On 05:18 PM 2/01/2002 -0500, Bob Wolfe said:
>Thanks very much, I understand you can put anything you want in there for a
>footprint, I just would like the system to update what IS there and use it,
>without any extra work involved. I just used the 3 footprints for the
>example of what I was trying to accomplish. Like was stated and tried, if
>you put anything in there other than the first footprint defined every time
>you do a footprint update with the sync it WILL change the footprint back to
>that first one in the pulldown list defined in the part library.

If as Bob says the footprint in the Sch component is changed back to the 
first on the drop down list it could be related to the bug I saw but had 
assumed was fixed a long time ago.  This bug (from memory) was triggered 
when one of the components in the list had a name that the first n-letters 
were identical to the letters in the footprint entered in the edit 
box.  So, I found it was not possible to enter 0805 (and have it preserved) 
if there was a footprint in the drop list 0805_WAVE, for instance.  This is 
from (distant) memory so it may be all screwy.  But I do not think this is 
in fact what Bob is seeing.

>I really am
>just basically looking for the system to be driven by library and schematic

I think that, Bob, you may be using your library system a little 
differently from many of us.  You seem to be changing the footprint list in 
the library and then updating the Sch and then having to touch each 
instance of the symbol and then updating the PCB.  I think most people 
would fall into one of two other camps.  Camp 1 - Use the symbol as-is and 
simply enter the new footprint in the Sch symbol edit box, using the global 
functions to make it easy to change multiple component instances at a 
time.  In this case you are using the drop-list as a suggested list of 
common footprints but not the only legal footprints (that is if you enter 
any footprints into the list at all when you create the library 
part).  Camp 2 - the one value/one symbol crowd.  These people make a new 
Sch library part for every part they use - including each resistor value 
and variant (5%, 1%, 0.1%, 1watt 0.25 watt etc).  In this case the 
footprint drop list can potentially be used to hold only legal footprints.

Camp 1 users may well go back and occasionally change the footprint list in 
the library to reflect a change in design patterns (what sort of footprints 
they are using most).  But they do not have to.  Camp 2 users essentially 
believe that if it has a new footprint then it should have a new symbol as 
it is a different component.  There is some shades of grey between Camp 1 
and 2 but I have not come across anyone using the library system as I 
understand you are, but that is not saying it is wrong, just that I have 
not seen it before.

(I am hoping that the next version of Protel has better support for camp 2, 
by allowing locking of all attributes but designator in the library. It 
would be good if the designator prefix could be, optionally, locked as well.)

>I don't want to have to keep typing anything, I would like the update
>schematic or cache to actually take and use the footprint defined in the
>part even if it was the
>same name part but with the new footprint. My feeling is that update should
>work this way.

I just ran a test, pretty much as I understand you are doing, and it ran as 
I expected and as I would like.  That is, updating the footprint list in 
the Sch library for a symbol and the updating the Sch caused the footprint 
*list* of affected components to change but *not* the actual footprint as 
previously entered for that component.  Any other behavior would not seem 
correct to me - based on the fact that the drop list is only an offering of 
suggested footprints not a firm list with any sort of precedence.

I did find a little bit of a funny effect related to the bug I talked about 
above - in that the edit box text is used as a look-ahead, auto-complete, 
prefix to preselect an element on the drop list (if it matches) when the 
drop list arrow is clicked.  this can have an unintended side effect of 
changing the footprint to something else if you simply open the footprint 
drop list and close it again.  Try this, change the footprint on a 
component to only the first two letters of a footprint that is in the drop 
list.  Then click the footprint arrow twice and see what happens.  Not 
quite what some may expect since there has been no actual click in the drop 
list client area.

Ian Wilson

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* Contact the list manager:
* 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