[PCB_FORUM] Re: Non plated Holes DRC checking?
- From: "Bolman, Shirley H" <shirley.h.bolman@xxxxxxxxx>
- To: "icu-pcb-forum@xxxxxxxxxxxxx" <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Tue, 10 Aug 2010 09:34:16 -0700
There is always a possibility of a sliver of copper floating around when you
use pad same size as drill.
We create all of our NPTH padstacks with a 10 mil spotter pad. We also define a
circular line on a board geometry
subclass that is the same size as the drill. This can then be set up so line to
line checking will generate a DRC.
Shirley in Oregon
It is a PRIVILEGE to be born free.
It is a RIGHT to live free.
It is a DUTY to die free.
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
Sent: Tuesday, August 10, 2010 4:16 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Non plated Holes DRC checking?
We create the padstack with the same size pad as drill. After it is
drilled...no more copper.
We used to have the pad smaller than the drill, but then you are not checking
the actual distance for drc.
Regards,
Mark
Bill Zembek wrote:
Hi
In version 16.3 & 16.2 you can setup the drc for hole to shape, line, hole
checks.
To create a donut pad create a circle shape, cut a narrow rectangular void,
then void the center.
It creates a C.
Bill Zembek
Technical Support - Allegro Specialist
EMA Design Automation, Inc.
225 Tech Park Drive
Rochester, New York 14623
Phone 585-334-6001 Opt 5
Fax 585-334-6693
www.ema-eda.com<http://www.ema-eda.com>
www.timingdesigner.com<http://www.timingdesigner.com>
Cadence(r) OrCAD(r) Capture CIS with Digi-Key(r) Integration
View a live demo * Register
Now!<http://www.ema-eda.com/products/orcad/cis-digi-key-integration.aspx?campaignID=164>
________________________________
From:
icu-pcb-forum-bounce@xxxxxxxxxxxxx<mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx>
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dave Seymour
Sent: Monday, August 09, 2010 2:03 PM
To: icu-pcb-forum@xxxxxxxxxxxxx<mailto:icu-pcb-forum@xxxxxxxxxxxxx>
Subject: [PCB_FORUM] Re: Non plated Holes DRC checking?
As far as the donut pads goes: One of the problems is flash symbols can not
have void:
Create symbol started.
ERROR(SPMHCS-8): Flash symbol cannot have a void in a shape.
Dave
Dave Seymour
Ixia
www.ixiacom.com<http://www.ixiacom.com>
919.267.4840
________________________________
From: Dave Seymour
Sent: Monday, August 09, 2010 1:58 PM
To: 'icu-pcb-forum@xxxxxxxxxxxxx<mailto:icu-pcb-forum@xxxxxxxxxxxxx>'
Subject: RE: [PCB_FORUM] Re: Non plated Holes DRC checking?
16.3
Dave Seymour
Ixia
www.ixiacom.com<http://www.ixiacom.com>
919.267.4840
________________________________
From:
icu-pcb-forum-bounce@xxxxxxxxxxxxx<mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx>
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Les Wong
Sent: Monday, August 09, 2010 1:56 PM
To: icu-pcb-forum@xxxxxxxxxxxxx<mailto:icu-pcb-forum@xxxxxxxxxxxxx>
Subject: [PCB_FORUM] Re: Non plated Holes DRC checking?
What version of Allegro are you using ?
--- On Mon, 8/9/10, Reade, Sue
<Sue.Reade@xxxxxxxxxxx><mailto:Sue.Reade@xxxxxxxxxxx> wrote:
From: Reade, Sue <Sue.Reade@xxxxxxxxxxx><mailto:Sue.Reade@xxxxxxxxxxx>
Subject: [PCB_FORUM] Re: Non plated Holes DRC checking?
To: "icu-pcb-forum@xxxxxxxxxxxxx"<mailto:icu-pcb-forum@xxxxxxxxxxxxx>
<icu-pcb-forum@xxxxxxxxxxxxx><mailto:icu-pcb-forum@xxxxxxxxxxxxx>
Date: Monday, August 9, 2010, 10:18 AM
To get the pull back on power layers we use Route keepout around NP pins. This
also serves the same function on signal layers to keep traces out of the holes.
Sue Reade
CAD Engineer, Hardware Engineering, NSG
(o) +1.919.461-1047 | (m) +1.919.819-8092
From:
icu-pcb-forum-bounce@xxxxxxxxxxxxx<mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx>
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Jean Bratton
Sent: Monday, August 09, 2010 1:17 PM
To: icu-pcb-forum@xxxxxxxxxxxxx<mailto:icu-pcb-forum@xxxxxxxxxxxxx>
Subject: [PCB_FORUM] Re: Non plated Holes DRC checking?
We put a pad but in the flash name we put "BLANK" and then it's not actually a
pad on the board, just a pad for Allegro to use. Alternate would be to put a
route keepout around the pin.
Jean Bratton
Senior PCB Designer
Freedom CAD Services, Inc.
Phone: 603-864-1349
Skype: jean.bratton
Email: jean.bratton@xxxxxxxxxxxxxx</mc/compose?to=jean.bratton@xxxxxxxxxxxxxx>
Visit us at http://www.freedomcad.com
From:
icu-pcb-forum-bounce@xxxxxxxxxxxxx<mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx>
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dave Seymour
Sent: Monday, August 09, 2010 1:06 PM
To: icu-pcb-forum@xxxxxxxxxxxxx<mailto:icu-pcb-forum@xxxxxxxxxxxxx>
Subject: [PCB_FORUM] Non plated Holes DRC checking?
To All,
I'm looking for alternative way of creating Non plated holes in allegro.
I have 2 situations:
1) Non plated hole, No pad. - What are people using to keep traces away
from the edge of the drill hole?
2) Non plated hole with a pad. - In this case a donut shaped pad would be
best where one could specify an inside diameter and an external diameter.
I have a current method, but am curious as to how other folks are doing either
of the above.
Thanks
Dave
Dave Seymour
Ixia
www.ixiacom.com<http://www.ixiacom.com>
919.267.4840
This correspondence and any attachments are considered confidential. If you are
not the intended recipient, please notify Freedom CAD Services, Inc.
immediately by either replying to this message or by sending an email to
operations@xxxxxxxxxxxxxx<mailto:operations@xxxxxxxxxxxxxx>; please destroy all
copies of this message and any attachments. Thank you.
Other related posts:
