[PCB_FORUM] Re: Where do you set drill to other features clearance?

Hi Gary,

All positive planes...I'll never use negative planes again...if I can help
it.

In PADS I removed the inner layer pads on the layers that didn't have any
connections in my via padstacks, and set a drill to copper clearance.  Drill
was 10, clearance was 7.  Effectively, a 24 mil "void" in the planes.  My
pad to copper clearance was 6.

To accomplish the same thing in Allegro, in the padstack editor, I removed
all the inner layer pads on the layers that didn't have any connections, and
added to all those layers with no pads an anti-pad of 12 mils.  I setup
clearance for pad to shape to 6.  I updated all the vias on the board, and
voila!, seems to work just as I expected and I now effectively have the same
24 mil "void" in the planes.

This almost works the same for trace to pad, but I need to do a little
tweaking there I think to get the same results as I had in PADS.  I liked
having drill as an object to have clearance to in PADS, and wish Allegro
offered the same feature...

Regards,

Austin
  -----Original Message-----
  From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of Macindoe, Gary
  Sent: Friday, June 20, 2008 11:23 AM
  To: icu-pcb-forum@xxxxxxxxxxxxx
  Subject: [PCB_FORUM] Re: Where do you set drill to other features
clearance?


  Hey Austin,



  The clearance for a shape is accomplished in one of two ways (negative or
positive shapes).



  For inner negative shapes (planes), Allegro uses the padstack definition,
"Anti Pad".

  If you need to increase this clearance on a board wide basis, you would
modify the "Anti Pad" definition for the padstack in the design.

  If you want to increase the clearance on a case by case basis (i.e.
"individual THP"), use Shape -> Manual Void -> Circular (or Rectangular,
Polygon etc.).



  For a positive inner or outer shape, you have much more control.

  Using Shape -> Global Dynamic Params., you set up the parameters that will
be applied to every shape that you create in your design.



  Then, you can adjust the parameters of each shape individually, after it
is created:

  -          Shape - > Select Shape or Void

  -          click on the shape to highlight it

  -          RMB on the shape to Parameters.

  -          Adjust the parameters as needed





  Good luck, e-mail me if you have any questions about this.



  Gary





  Gary E. MacIndoe
  PCB Design Engineer
  Fort Collins, Colorado

  amd.com

  gary.macindoe@xxxxxxxxxxxxxxxxxxxx Message-----
  From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Austin Franklin
  Sent: Thursday, June 19, 2008 5:33 PM
  To: icu-pcb-forum@xxxxxxxxxxxxx
  Subject: [PCB_FORUM] Where do you set drill to other features clearance?



  Hi,



  In PADS, the clearance matrix contains a drill to other feature clearance

  (such as copper, trace, via, pad).  Where in Allegro can I set up similar

  clearances, say, for drill to copper (shape)?



  Regards,



  Austin



  -----------------------------------------------------------

  To subscribe/unsubscribe:

  Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx

  with a subject of subscribe or unsubscribe



  To view the archives of this list go to
http://www.freelists.org/archives/icu-pcb-forum/



  Problems or Questions:

  Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx

  -----------------------------------------------------------

GIF image

Other related posts: