[PCB_FORUM] Re: Soft to hard location (Concept v.15.1)
- From: "Dave Mattice" <DMattice@xxxxxxxxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Mon, 13 Jun 2005 10:58:23 -0700
Have experienced similar problems also. We use Orcad (Ver 10)
As our schematic capture to Allegro Expert(Ver 15.2).
Here is the latest example that just happened to me.
We have a row of connectors that use a metal shielding
Cage. The metal cage has compliant or press fit pins
That attach to the pcb. We recently changed several
Of the pins from "MECHANICAL" to "CONNECT". Pin locations
Didn't change and the symbol name didn't change.
The connector symbols were replaced in the schematic and a new netlist
Created. The designators were preserved.
In Allegro, I import Logic with Place Changed Component ALWAYS selected.
By the way, The connectors have a hard location property assigned.
When the new netlist is read in, the connectors as you say, "Get blown off the
board".
I tried refreshing the connectors before logic import but get an error because
of the pin
Number mismatch because we changed some mechanical pins to connect pins.
Catch 22.
My opinion is, Selecting the "Changed Component ALWAYS" should replace the
connectors.
I think Allegro has worked this way for some time. I don't agree with it and
wish this would
Be fixed. I'll fill out another service request when I have time later this
afternoon. I just
Wanted to add my to cents worth.
Incidentally, My quick little work around was to export a placement before
importing the logic.
Then importing the placement after the netlist was read in. Worked fine. So my
humble conclusion
Is the placement should not have been removed.
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
Sent: Monday, June 13, 2005 9:57 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Soft to hard location (Concept v.15.1)
Thanks for all of your responses.
From being paranoid of parts getting blown off the board we have always
hard located all "defined designators" parts in the schematic.
And any new parts we would leave "?" to let the system assign the next
available.
We also use "repackage" which may have been the problem for a few in the
past. (For any soft located parts).
We assign a hard located ref des to multi-section / multi-gate parts. Do
you do this...or use the GROUP property?
Then back annotate to update "?" in the schematic.
Then finally hard locate all.
Judging from your responses, we are in the minority.
So let me summarize:
If we select "PRESERVE" while packaging, existing "soft located"
designators will remain and all "?" locations will be assigned new ref des.
What about multi sectioned parts?
We are still able to renumber ref des in Allegro if we want to. Usually
only on a rev. A / new design.
We do not do this on a revision, because ALL parts would be renumbered.
This is discouraged by the Bill of material police. They want to track
changes from one rev to the next.
Also, as mentioned below by Juan, this can be accomplished by global
update now.
Thanks again for all of your feedback.
Mark
Munoz, Juan wrote:
>Mark,
>
>Yes, there is an easier way.
>
>In the Concept toolbar, go to: Tools -> Global Update -> Global Property
>Change.
>
>After a few seconds, a Global Modification dialogue box will pop up. The
>default tab should be the "Property Change" tab. There are some fill in boxes
>(2 rows and 2 columns).
>
>In the first row type in the property you wish to change. In your case, it
>would be: $LOCATION. For the value, use a wildcard ( * ).
>
>In the second row, type in the new property name: LOCATION. For the value,
>click on the drop down arrow and select: ++Preserve Source Value++
>
>Click on the radio button to select how you want the changes applied (Design,
>Sheet, Page range, etc.).
>
>Click on the " OK " You will get a warning saying something to the effect that
>you cannot undo changes or something like that. Click on "Continue" and watch
>the status window until its done.
>
>Juan M. Muqoz
>Tyco Electronics Power Systems, Inc.
>CAD Support Group
>phone: 972-284-3019
>e-mail: juan.munoz@xxxxxxxxxxxxxxxxxxx
>-----Original Message-----
>From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
>[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
>Sent: Friday, June 10, 2005 6:15 AM
>To: Cadence User Group
>Subject: [PCB_FORUM] Soft to hard location (Concept v.15.1)
>
>Is there an easier way to hard locate reference designators in Concept?
>When allowing Concept to assign ref des.
>
>We are still doing the old,
>find $LOCATION on each page.
>Change "group" A
>Ctrl E
>find / replace $LOCATION with LOCATION
>save text file
>save schematic page
>
>There should definitely be a better way!
>
>Also, is there a file (prior to packaging to Allegro) that lists all ref
>des used?
>We usually package, then run a component report to see.
>
>Thanks,
>Mark
>
>
>_____________________________________________________________________________
>Scanned by IBM Email Security Management Services powered by MessageLabs. For
>more information please visit http://www.ers.ibm.com
>_____________________________________________________________________________
>-----------------------------------------------------------
>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
>-----------------------------------------------------------
>
>_____________________________________________________________________________
>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
_____________________________________________________________________________
-----------------------------------------------------------
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
-----------------------------------------------------------
Other related posts:
