Bob,
        I am beginning to understand your issues. But most of them are not
bugs. See my comments interspersed below. Somewhere in my comments I might
stumble on a little gotcha because I haven't tried to mimic this whole
process exactly as you describe. Maybe a small detail or two might do
something that I wouldn't expect and didn't know.

Sincerely,
Brad Velander.

Lead PCB Designer
Norsat International Inc.
Microwave Products
Tel   (604) 292-9089 (direct line)
Fax  (604) 292-9010
email: [EMAIL PROTECTED]
http://www.norsat.com

Check out our fall promotion at www.norsat.com. Limited quantities. Sale
ends December 24, 2002.
Contact your Account Manager or call 1-800-NII-4LNB or email
[EMAIL PROTECTED]



> -----Original Message-----
> From: Robert M. Wolfe [mailto:[EMAIL PROTECTED]]
> Sent: Tuesday, December 03, 2002 1:29 PM
> To: Protel EDA Forum
> Subject: Re: [PEDA] 10 best options I want
> 
> 
> Brad,
> Well, it may come down to how Protel
> actually defines "Update Footprint"
> IMHO that verbage should mean update
> the footprint to what is currently in the library
> for that footprint. I guess Protel's definition of
> this is change the footprint on the pcb to what
> the schematic symbol calls out for, and don't
> pay any attention to the fact that there may be 2 or
> more alternates that could be used.
> (I could be wrong but I think I've seen do some
> updates but not all, not really sure though) had to go
> and do all footprints I know changed indivually
> from the libray side.

        I assume that your comment "Update Footprint" means that you are
using the synchronizer to update 'schematic' changes to your PCB. Yes I
understand that this function will not necessarily update every footprint to
the current version that is in the PCB footprint library. This is an old
gottcha with many CAD packages. It will update the footprint to the latest
library defined footprint typically only if this footprint is not previously
used in the existing PCB or if you have defined a new name for the
footprint. If it was used in the existing PCB then there is a copy of that
footprint in the PCB footprint cache and the cache version is typically
used. The only way to update a changed footprint in the PCB is from the
library update PCB function on all parts that changed.
        The "Update Footprint" that you refer to is to update the footprint
in the PCB if it is different than the one defined as the desired footprint
(displayed in the field, not unselected in the display list) in the
schematic symbol. There is no check to determine if it is in any way
different from one in the footprint library if it was revised.

> 
> Well, basically in th eprocess of using synchronize function to
> update your design you can check update footprints,
> first off it will not update all of the footprints at once
> with changes made in library footprints (unless I totally
> misunderstand what update means by Protel see above) but what it
> does do is change all footprints to the ones specified in
> their symbol. i.e. the one shown as first in pulldown of
> list of footprints if there are more than one. The system is not
> intelligent enough to know there are more than one legal
> footprint for a part.

        Has nothing to do with intelligence, it has to do with which one is
displayed in the footprint field window. Has nothing to do with any that are
in the list unless they are the 'one' that is displayed in the field. The
order in which they display in the list has nothing to do with this either.

> 
> Yes you can change the footprint in the PCB and
> backannotate to schematic so this new footprint will
> be first and then there after used. But I heard many times
> on this forum backannotate was not a good thing
> always drive it forward from schematic. Which
> then would mean one has to go back to schematic
> to make change them re-sync every time.

        Yes you are correct, back annotating in any CAD package has it's
limitations and possible pitfalls. As a 'general' rule one should forward
annotate. But this does not have anything to do with the above points. It is
no solution for the update problem because again if the footprint was used
in the PCB you will get the same footprint from the cache as you already
had. If you use a new footprint then the latest version from the library
would be used if you forward annotate the change from the schematic.

> 
> But it seems to me  that it would be alot easier if you can 
> define up front
> in your library (one time) what possible footprints can
> be used by a particular symbol/part and once done
> there could be a pulldown list on BOTH schematic AND
> PCB to choose a footprint from an alternate list. Then
> the system should be intelligent enough to know
> if a footprint on the PCB is on list in symbol keep it on the board.
> Also if there were a way to actually update ALL the footprints
> in a design to latest in library in one shot, with the 
> ability to control
> it somewhat just like update list of changes from design iterations
> in synchronize.

        I really don't understand this comment for it's reference to
footprints and a pulldown list in PCB. Within the PCB a 0603 footprint could
be used for a resistor, capacitor, inductor, (probably also a few more that
don't come to mind right now) then if you cross this to all of the possible
alternate footprints for these types of 0603s your cross-references could go
on forever. This would open up a can of worms that one could never close.

        In the PCB library you have defined a footprint, what alternate
footprints for a singular footprint do you want? One footprint is one
footprint for a specific physical device for certain manufacturing
conditions, there is no alternate without changing conditions, it is a
singular device.
 
        If the footprint is in the footprint field in the schematic then it
will be either left on the board or put onto the board. Period, no if and or
buts about it. Do you think it randomly picks a footprint and substitutes
it? It will be the latest version from the library if the part was not
previously on the board. If an older variety were on the board then the
older variety will be put on the board because of the footprint within the
PCB cache memory. If you want to revise a footprint to the newer library
version then you must use the "Update PCB" function from within that part
occurrence in the library while the target PCB file is open. However, that
will update every device of the same name on the PCB. If you wanted to only
update one of the devices then you must have a footprint with a unique name,
otherwise how would even you know which footprint was which? This is one of
the golden rules of CAD library management.  Library management is not
simple, it is not easy, this is what trips up more designers than most any
other aspect when they start out.

> 
> So what your saying is if you change a footprint on the fly
> in the PCB and do not change the schematic symbol to reflect that
> footprint, or do not run a backannoptate to change that footprint
> in symbol, the next time you run sync with update footprint checked
> it keeps footprint changed in board??????

        No it would insert whatever footprint was listed for that device in
the footprint field. If you have "update Footprints" checked when you ran
the synchronizer. My example was based upon experience of how this package
and most all CAD packages (I have used 5 - 6 different packages over the
years) work. CAD packages are typically schematic driven. The change that I
commonly make as described in my example was to the footprint field in the
schematic, thereafter the footprint never changes no matter how many times I
update, unless I change the footprint in the schematic footprint field
again. If I changed the footprint in the PCB manually then I am responsible
for getting that change back into the schematic correctly, if I don't it is
my mistake.

> 
> Exactly what is that "footprint update" function supposed to do?

        Change the footprint in your PCB to the footprint defined in your
schematic footprint field for that part occurrence. Note: that is not any
footprint in the drop-down list but the one that is defined when you look at
the part properties without clicking on the footprint drop-down list button.
 
> Sorry to be a little long winded, I hope I spelled it out OK.
> Bob Wolfe.

        Glad you were so long winded otherwise I probably wouldn't have
understood what exactly you were trying to do or expecting. I hope that my
comments have shed some light on your problems, seems that your expectations
are out of line with reality. Imagine how screwed up things could get if you
were making changes at both ends and then synchronizing things both ways.
Having checked the schematic you update the PCB. Make some modifications to
the PCB and then back annotate to the schematic, now your schematic is
unchecked, unverified. And vice versa. Typically you should consider your
schematic as the driving document and you will seldom go wrong. If you
modify a library part you can't expect the system to know when and where you
want that revision applied and in which project. Thus it is acting to
protect the integrity of existing designs by not updating the revised
footprint uncontrollably where it was already used. It does make it a bit of
a pain to change it when you do want it changed but that is better than the
CAD system changing everything without your knowledge.


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to