Stats

  • Locked Locked
  • Replies 3
  • Subscribers 166
  • Views 16881
  • 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

Thru Pin to Shape Spacing DRC

TC2019

Hello Everyone,

I am using Orcad PCB Designer Standard (version 17.2-2016 S065 [3/16/2020] Windows SPB 64-bit Edition) to design my second board and run into this Thru Pin to Shape DRC. Any help would be very much appreciated.

My board is a 4-layer board (signal/GND plane/PWR plane/signal). Whenever I add a shape (for copper) to enclose a thru-hole part on the inner plane (GND or PWR), I get this DRC on every pin of the part. The copper connects to all the pins and therefore these P/S DRC errors. Yet, when I add a shape in the same way on the outer layers, there is no problem. I did not run into this problem while working on my first board.

I am attaching two screenshots for your review with shape enclosed an 8-pin through-hole terminal block:

- Screenshot 1 with orange shape on the GND plane (with 8 DRC's)

- Screenshot 2 with green shape on the top signal layer (with no DRC)

- Screenshot 3 with green shape on the GND plane of my first board (with no DRC)

Please note that the second board started from scratch and not from the first board design environment/settings. I have checked the "Shape -> Global Dynamic Parameters..." of both files and they are the same.

What seems to be the cause ?. What other areas should I check?. Thanks.

TC

Parents

  • I think your sceenshot ID is wrong.  Screenshot 2 has the orange so let's discuss.

    Do you see anything obviously different between the orange shape and the pins?  I can't see any pin space clearance on the orange shape.

    What is the clearance rule in the global shape parameters?  DRC or Antipad?

    Did you read this help box?

  • in reply to redwire

    Hi Redwire,

    Thanks for your quick comment.

    There is no pin space clearance on the orange shape. This is precisely the issue that I am having. It should have a void clearance around each pin, but in this case the orange copper pour (with dummy net) connects to all pins and therefore DRC errors at all those pins.

    I did read the Help box. I have 8 mils as default spacing set for "Thru Pin To" all. I also set DRC for thru pin under "Clearances". You can see these in the screenshot below.

    Please note that I assigned the shape to GND net this time. The 4 GND pins (2,4,6,8) are connected to this net but the rest of the pins still have this DRC error. I have also tried setting Thru pin under Clearances to Thermal/anti with 20 mils for Oversize value and still got the same error. This error is very strange because I do not get it when I do the same on my first board.There must be some differences in settings that I cannot figure out.

    Please also note that this second board was created using File -> New Drawing -> Board (Wizard) and followed the steps prompted; whereas, I created the first board manually (like drawing design outline, route keepin, etc...). 

    TC

    PS. I referred to filenames given to the screenshots as image ID. After posting, the images appeared in different order leading to incorrect references in the message. 

Reply
  • in reply to redwire

    Hi Redwire,

    Thanks for your quick comment.

    There is no pin space clearance on the orange shape. This is precisely the issue that I am having. It should have a void clearance around each pin, but in this case the orange copper pour (with dummy net) connects to all pins and therefore DRC errors at all those pins.

    I did read the Help box. I have 8 mils as default spacing set for "Thru Pin To" all. I also set DRC for thru pin under "Clearances". You can see these in the screenshot below.

    Please note that I assigned the shape to GND net this time. The 4 GND pins (2,4,6,8) are connected to this net but the rest of the pins still have this DRC error. I have also tried setting Thru pin under Clearances to Thermal/anti with 20 mils for Oversize value and still got the same error. This error is very strange because I do not get it when I do the same on my first board.There must be some differences in settings that I cannot figure out.

    Please also note that this second board was created using File -> New Drawing -> Board (Wizard) and followed the steps prompted; whereas, I created the first board manually (like drawing design outline, route keepin, etc...). 

    TC

    PS. I referred to filenames given to the screenshots as image ID. After posting, the images appeared in different order leading to incorrect references in the message. 

Children
  • in reply to TC2019

    Hi,

    After looking into how new Board (Wizard) creates a new layout and a few trial and error in new board creations, I have found the answer to my problem. I used default settings in the wizard in creating my second board, particularly the "Generate negative layers for Power planes" option. I left this box checked. To correct the problem, I unchecked the two boxes under Cross-sector Editor -> Physical -> Negative Artwork for the two inner planes (GND and PWR). After that, the orange shape no longer connects to the pins.

    I hope others find this helpful. Thanks.

    TC

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.