You got it. Sorry I did not see your earlier post before, I just read it
I thought I was pretty clear what I was looking for, but guess it was clear
I guess from what you say it really is a bug and should not really function
I will need to experiment with global update a bit more extensively or look
doing something with a spreadsheet as suggested, just thought it could be
done within Protels
schematic update function much easier.
Again basically I have this client whose first Orcad schematic was actually
the start of the symbol library for this client, being that the import from
Orcad worked pretty well. The footprint fields came
over fine but were not what I wanted to see on the protel side I devoloped.
So each time I take in a new design I just copy the new symbols into the
existing library. Once they are all there I delete the
cache library that was created upon import and point only to that existing
library. It really seemed like the updateschematic function would work very
well and just automatically replace these footprint names from the library
it was pointing to with just the use of that function. Yes a good library is
a big portion
of any design job, I was just trying to keep that work effort to a minimum
and thought Protel's function
would have done just that. Oh Well.
Thanks again very much for the insight into this issue.
Robert M. Wolfe, C.I.D.
----- Original Message -----
From: "Abd ul-Rahman Lomax" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Thursday, January 03, 2002 4:05 PM
Subject: Re: [PEDA] Multisheet Problems & Updates etc.
> At 02:18 PM 1/3/2002 -0500, Bob Wolfe wrote:
> >But is it not true that you need to globally update each unique footprint
> >type part (not every part) at least separately globaly, sorry if I was
> >clear enough about this.
> When you are changing footprints -- or anything else -- you must select in
> some way those parts which are to be changed. You may use global edits or
> combinations of edits to make these changes based on almost any shared
> Mr. Wolfe has indeed uncovered a deficiency, but it seems to me that he
> not clearly expressed it. The way that Protel works is completely in line
> with schematic-driven design. The footprints are controlled from the
> design, if that is they way you want to operate. Or they can be
> alternatively controlled from the PCB, with the changes being taken back
> into the schematic.
> I wrote extensively on this yesterday, but today's comment from Mr. Wolfe
> does not seem to reflect his having read what I wrote. Perhaps I wrote too
> much; but I felt it necessary to examine his experience and complain in
> >By that I mean you can globally update all the footprint names FROM
> >"conn,.1ctr,.025pin,vert,shrd" TO say "XYZ" , etc but you still need to
> >that for each footprint type.
> Not necessarily. You could, for example, update all capacitors to "0603"
> without any regard to what footprint was originally there. Or you could by
> a global edit or manually (by "touching" each instance with shift-click)
> select what you did *not* want to change and then change the rest by
> appropriately controlling the global edit.
> >On a large schematic that can still be a bit of work.
> As I have mentioned, determining what footprints to use is about one-third
> of a PCB designer's job. There are ways that this could be automated, to
> sure, but those too take a lot of work to develop, and many of us would
> like to be forced to use them.
> As I have written, in the end we may find ourselves with
> footprints, but that is *not* what we now have. We have
> schematic-controlled footprints.
> >I admit it is easy for resistors, caps etc. the majority use the same
> >0603 etc. And those are not as much an issue to change.
> >Unless there is some other way to drive the global update or I am not
> >it to its fullest,
> >this is still seems way too much work for a large schematic.
> Nothing that Mr. Wolfe has explicitly described so far is much more work,
> if any, than the minimum necessary for footprints to be intelligently
> The situation Mr. Wolfe has described is one where a schematic is provided
> to the designer which has either no footprints assigned, or the footprints
> assigned are incorrect for use with Protel. This is a common situation for
> contract designers or service bureaus.
> If one wants the schematic to control footprint selection, which I
> a good idea and which Mr. Wolfe also seems to desire, one must choose *for
> each part* a footprint. However, if parts have some shared characteristic
> that can be used to control a global edit, those parts can be changed en
> There is another option, which is to change the footprints in a
> spreadsheet. This is how I used to accomplish the matter aforetime: I
> extract component information from the net list, convert it to a
> spreadsheet, enter footprint names in the appropriate fields (and I could
> use various sort and/or replacement techniques to make a whole series of
> footprint changes at once), and then convert that back to a net list part
> section for load into the PCB. I did this with Tango and I did this with
> Protel, indeed, I still do where I have no Protel schematic but only a
> client-supplied net list.
> But in the present case, brought to us by Mr. Wolfe, we have an OrCAD
> schematic which has been imported to Protel, so we might as well control
> footprints from the schematic; this will help with changes later on.
> Now, here is the deficiency: if I have assigned the footprints in the
> schematic and I make a project library, the footprints I have assigned are
> not taken back into the library. This causes me no pain with the present
> design, but if I am going make schematic changes to add parts, or if I am
> going to do new schematics for this client, I will regret that the
> footprints I have painstakingly assigned -- yes, it is work -- will not be
> shown as options in the project library part description dialog; I will
> need to assign footprints again, or edit the library. And there is no easy
> way to edit the library other than by editing each part in it. This is not
> a *huge* amount of work, normally, particularly if one has a report in
> with all the footprints listed, easy to generate, but I can see that it
> would seem irritating to have to do it.
> I have suggested a solution, a utility to read a schematic and stuff the
> used footprints into the footprint option fields in the cache copy of the
> parts. This would cause the project library, when created, to contain
> footprints. This is not a difficult utility to write. Questions to be
> answered would include how the program should behave if more than four
> footprints are used for that part in the schematic and how to treat
> existing unused footprint options.
> But a case could be made for using only one footprint per library part
> (i.e.. one would use a separate symbol for each footprint variety, so one
> would have, for example, C-0402, C-0603, C-0805, etc. If this practice
> followed, then the whole process would be simplified even though many more
> symbols would exist.
> Now, with the instant problem, an OrCAD imported schematic with wrong
> footprints. Sometimes there are no footprints, but let me assume that
> has been configured to give footprints that some engineer actually chose.
> So the names means something to him or her, but they just don't pull up
> right Protel parts. In this case I'd recommend making a PCB library which
> gives those names to the right footprints. This would be a client-specific
> library, used whenever working with schematics from that client.
> Now, it might be useful to be able to use a translation table. I.e., if
> there is X footprint name, change it to Y based on a table. Again, it
> not be difficult to write a utility to do this. Service bureaus often face
> special problems like this, certainly I did, which I why I used to write
> lots of utilities. But Protel's global edits and spreadsheet facilities
> have made much of what I formerly would have done by opening up QuickBasic
> no longer necessary.
> One very powerful and fast technique for using global edit is to select,
> with shift-click, whatever one wants to edit. Then selection can be used
> a match criterion. Or various edits, as Mr. Wilson has noted, can be used
> to select what one wants to edit. One could select all capacitors in the
> first edit (by matching on C*, perhaps), then deselect all electrolytics
> either manually with shift-click or by some other shared criterion, and
> then assign a footprint to what remains.
> Using a spreadsheet taken into Excel, one can do much more sophisticated
> global edits based on formulas and more, perhaps even lookup tables, I
> haven't tried it but I'm fairly sure it could be easily done. So if I
> received an OrCAD schematic from a client who uses particular footprint
> names, I could translate those names to Protel. But as I have mentioned
> above, I think it might be better to use a client footprint library,
> certainly it would be more direct.
> [EMAIL PROTECTED]
> Abdulrahman Lomax
> Easthampton, Massachusetts USA
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *