[PCB_FORUM] Re: How do I include .dra file that contains my board outline in a DxD schematic?

Hi,

I dumped the libraries from an existing design with an instance of mechanical 
component (Board outline symbol).
The device file came out like this:

*************************************************
(DEVICE FILE: BOARD-BOARD-1_1057-2_TVJ119233A)

PACKAGE '1_1057-2_TVJ1192331_D'
CLASS MECHANICAL
PINCOUNT 0

PINORDER 'BOARD-BOARD-1_1057-2_TVJ119233A'
FUNCTION 'TS-1' 'BOARD-BOARD-1_1057-2_TVJ119233A'

PACKAGEPROP PARENT_PART_TYPE BOARD
PACKAGEPROP PARENT_PPT BOARD
PACKAGEPROP PARENT_PPT_PART 'BOARD-BOARD'
PACKAGEPROP PART_NAME BOARD
PACKAGEPROP PART_NUMBER TVJ123456
PACKAGEPROP SCH_MODIFIED_PART TRUE

END 
**************************************************

Jan Blückert
Ericsson AB
Kista, Sweden



-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx 
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Austin Franklin
Sent: den 30 april 2009 14:28
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: How do I include .dra file that contains my board 
outline in a DxD schematic?

Hi,

Does anyone have a device file the can send me that references a .bsm (either a 
fiducial, or a npth, something with no pins on it)?  Then, I could see what it 
is I need to get out of DxD to be able to do this.

Regards,

Austin

> -----Original Message-----
> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of JCharles 
> TEYSSIER
> Sent: Thursday, April 30, 2009 8:22 AM
> To: icu-pcb-forum@xxxxxxxxxxxxx
> Subject: [PCB_FORUM] Re: How do I include .dra file that contains my 
> board outline in a DxD schematic?
>
>
> Group,
>
> i remember we have do tha in the past:
> Define a package symbol, so you can add a reference designator. Do not 
> put any pin.
> In setup, declare the symbol as mechanical: the reference designator 
> is still here (but can not be directly defined in mecanichal symbol)
>
> Use it with capture in front end... works well
>
> Jean-Charles
>
> Dave Schaefer a écrit :
> > A comment on Mechanical parts ...
> >
> > They are well defined within Allegro and the Cadence tools, but many 
> > downstream 3rd party translators (manufacturing, ICT, etc.)
> don't support
> > them and having them in the design will result in corrupt data
> (I've seen
> > this with both Fabmaster and Circuitcam).
> >
> > I define any true "mechanical" parts that are added via
> schematic/netlist as
> > "package" symbols with a small pin as Jeff suggested.
> >
> > Hth,
> >
> > Dave Schaefer
> > dave.schaefer@xxxxxxx
> >
> >
> > -----Original Message-----
> > From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> > [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Austin 
> > Franklin
> > Sent: Wednesday, April 29, 2009 7:45 PM
> > To: icu-pcb-forum@xxxxxxxxxxxxx
> > Subject: [PCB_FORUM] Re: How do I include .dra file that
> contains my board
> > outline in a DxD schematic?
> >
> > Hi Jeff,
> >
> > I don't know.  It would now be an electrical item, instead of a
> mechanical
> > item.  That may cause an issue.  I should be able to do this
> without that.
> > People add non-electrical mounting holes to their schematics
> all the time,
> > and this should be the same thing.
> >
> > Best Regards,
> >
> > Austin
> >
> >
> >> -----Original Message-----
> >> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> >> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of Jeff 
> >> Schmitt
> >> Sent: Wednesday, April 29, 2009 8:38 PM
> >> To: icu-pcb-forum@xxxxxxxxxxxxx
> >> Subject: [PCB_FORUM] Re: How do I include .dra file that contains 
> >> my board outline in a DxD schematic?
> >>
> >>
> >> Hi Austin,
> >>
> >> I haven't followed this thread closely...but if the only error
> is that it
> >> has no pin, what's the harm in adding 1 small (virtually
> invisible) pin on
> >> the symbol somewhere?
> >>
> >> Jeff
> >>
> >> -----Original Message-----
> >> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> >> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
> Austin Franklin
> >> Sent: Wednesday, April 29, 2009 7:44 AM
> >> To: icu-pcb-forum@xxxxxxxxxxxxx
> >> Subject: [PCB_FORUM] Re: How do I include .dra file that
> contains my board
> >> outline in a DxD schematic?
> >>
> >> Hi Nagaraj,
> >>
> >> My schematic symbol (and dra) have REFDES.  It's the pins that it's 
> >> complaining about.  When reading it in when I do an import, Allegro 
> >> doesn't like that it has no pins.
> >>
> >> So, yes, it would be just like mounting holes that have no 
> >> electrical connection.  Anyone do that with DxD?
> >>
> >> Best Regards,
> >>
> >> Austin
> >>
> >>
> >>> -----Original Message-----
> >>> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> >>> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of Shanmugam, 
> >>> Nagaraj
> >>> Sent: Wednesday, April 29, 2009 7:34 AM
> >>> To: icu-pcb-forum@xxxxxxxxxxxxx
> >>> Subject: [PCB_FORUM] Re: How do I include .dra file that contains 
> >>> my board outline in a DxD schematic?
> >>>
> >>>
> >>> Austin,
> >>>
> >>> The third party syntax  $PACKAGES for components needs to
> have a refdes.
> >>> Example : 'RS0402_01A' ! RJX0087400 ! 332 ! '1%' ; R390 R391
> >>>
> >>> If you need to automate the process then you need to have a refdes 
> >>> defined and created as *.dra symbol. For example like NPTH 
> >>> mounting hole.
> >>>
> >>> Hope this helps
> >>>
> >>> Nagaraj Shanmugam | Lead Designer - PCB Development 
> >>> nshanmug@xxxxxxxxx
> >>>
> >>>
> >>>
> >>> -----Original Message-----
> >>> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> >>> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
> Austin Franklin
> >>> Sent: Monday, April 27, 2009 5:46 PM
> >>> To: icu-pcb-forum@xxxxxxxxxxxxx
> >>> Subject: [PCB_FORUM] Re: How do I include .dra file that contains 
> >>> my board outline in a DxD schematic?
> >>>
> >>> Hi Jan,
> >>>
> >>>
> >>>> Not sure about DxD, but with Concept (or Allegro Design Entry
> >>>> HDL) as the schematic capture tool, non-electrical components 
> >>>> works well and we use this in every design.
> >>>> (We handle the board outline as a non-electrical component, along 
> >>>> with other stuff of nonelectrical/mechanical nature).
> >>>>
> >>> Exactly what I want to do using DxD...
> >>>
> >>>
> >>>> You have to generate non-electrical symbols as .bsm's on the 
> >>>> Allegro PCB Layout side.
> >>>>
> >>> Already done.  I can place it manually, so I know that part works.
> >>>
> >>> 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 go to 
> >>> http://www.freelists.org/archives/icu-pcb-forum/
> >>>
> >>> Problems or Questions:
> >>> Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
> >>> -----------------------------------------------------------
> >>>
> >>> -----------------------------------------------------------
> >>> 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 go to
> >>>
> >> http://www.freelists.org/archives/icu-pcb-forum/
> >>
> >> Problems or Questions:
> >> Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
> >> -----------------------------------------------------------
> >>
> >> -----------------------------------------------------------
> >> 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 go to 
> >> http://www.freelists.org/archives/icu-pcb-forum/
> >>
> >> Problems or Questions:
> >> Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
> >> -----------------------------------------------------------
> >>
> >>
> >> -----------------------------------------------------------
> >> 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 go to 
> >> http://www.freelists.org/archives/icu-pcb-forum/
> >>
> >> Problems or Questions:
> >> Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
> >> -----------------------------------------------------------
> >>
> >>
> >
> > -----------------------------------------------------------
> > 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 go to 
> > http://www.freelists.org/archives/icu-pcb-forum/
> >
> > Problems or Questions:
> > Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
> > -----------------------------------------------------------
> >
> > -----------------------------------------------------------
> > 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 go to
> http://www.freelists.org/archives/icu-pcb-forum/
> >
> > Problems or Questions:
> > Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
> > -----------------------------------------------------------
> >
> >
> >
> -----------------------------------------------------------
> 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 go to 
> http://www.freelists.org/archives/icu-pcb-forum/
>
> Problems or Questions:
> Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
> -----------------------------------------------------------

-----------------------------------------------------------
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 go to 
http://www.freelists.org/archives/icu-pcb-forum/

Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
-----------------------------------------------------------
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 go to 
http://www.freelists.org/archives/icu-pcb-forum/

Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------

Other related posts: