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

Larry,

I am a little late to the party here but doing an Edit > Z-Copy of the
Route_Keepout/All Shape will explode it from the component and it will
no longer move with the symbol. I believe you meant to say use Edit >
Change to move the Route_Keepout/All Shape to the appropriate
Route_Keepout layer.

Hope this helps,
Michael Catrambone
UTStarcom, Inc.

-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Larry Briski
Sent: Friday, June 20, 2008 2:44 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: