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

Small question about this issue.

If one of the connectors is NOT STUFFED, why do you need to put a part
number in the BOM? Wouldn't that put two parts

in the BOM when only 1 is really needed?

 

We handle the STUFFED/NOT STUFFED issue in the part.ptf file by having
two line entries.

We have a KEY property of Material and on one line there is info about
the stuffed part,

on the second line there is EMPTY. When the BOM is generated, they flush
out any EMPTY parts so

they are not adding to the parts count.


Shirley 

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: Wednesday, August 27, 2008 11:21 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [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
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] On Behalf Of Mark Salberg
Sent: Wednesday, August 27, 2008 10:58 AM
To: 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] On Behalf Of Gerry Meier
Sent: Wednesday, August 27, 2008 10:34 AM
To: 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

visit us at http://www.freedomcad.com

 

 

________________________________

From: 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
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] On Behalf Of Mark Salberg
Sent: Wednesday, August 27, 2008 10:11 AM
To: 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; 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: