[PCB_FORUM] Re: How to connect Two thru-hole pads that are placed same location.

Great suggestion Michael,
Thanks, We'll give it a try.

Mark

Michael Catrambone wrote:


Mark,
One more suggestion, which it looks like you got a lot already, is to define a round static shape inside the pad boundary associated to the net name of the pins and the rat will go away / 100% routed. You could add these static shapes to the connector symbol and after being placed the shapes will automatically associate to net of the pin it is on top of. Of course if the net names on the pins change during an ECO then the shape will not change along with them but you could delete the symbol and replace it again. It's a workaround but it does the job. 

Hope this helps,
Michael Catrambone
UTStarcom, Inc.

------------------------------------------------------------------------
*From:* icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] *On Behalf Of *Mark Salberg 
*Sent:* Wednesday, August 27, 2008 11:55 AM
*To:* icu-pcb-forum@xxxxxxxxxxxxx
*Subject:* [PCB_FORUM] Re: How to connect Two thru-hole pads that are placed same location. 


Thanks for all the suggestions.
We will try a few suggestions after completing the design.
As of now, we removed nets from second schematic symbol...thus removing second set of rats. Placed both connectors on each other as before. Then waived DRC's. Both connectors still get passed to the BOM except if one is set as a no-pop. (BOM_IGNORE). 

Mark



Les Wong wrote:

Mark:

Here is what we do:
1. one padstack is thru hole pin, lets say for the top connector
2. one padstack is smt, for the bottom connector
3. you can create a physical region around the connectors
4. you will need to go into constraint manager and change the Allow-> Pad-Pad Connect 
to ALL_ALLOWED for each net on the connector

Les
--- On *Wed, 8/27/08, Dave Seymour /<dseymour@xxxxxxxxxxx> <mailto:dseymour@xxxxxxxxxxx>/* wrote: 

From: Dave Seymour <dseymour@xxxxxxxxxxx> <mailto:dseymour@xxxxxxxxxxx>
Subject: [PCB_FORUM] Re: How to connect Two thru-hole pads that are placed same location. 
To: icu-pcb-forum@xxxxxxxxxxxxx <mailto:icu-pcb-forum@xxxxxxxxxxxxx>
Date: Wednesday, August 27, 2008, 8:02 AM

That's fine.


So, you need a work around in Allegro to get rid of the ratsnest lines.
Make sure you leave "stretch etch" box checked when you move the connector back into position. 


Which was the original idea below:


Mark,


I never have done this, but it seems like it might work.
Move one of the connectors off board and make the connections, then move the connector back into position. 


If I had to guess, Allegro will keep the connection.


Just an idea, Hope this helps.


Dave Seymour

Ixia

919.267.4840

------------------------------------------------------------------------
*From:* icu-pcb-forum-bounce@xxxxxxxxxxxxx <mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] *On Behalf Of *Mark Salberg 
*Sent:* Wednesday, August 27, 2008 10:58 AM
*To:* icu-pcb-forum@xxxxxxxxxxxxx <mailto:icu-pcb-forum@xxxxxxxxxxxxx>
*Subject:* [PCB_FORUM] Re: How to connect Two thru-hole pads that are placed same location.
Our schematic feeds the BOM. Must have both in the schematic for different populations. 


Dave Seymour wrote:
Well, one could make a special padstack and remove the drill, just like an SMT pad and waive the DRCs.
IMHO - The best way to would to let the BOM control which connector is populated and only have one connector on the schematic.
In some backplane applications, the pins are really short and the primary side connector and the secondary side connector share the same hole.
On this type of backplane we have the BOM control the connector and the schematic shows only one connector, even though both connectors (top, bottom) are populated. 


D


Dave Seymour

Ixia

919.267.4840

------------------------------------------------------------------------
*From:* icu-pcb-forum-bounce@xxxxxxxxxxxxx <mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] *On Behalf Of *Gerry Meier 
*Sent:* Wednesday, August 27, 2008 10:34 AM
*To:* icu-pcb-forum@xxxxxxxxxxxxx <mailto:icu-pcb-forum@xxxxxxxxxxxxx>
*Subject:* [PCB_FORUM] Re: How to connect Two thru-hole pads that are placed same location. 


What is that doing to do to your "Drill file" Double drills??


Gerry Meier, Sr. PCB Designer

Freedom CAD Services. Inc

Voice: (256)776-7470 or (603) 864-1350

Email:gerry.meier@xxxxxxxxxxxxxx <mailto:Email:gerry.meier@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:* Wednesday, August 27, 2008 9:32 AM
*To:* icu-pcb-forum@xxxxxxxxxxxxx <mailto:icu-pcb-forum@xxxxxxxxxxxxx>
*Subject:* [PCB_FORUM] Re: How to connect Two thru-hole pads that are placed same location. 


Mark,


I never have done this, but it seems like it might work.
Move one of the connectors off board and make the connections, then move the connector back into position. 


If I had to guess, Allegro will keep the connection.


Just an idea, Hope this helps.


Dave Seymour

Ixia

919.267.4840

------------------------------------------------------------------------
*From:* icu-pcb-forum-bounce@xxxxxxxxxxxxx <mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] *On Behalf Of *Mark Salberg 
*Sent:* Wednesday, August 27, 2008 10:11 AM
*To:* icu-pcb-forum@xxxxxxxxxxxxx <mailto:icu-pcb-forum@xxxxxxxxxxxxx>
*Subject:* [PCB_FORUM] How to connect Two thru-hole pads that are placed same location.
We have two thru-hole connectors placed on top of one another. One populated, one not. 
PROBLEM: We can not get rid of rats, because two pins / pads at same X:Y.

*Any ideas how to get connection to both pads?*
We decided to remove net names from one of the connectors in the schematic, to allow us to connect to one pad on board. Then waive DRC's. 
We are using V.15.7 and Concept front end.

Regards,
Mark
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. 


_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com 
_____________________________________________________________________________


_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com 
_____________________________________________________________________________


_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com 
_____________________________________________________________________________


_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com 
_____________________________________________________________________________


_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For more information please visit http://www.ers.ibm.com 
_____________________________________________________________________________



_____________________________________________________________________________
Scanned by IBM Email Security Management Services powered by MessageLabs. For 
more information please visit http://www.ers.ibm.com
_____________________________________________________________________________

Other related posts: