[PCB_FORUM] Re: Removing unused pad rings on inner layers DURING design...
- From: "Austin Franklin" <austin@xxxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Thu, 31 Mar 2005 19:45:44 -0500
Hi Michael,
> What size anti-pad are you using for your vias ? (Hole size + ?)
On planes that don't get connected to, they are the size of the via (24)
with a 10 mil drill in the center, so the drill to copper clearance is 7.
On planes that do get connected, there are thermals that are 24 mils in
size, and are "spoked" to the drill hole.
Here's the arithmetic for my current case:
39.37 - (4 + 4.5 + 4) - 24 = 2.87/2 = 1.43...so the plane is always 1.43
mils outside the differential pair trace. So, it has, in the case of
4/4.5/4, full coverage. Trace to drill clearance is 39.37 - (4 + 4.5 + 4) -
10 drill - 3 drill oversize /2 = 6.93 mil trace to drill clearance.
Obviously, if you need wider trace/gap, you can end up not being coupled to
the plane for the entire width of the trace for that short arc of a circle.
I'm not sure how much of an issue, if any, this might be given how short a
distance this is. It depends on how much the coupling area is reduced...and
if I run into a situation when I need to do this, I'll simulate it and see
what, if any, problems it shows.
> In one of your previous responses you indicated that you will still
> have a plane reference when routing thru the suppressed pad area
> so I wanted to know how you are accomplishing this.
No problem.
> BTW: I think it would be a cool option to suppress the via pads
> so you are able to route more traces thru between vias but I
> don't know if I would really use it.
It works very very well, it allows me to route two 4/4.5/4 differential
traces (which works for .062 10/12 layer stack-ups just fine) from the
middle of a BGA out while maintaining full differential coupling...and to be
able to route differential traces THROUGH a BGA via field and maintain the
differential coupling as well. It allows dispersion on less layers. I
haven't found any downsides to it yet. Except getting the tool to do it
that is.
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
-----------------------------------------------------------
Other related posts:
