I haven't read all the other replies so forgive me if I repeat someone
else's fix.  It sounds like you are editing your schematic lib each time to
get the new footprint into the footprint attribute of schematic symbol
"KEY".  You should be able to use the footprint pulldown and select the
alternate footprint.  That done now to get the netlist updated and input to
PCB.  I run the netlist program and CHECK the netlist for the reference
designator and the new footprint requirement.  If it doesn't show up, like
it may not have done in your case, the problem is that your new schematic
lib part was not accepted into the schematic.  I used to think that changing
a sch lib component and clicking "Update Schematic" was enough to get the
new part in.  There is a function in schematic called "Update Parts in
Cache" the needs to be clicked if you are bringing in changed components of
the same name.

Now try your netlist generation.

When importing the new netlist into PCB and with "Delete Components not in
netlist" and Update Footprints" checked you would think that these two
options would refresh the footprint association between a sch component and
it's footprint.  It doesn't always work.  I found that deleteing the old
footprint is more reliable when trying to get PCB to replace it with the new
assignment.

-----Original Message-----
From: Bob Wolfe [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, January 02, 2002 1:04 PM
To: Protel EDA Forum
Subject: [PEDA] Multisheet Problems & Updates etc.


OK Here is the scenario, I ran through this today.
Hopefully I have described it clearly enough.
I am running 99SE, SP6 on WIN98 Second Ed.
Using the Database structure.

Create 3 footprints called KP1, KP2, & KP3 that could be used for this
part in a library,
Create a part for a contact pattern for a keypad in a library.
Part named "KEY"
In that part I have defined KP1, KP2 & KP3 as legal footprints for that
part,
KP1 the 1st on the list then KP2, then KP3.

With the above scenario I have two problems, 1 on the schematic update side
and the other on the PCB update side.

I create a new schematic put these parts on it and connect them up.
Then I annotate.
Then I run update PCB.
Once in the board I see that the footprint that came out on the board
is the first one on the list (KP1) in the part in the library.

Later on at some point I need to change this footprint, I don't want the
same name
because it is physically different but I still want to keep the old
footprint
even though I do not want it used for this part anymore.

So I create the new footprint KP4 and edit the library for the part KEY
to use only KP4 as a footprint, while both databases for board and library
are open.

While editing the part in library I select update schematic.

Save then go in to schematic, hit part properties and guess what the old
footprint, KP1,
is what is listed,
I can then select the arrow pulldown and see there is a choice for KP4 and
once selected it now becomes the only choice for that part. But that means
every unique part needs a global update, that's allot of needless work in my
mind.

Schematic Problem:

Problem here is each unique part needs to be touched separately and then
globally updated
to REALLY change the footprint. Other wise the old footprint will get put on
the board.
And yes you could then change it in the board but why I already supposedly
updated
it in the schematic. Seems like allot of extra useless work.
In my opinion the update schematic function does not work properly, don't
know whether Protel intends it to work this way or if it is a bug.
You might as well not have this update feature if it will not change this
data in the schematic
globally for you automatically.
Now for one or two parts this may not be that much extra work but if your
library structure needs to change drastically this is a major issue.
Especially
in a service bureau environment.

PCB Problem:

Back to the part that calls out 3 footprints that can be used.
"KEY" has all 3 footprints listed as legal footprints, and ALL 3 are in fact
used
on a board.
I go ahead and change the specific ones as needed to KP1, KP2 & KP3 in the
PCB.
Now I realize I have to make some changes to many other parts in the
footprint
library at some point. Which would then logically say that I would want
to update footprints next time I run the synchronizer on this board.
However what happens is ALL of the parts on the board that are "KEY" change
back to KP1, which was the 1st one on the list in the part in the library.
This is not a good thing in my mind.

In my opinion again this does not work properly. If Protel is giving you the
ability
to specify other legal footprints for a part then when you run an update
function
it should not remove those alternate legal footprints, but just update them
to the latest
that is in the library. Again why have this update function and the
ability to define alternate footprints in the part, if it will not leave
alone
a footprint that was defined in that part in the library. Now I suppose you
could
keep track of every footprint you update and do them individually, but why.
The software should do this.
Also people mentioned I could change the footprints on the board side and
back
annotate, however this is a new board there are no footprints in it yet. So
one
would need to have some sort of old footprints there but then again allot of
extra work.

One last statement, this all stems from my need & want to import an Orcad
schematic with
footprints names on the parts that I do not wish to use. Therefore I would
have
thought the update schematic would have worked properly and forced the
footprints
defined in my library to be placed on a new PCB.
The PCB problem is less of an issue because I have just went ahead and made
3 separate parts defining the 3 keypads so it will not rip them up when I
need to
update footprints during synchronization. But it still bugs me that the
alternate
footprints do function as I would expect.

Again not sure if this is a bug still or whether Protel intends it
to work this way.

Hopefully I have defined this issue clear enough for everyone, I really feel
these are two major issues in the way Protel functions with respect to
updates,
both Schematic and PCB.
Even if Protel wanted you not to be able to globally update footprints as a
default
in the schematic there could at least be a few options of how the update
function operates.

Is anyone trying to use Protel in this fashion for update?
If that is the way it is, I can still get the job done, but there really is
way too much extra work involved.

Thanks
Bob
Robert M. Wolfe, C.I.D.
[EMAIL PROTECTED]

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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