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

All,
I'm reading that Dale wanted to know how to void out underneath a component's case rather than just a padstack. If that's the case (pun intended, its Friday) the method I've been using is to use the Allegro symbol editor to add a route_keepout_all shape under the component. When the component is placed onto the board, edit-z-copy the shape to the appropriate layer(s) and delete the route_keepout_all shape. This way if the component is moved the route keepout shape follows along with it. 

And yes, I learned that the hard way.

Larry

Macindoe, Gary wrote:

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

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



--
Lawrence Briski
PCB Designer
SGI

lgb@xxxxxxx
tel: 715.726.7440
fax: 715.726.4345
sgi.com
-----------------------------------------------------------
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
-----------------------------------------------------------

Other related posts: