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

Thanks guys, I really like to see the different methods.  We are starting to 
use the upper G speeds, so we need to simulate how this is going to work.

Thanks,


Dale Rasmusen
CAD Manager
TEKNOVUS
(707) 665-0400 ext 133
(707) 665-0491 fax
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Larry Briski
Sent: Friday, June 20, 2008 12:44 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [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
-----------------------------------------------------------
-----------------------------------------------------------
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: