[PCB_FORUM] Re: Removing unused pad rings on inner layers DURING design...
- From: "Musetti, Carl" <cmusetti@xxxxxxxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Fri, 1 Apr 2005 10:38:39 -0500
Yes Chris that is exactly what I am saying but I still would advise completely
ignoring manufacturing tolerance. as the is a tolerance on where the drill head
actually hits the board vs. specified XY coordinate in the drill file. I
believe this is referred to as drill wandering. Another thing to be aware of is
that many drill machines are only calibrated to a mil, so you can specify
coordinates in sub mil values in your drill file but if the drill machine is
only calibrated to a mil then those sub mil values will be truncated and the
true drill position could be as much as a half mil different than the design.
For this reason I wish allegro had a via grid sometimes! If you use IPC
standard manufacturing tolerance you can probably take the laminate anywhere
that can build to IPC standards, which is pretty much most of them. I would
check with the fab vendor 1st. Many shops can do better than the IPC standard
tolerances which will give you more space but the down side of that is you may
be lock into that vendor.
-----Original Message-----
From: chris.ball@xxxxxxxxx [mailto:chris.ball@xxxxxxxxx]
Sent: Friday, April 01, 2005 10:10 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Removing unused pad rings on inner layers
DURING design...
Both good points.
Carl is stressing the fact that DRILL size is not the same as FINISHED HOLE
SIZE (after plating). For internal layers, you need to focus on drill size.
If you specify a 10mil finished hole size on the via, then make sure your
internal pad is upsized to the actual drilled hole.
You might get by without worrying about adding std. mfg. tol. Depends. If
you have a min clearance for higher voltage potential, then you'd want to
add it in. If your electrical spacing requirements can live with min
spacing minus mfg.tol., then you're OK (I think).
-Chris
"Austin Franklin"
<austin@xxxxxxxxxxxx> @ To:
<icu-pcb-forum@xxxxxxxxxxxxx>
VALSMTP cc:
Sent by: @VALSMTP Subject:
[PCB_FORUM] Re: Removing unused
pad rings on inner
layers DURING design...
04/01/2005 09:48 AM
Please respond to
icu-pcb-forum
Hi Carl,
> I'm sure most of you are aware of this but when you talk about
> making a pad size the size of the drill you need to consider that
> pad size as the actual drill bit size not finished drill + the
> standard manufacturing tolerances. Then you would apply that
> minimum clearance to that pad shape.
I think you want to increase the "pad" size larger than the drill size by
that "standard manufacturing tolerance" (for me, that would be 10 mils plus
3 mils) so that you can use the default trace to via clearance. If you
make
the pad the size of the drill, then you have to increase the trace to via
clearance to include this "standard manufacturing tolerance", which would
then apply to every trace to via, not just the ones with the pads
"removed".
I agree, that making a via with no "regular" internal pads, and then
running
a skill script to add the "regular" pads to places where connections were
made is a great idea, and would make this issue really easy to solve.
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum
or go to //www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
"This e-mail message is intended only for the use of the intended
recipient(s).
The information contained therein may be confidential or privileged, and
its disclosure or reproduction is strictly prohibited.
If you are not the intended recipient, please return it immediately to its
sender at the above address and destroy it."
-----------------------------------------------------------
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum
or go to //www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
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 please login at
//www.freelists.org. Our list name is icu-pcb-forum
or go to //www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
Want to post a job listing ? DON'T DO IT HERE!
Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx
POST: icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
Other related posts:
