Using Cadence Allegro PCB designer 16.6

Thanks

  • You can do the same thing in a PCB Editor Package Symbol, ensure that the connecting copper shape covers the connect point(s) for the pads, usually pad centre, you will get "pin to shape" DRCs in the Package Symbol since it has no nets to reference but, once the Package Symbol is loaded into a board with a valid netlist connecting the pins, the shape and the pins will get the same net, because the shape covers the pin connect points, and the DRCs will clear.

  • Thank you so much!  Do I create the copper shape as a "sub drawing"?  do I also create a solder mask layer shape, or will it automatically clear it (add it when package is complete)?

    Best regards

  • Use Shape>Polygon set the Options for Etch / Top and draw the required shape to cover the pins, as described. If you want the same shape for soldermask, Edit>Z-Copy Shape, set Options for the target layer, likely Class Package Geometry / Soldermask_Top and the select the copper shape just added in the canvas. (Otherwise use Shape>Polygon again and change the Options to Package Geometry / Soldermask_Top and draw the required soldermask shape)

  • Thanks!  I was finally able to try it, and it worked perfectly, the Z-copy is awesome!  I ran all the gerbers and no problems.

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.