[PCB_FORUM] Re: Intelligent Dual Footprints 15.x

  • From: "Feehan, Stephen" <stephen.feehan@xxxxxxxxxxx>
  • To: "'icu-pcb-forum@xxxxxxxxxxxxx'" <icu-pcb-forum@xxxxxxxxxxxxx>
  • Date: Wed, 29 Sep 2004 12:31:40 -0700

Jack,
We have a separate schematic page with the ref des's named U1, R1, C1. 
Then we have a custom script that renames the block into 3 multiple blocks
and outputs three was/is text files to import into allegro.  Then the sheets
of the
blocks are copied into the main hierarchy schematic.
 
This is the batch file:
reftxt dx270_blk_a_a.txt dx270.brd dx270_A.brd
reftxt dx270_blk_b_b.txt dx270.brd dx270_b.brd
reftxt dx270_blk_c_c.txt dx270.brd dx270_c.brd
 
After I run this script I have 3 board files with the new ref des's.  I then
create 3
separate clip files and import them on the board.
 
Hope this helps,
 
Thanks,
Stephen
SIEMENS ICN

-----Original Message-----
From: JACK KELLY [mailto:jack.kelly@xxxxxxxxxx]
Sent: Wednesday, September 29, 2004 2:20 PM
To: 'icu-pcb-forum@xxxxxxxxxxxxx'
Subject: [PCB_FORUM] Re: Intelligent Dual Footprints 15.x


Stephen,
i wish you could go into a little more detail on the clip file process.  how
was your schematic setup,how was those three bga circuits numbered?
can you give more detail on the batch file you ran?  i am just trying to
find out if there is a better to do this than the way we do it.

-----Original Message-----
From: Feehan, Stephen [mailto:stephen.feehan@xxxxxxxxxxx]
Sent: Wednesday, September 29, 2004 12:33 PM
To: 'icu-pcb-forum@xxxxxxxxxxxxx'
Subject: [PCB_FORUM] Re: Intelligent Dual Footprints 15.x


Modules will also work, however they are treated like footprints so if you
change one they all change on the board.  Using clip files is the most
efficient
way in my experience because it gives you flexibility to change one group on
the
board level if needed.
 
I just used it today on three 788pin Bga's (Switches) with about 300
components
and most of them differential signals.  I place one group, ran a batch file
to
rename the other 2, created clip files then placed them on the board.
 
Stephen
SIEMENS ICN
 

-----Original Message-----
From: design1955@xxxxxxxxxxx [mailto:design1955@xxxxxxxxxxx]
Sent: Wednesday, September 29, 2004 1:08 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Intelligent Dual Footprints 15.x


Am I hearing that the clip command may be the easiest way to do this? Or is
there a way to pull all the symbols in at one time with ref des assigned to
each individule component? I have done the clip several times but seems to
me there should be an easier way to do this. I just can't find any info on
Modules and 3rd party tools. 

This is also something I want to do with power supplies. Design for re-use.

Thanks

Steve

 

-------------- Original message -------------- 

> I have used modules several times, but only when using the Concept HDL 
> front end. Modules work great for placing a common circuit on several 
> different boards and the upper-level schematic symbol just displays the 
> interface signals to that circuitry. Each footprint that is place on the 
> board within the module will have a unique reference designator which 
> you can designate. Such as M1_R1, M1_C1, ets... Module two would have 
> M2_R1, M2_C1, etc.... 
> But like I said, I've only performed this using Concept HDL into Allegro 
> Performance. Email me directly if you require further assistance. 
> Good luck. 
> 
> Jim S. Wages / SR. PCB Layout Designer: 
> (919) 484-2963 
> 
> -----Original Message----- 
> From: Kevin McCowan [mailto :kmccowan@xxxxxxxxxxxxxx] 
> Sent: Wednesday, September 29, 2004 11:44 AM 
> To: icu-pcb-forum@xxxxxxxxxxxxx 
> Subject: [PCB_FORUM] Re: Intelligent Dual Footprints 15.x 
> 
> This is the point I am trying to make. A module is just like a small 
> circuit board, if I am not mistaken. You still have the individual 
> components so your placement file would show each one. Once you 
> import it it acts like you placed and routed each component as 
> you normally would. 
> It is not a "symbol" per se. It is a subassembly. 
> 
> Kevin 
> 
> gnieski, mike wrote: 
> > Isnt another issue on the assembly end? If you have one symbol 
> representing 
> > a bundle of parts 
> > How can you export the pick and place data to be used at assembly? 
> Centroid 
> > data usually comes 
> > From the place bound of each part or by adding body center. Just 
> another 
> > thing to think about. 
> > 
> > Thanks, 
> > Mike 
> > 
> > 
> > -----Original Message----- 
> > From: Kevin McCowan [mailto:kmccowan@xxxxxxxxxxxxxx] 
> > Sent: Wednesday, September 29, 2004 11:45 AM 
> > To: icu-pcb-forum@xxxxxxxxxxxxx 
> > Subject: [PCB_FORUM] Re: Intelligent Dual Footprints 15.x 
> > 
> > 
> > But that makes no sense. 
> > If you have the footprint right why cannot you assign a refdes to the 
> > allegro symbol? Why should allegro care what tool the netlist came 
> from once 
> > it is imported? It would be like placing a spare component and then 
> once the 
> > netlist is in assigning the refdes. I could be wrong, but still, it 
> does not 
> > add up to me. 
> > 
> > Somebody try it, please and let us know. 
> > 
&g t; > Thanks, 
> > Kevin McCowan 
> > Sr. PCB Designer 
> > TSI Telsys 
> > 
> > Jean Bratton wrote: 
> > 
> >>Yes it is, but it only works with Concept and Capture. 
> >> 
> >> 
> >> 
> >>---------------------------------------------------------------------- 
> >>-- 
> >> 
> >>*From:* george.h.patrick@xxxxxxxxxxxxxx 
> >>[mailto:george.h.patrick@xxxxxxxxxxxxxx] 
> >>*Sent:* Wednesday, September 29, 2004 11:33 AM 
> >>*To:* icu-pcb-forum@xxxxxxxxxxxxx 
> >>*Subject:* [PCB_FORUM] Re: Intelligent Dual Footprints 15.x 
> >> 
> >> 
> >> 
> >> 
> >> 
> >>This is a perfect use for a module. 
> >> 
> >> 
> >> 
> >>I don't know if you can do this without Concept-HDL, t hough. 
> >> 
> >> 
> >> 
> >>-- 
> >>/George Patrick/ 
> >>*Tektronix, Inc.* 
> >>Central Engineering, PCB Design Group 
> >>P.O. Box 500, M/S 39-512 
> >>Beaverton, OR 97077-0001 
> >>Phone: 503-627-5272 Fax: 503-627-5587 
> >>http://www.tektronix.com 
> >>http://www.pcb-designer.com 
> >> 
> >>/It's *_my_* opinion, not Tektronix'/ 
> >> 
> >> -----Original Message----- 
> >> *From:* Design1955@xxxxxxxxxxx [mailto:design1955@xxxxxxxxxxx] 
> >> *Sent:* Tuesday, September 28, 2004 17:23 
> >> *To:* icu-pcb-forum@xxxxxxxxxxxxx 
> >> *Subject:* [PCB_FORUM] Intelligent Dual Footprints 15.x 
> >> 
> >> I have been asked to create a footprint containing the followi ng 
> >> information: 
> >> 
> >> A bga containing all of it's fan-out recommended by the spec. 
> >> 
> >> all of it's supporting decoupling caps, connected per the EE's 
> >>rules. 
> >> 
> >> So every time I place this component it will have the particular 
> BGA 
> >> and the supporting caps placed and also routed to the power and 
> >> ground pins per the schematic. 
> >> 
> >> I am using 15.2 and VueLogic front end. 
> >> 
> >> Does anyone know if there is a way to make this work as a complete 
> >> intelligent footprint you placing it as a block of components with 
> >> routing? 
> >> 
> >> Thanks 
> >> 
> >> Steve 
> >> 
> >> 
> >> 
> > 
> > ------------------------------- ---------------------------- 
> > 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 
> > ----------------------------------------------------------- 
> ----------------------------------------------------------- 
> To subscribe/unsubscribe: 
> Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx 
> with a subject of subscribe or uns ubscribe 
> 
> 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 http:// 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: