[PCB_FORUM] Re: Dual Plane VIA Connection Question

Good morning to all .... and thanks to all for the great suggestions. I greatly 
appreciate the fast and wonderful help I always get with this forum .... 
further (and in closing) to this discussion .... one credo that I try to follow 
with each hurdle I face with the design tool set is to always try and come up 
with a solution that is as fool proof as possible should another designer pick 
up the design sometime in the future so that he/she does not accidently cause 
errors due to the fact that they were not aware of something. This 
unfortuantely is the byproduct of too many work arounds.
 
Therefore, with this problem, taking suggestions from everyone, I was able to 
come up with a fool proof solution but with a little different twist. Instead 
of using a conventional VIA, due to it's lack of flexability in not being able 
to add individual route keepout too, I have decided to use a conventional PART 
(SYMBOL) using the same size padstack as the via. The negative drawback is that 
each one that I need will have to be added to the schematic, but the major 
upside is that I can add a Route Keepout for a specific layer. (An FYI on this 
- when you first create your symbol, your only choices for adding a Route 
Keepout are Top, Bottom & All. What I did was chose Top and then when I brought 
the part (symbol) into my design, because my design was (8) layers, I was able 
to Change the Route Keepout plane for that part (symbol) from Top to the Inner 
Layer that I needed). We simply call these parts Vitual Pins or Virtual Vias 
and simply turn off (or delete) the reference designation as they are not 
required for visibility on the final assembly.
 
Thanks again to all who provided some great feedback. I hope you all enjoy what 
is left of the weekend.
Vincent Di Lello, CID+

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx on behalf of westfeldt
Sent: Sun 3/12/2006 6:52 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Dual Plane VIA Connection Question


I would create a route keepout on the internal layer, so that automatic plane 
void clears the area around the vias.  I would then have to accept, and perhaps 
note, the drcs that would be caused by the two vias being in the middle of the 
route keepout.
 

Patrick Westfeldt, Jr. 
720-406-0887 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Vince Di Lello
Sent: Saturday, March 11, 2006 3:27 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Dual Plane VIA Connection Question



Here's hoping one of you great designers out there (and Allegro expert) can 
help me out ... in the picture below you will see a light blue external (Top 
Side) 3.3V plane. Inside this board (but not shown) is a separate 3.3V plane. 
What I would like to do is have the (3) vias at the top of the picture (coming 
off the electrolytic cap) make connection with the internal 3.3V plane and then 
connect to the electrolytic cap with traces as shown in the picture. The 3.3V 
then travels down this small external plane coming into contact with some other 
capacitors and ultimately ends at the two vias at the bottom which carry the 
current from the top side of the board to the bottom side of the board where in 
turn there are two traces that connect to two bottom side pads of a bottom side 
connector. Now for my problem - the two vias at the bottom of the light blue 
area are now also connected to the INTERNAL 3.3V master plane (for clarity sake 
I did not turn that plane on). I DO NOT WANT them to connect to the internal 
3.3V plane. I want to force the 3.3V signal to have to travel through the caps 
and then into the connector pads on the external layer only. Is there a setting 
or a property that I can add to those two vias so that they get connected to 
the small external 3.3V copper plane, but NOT to the INTERNAL 3.3V master plane?

 

Any help, especially on a weekend, would be greatly appreciated. Thanks in 
advance and I hope all who are listening will have a great weekend - at least 
what is remaining of it. Thanks again.

 

 

 

 

Vincent Di Lello, CID+

Other related posts: