At 06:41 PM 12/27/2001 -0500, Bob Wolfe wrote:
>But what would you do if you are doing a new board and the schematic was
>imported from Orcad and none of the footprint names matched the ones in the
>you want to use.

In other words, situation normal, all fouled up.

I would edit the footprint fields in the parts to show correct footprints. 
Much of this can usually be done globally. Any parts where I don't know 
what footprint to use I'd probably use some descriptive name so I know what 
to create later. The synchronizer will tell me what does not exist.

Then I can make the needed footprints or get them from somewhere. It may be 
simpler to just place them on the PCB and give them the correct refdes. The 
synchronizer will sort this out; just don't let it replace your new 
footprints! (uncheck update component footprints in the Update PCB dialog.)

But you could also insert the correct new footprint names in the schematic 
symbol footprint fields, if they are different from what is already there. 
This, however, will then require that you have the new footprints in an 
open library, available when the synchronizer is running. This can be more 
trouble than it is worth. That is why I suggest simply placing the correct 
footprint on the PCB and letting the synchronizer deal with it.

Once you have all the correct footprints on the PCB, however you got them 
there, Update Schematic from PCB. This will stuff the footprint fields with 
what has been used on the PCB. (Make sure you have first run the 
synchronizer in the other direction and that it has matched all your 
footprints with a schematic instance.)

>Again what I saw was that it woul donly put down the first
>footprint on the list and untill you touched ALL of the
>different types of symbols to global
>update the footprints you still would not get your library footprints. At
>least without
>quite a bit of effort.

Yes, it does take effort to do PCB design. Else they would not pay us to do 
it, would they? Consider this: if the program could automatically choose 
all the correct footprints, half our job would be gone. Someone, somewhere, 
has to choose those footprints, and, yes, the choice must be made for each 
"type of symbol" or even more specifically than that!!! (in other words, we 
often have the same symbol with different footprints, this is totally 
normal. Consider capacitors....)

Once again, let me repeat: footprints are not controlled from the library 
level. Not as Protel is presently implemented, this may change. If it 
changes, as has been announced, I assume that we will have a separate 
superlibrary name that specifies a part completely: it will include a 
symbol name, a footprint name, and other information as well, I'd expect. 
I'll hope that Protel will preserve the ability to simply place a symbol 
without making all the other choices at that time, likewise footprints on a 
PCB, but ultimately there are physical parts presumed to be identical; then 
these parts have a symbol, which might be the same as the symbol for other 
parts, and these parts have a footprint, which might be shared with other 
parts as well.

If you take a part from the superlibrary, whatever they will call it, you 
will have symbol and footprint already specified. If you want to change the 
footprint, you will have to take *another* part from the superlibrary, 
which will be part-oriented, not symbol- or footprint-oriented.

If they have done something seriously different, I'll be surprised....

Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to