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

Not really all symbols.....when you replace a padstack inside the board
layout you have the ability to pick
a particular ref des, symbol, even pin number. So you could be pretty
particular about which pin you choose.
You would make the anti-pad the same size as the smd pad, it would be a
1 to 1 copy if the geometry is
the same. Depends on what your SI group is looking for.
 
 
Mike
 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Macindoe, Gary
Sent: Friday, June 20, 2008 3:21 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Where do you set drill to other features
clearance?



Dale,

 

The method that Mike describes below will work. But... keep in mind that
all symbols that use this padstack will be affected.

Also, I would make the anti-pad for the ground relief a little larger
than the smd pad.

You could create a unique name for this padstack that's only used for
that symbol.

 

Good luck!

 

  

Gary E. MacIndoe
PCB Design Engineer
Fort Collins, Colorado

amd.com

gary.macindoe@xxxxxxx

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
gnieski_mike@xxxxxxx
Sent: Friday, June 20, 2008 10:52 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Where do you set drill to other features
clearance?

 

    Do an edit padstack for the pad in the footprint, open the pad and
make and anti-pad on the gnd layer

    using the same geometry as the surface pad. Save the pad as a
different name....then replace the padstack

    on the component with the new one, it will void the layer below.
Only problem is that if you ever need to

    refresh the footprint you lose the void.

 

    Mike

 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dale Rasmusen
Sent: Friday, June 20, 2008 12:41 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Where do you set drill to other features
clearance?

Hi Gary,

 

I have a smd component that requires the gnd plane (layer 2) to be
cleared underneath the part for SI reasons.  Do you have any good
automatic way of doing this other than making a manual void in the
shape?

 

Thanks,

 

 

Dale Rasmusen

CAD Manager

TEKNOVUS

(707) 665-0400 ext 133

(707) 665-0491 fax

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Macindoe, Gary
Sent: Friday, June 20, 2008 8:23 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: