On 02:39 PM 4/04/2001 +0100, Coleman, Tim said:
>Hi Folks,
>When using the library editor to modifying the footprint field in the
>component description and then 'updating schematic' the function doesn't
>modify any of the relevant parts in the schematic.
>All the schematic sheets are 'open'.
>What I do notice is in the schematic diagram, the dropdown option in
>footfrint field of the component propertise does have the corrected
>footprint reference and so by selecting each incidence of the part the
>correct footprint reference can be selected. What a pain!!! it will takes
>ages, I though this was a labour saving tool???
>Anyone know any way of sorting this change to work through the schematic

Tim - this is a longish post - it is worth your while, though, to read it 
as your life will become easier.

To do what you want to do will require learning about the single greatest 
feature of Protel - global operations.  I assume all the major CAD packages 
have them but I suspect Protel was an early leader in these.  Global 
Operations take some getting used to but are very powerful.  (An excellent 
way of doing major stuffups like changing all parts to resistors in one go 
- please practice on backed-up files and go carefully until you are quite 
familiar with the global operations. Read the manual - in this case it is 
worthwhile - at least after you have had a play.)

Some explanation of your problem:
Simply changing the footprint in the sch symbol library will not cause an 
update to the footprint in the schematics.  Footprints - like designators 
and part value are variables - they are not stored in the library.  When 
you enter one or more footprints into the symbol in the library editor you 
are simply making those footprints more easily available through the 
footprint combobox.  You are at liberty to enter any footprint you like 
regardless of what the drop list contains.  Would you like the designators 
or part value to update when you made a change to a symbol in the library?

To do what you want will require global operations:
1) In the Sch double click any of the devices whose footprint you wish to 
update, lets say you wish to make all resistors 0402 but leaving your caps 
as 0603.  Double click a resistor.
2) Click the Global button.
3) In the Attributes to Match By column for the Lib Ref field enter RES (or 
whatever your resistor symbol is called).  If you have some RES and some 
RESISTOR and you wish all of them to change then you can leave the * 
wildcard at the end as RES*, for example.
4) Since we only want to change 0603 resistors in this example we will put 
0603 into the Match By column in the Footprint field - this is in the 
middle column of the global dialog.  Confusing the functions of the 
different columns is one area where people unfamiliar with global ops get 
5) In the Copy Attributes column enter your new footprint into the 
footprint column (overwriting the {}). 0402 in this example.
6) If you wish to change all instances in all documents change the Change 
Scope (at the bottom of the global dialog)
7) Click OK and away it goes.

By correct use of the global operation you will only need to touch one of 
the parts and choose the footprint from the drop list and then apply this 
across all similar parts in one go.

Now you just hit all the resistors with a broad heavy sledgehammer.  If you 
want to be more specific, and cut and slice with a scalpel, you can match 
on the same footprint - or some wild-carded variant of it - by entering 
something appropriate into the footprint attribute to match by field. You 
could have also previously selected only those components you wish to 
change and match on selection (or even items that are the opposite 
selection status from the current part).  The feature is very powerful and 
well worth spending a day to understand.  The garbled text above is only a 
tiny introduction to what you can do with it.

The online and book manuals are helpful for this subject.  The {} in the 
Copy Attributes can be used for partial text substitution - a nice powerful 
feature and one that everyone should play with so they know what it can do.

Good luck,
Ian Wilson

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To join or leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
* Contact the list manager:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to