Stats

  • Replies 17
  • Subscribers 161
  • Views 19873
  • Members are here 0
More Content

GND and VCC planes not assigned to GND VCC Nets

Cailloux

Schematic NETLIST is generated without any error. I can Import into PCB Editor from Import > Logic with no error. On my Schematic I have a GND Net and a VCC Net as well as many other Nets. The Cross Section is comprised of TOP, GND, VCC, BOTTOM ( 4 layers ).  GND layer has been assigned to the GND Net and VCC layer to VCC Net, using the creation of rectangular Shape creation, as directed in the Allegro PCB Editor Training Manual. Placing is complete and no DRC error shows up. I am ready to AutoRoute the board.

Everything goes quite well and the Board is now routed, still no DRC errors shows up.

Yet, I clearly see GND segments on the TOP and BOTTOM layers as well as VCC segments on the TOP and BOTTOM layers. It’s as if the AutoRouter did not observe the VCC Net to VCC plane assignment nor GND Net to GND plane assignment. Net Assignments to Plane where performed without error and Shape colors appeared on the screen after completion, so I have no reason to suspect the assignment went wrong.If I transfer a TOP net segment to BOTTOM where a GND segment is crossing, I get a DRC error clearly showing that both segments are in contact. Which clearly indicate that this GND segment is located on the BOTTOM layer.

What Im I doing wrong  ?  What can be the source of this problem ?

Parents

  • Hi. You need to turn GND and VCC off prior to running the autorouter. I haven't used it in some time, but there's a attribute you give nets so they don't route.

  • in reply to CadAce2K

    Almost there. I found how to turn GND and VCC off prior to autorouter but the result is that after autorouting now 49 pins are reported as Not Connected. I zoomed on a few of them and cannot graphically recognize if they are connected or not. How can I tell if an electrical connection as been done with the GND plane ? If connections are there why would the Unconnected Pins Report tell me that 49 pins are unconnected ?

    Thanks for your help

  • in reply to Cailloux

    Hi. You may need to refresh your shapes to get the connections completed. Either 1) Display/Status and see if the shapes need to refresh (green or yellow?); or 2) Tools/Database Check and click the top 2 open boxes ON and run 'Check'. That will refresh them too. If you're not sure, email me the .brd file and I can look. Regards.

Reply
  • in reply to Cailloux

    Hi. You may need to refresh your shapes to get the connections completed. Either 1) Display/Status and see if the shapes need to refresh (green or yellow?); or 2) Tools/Database Check and click the top 2 open boxes ON and run 'Check'. That will refresh them too. If you're not sure, email me the .brd file and I can look. Regards.

Children
  • in reply to CadAce2K

    Hey! A big thank you for your support. Attached is a link to my shared Google Drive. It contain 2 *.brd files. One is not routed the other is. See if you can find my misunderstanding, for I am sure this is a detail I am not getting yet. I am kind of new to PCB Editor and currently going through the Training Book. Thanks again

    My Google Drive

  • in reply to Cailloux

    The problem is your inner layer pads are the same size as the drill. The software does not have anywhere to connect the thermals. Increase the pad sizer ahd they will connect. 

  • in reply to Lennie

    From which part did you see that? I looked at C22 pin 2 pad, a GrouNDed pin.  PAD44CIR34D  Drill is 36 and Default Internal Regular Pad is Circle 54 ( a bigger ring then drill)  . That is a pad that I modified. Added pad and footprint files to Google Drive in case you want to see them.

    I did peak at PAD44CIR33 in the original library, not modified. The pad designer show drill size 33mils and Default Internal Regular Pad is Circle 33 ( ring and drill same size ) . I understand why such situation could create a problem, still this is an original unmodified pad, another puzzle to clarify later.

    I still don’t see what is wrong with PAD44CIR34D. The Inner pad is bigger than the drill isn’t it?

    By the way, related to the autorouting I do get an electrical connection on one pin. That pin that was chosen when I attached the shape to net, using Select Shape or Void command and RMB Assign Net. Still the autorouter wiil route all other GND pins.

  • in reply to Cailloux

    If you select the pin C22.2 / right click  mouse button / modify design padstack/single instance the padstack editor will come up. Look under design layers and you will see the outer layers are 54 and the inner are 36. They are the same size as the drill. 

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.