Re: gEDA-user: Heavy Symbols and such

[Dan McMahill <dan@xxxxxxxxxxxx>]

Steven Ball wrote:
> I've been thinking about this a bit, and here's my 2 cents:
> 
> gschem and pcb both really just want light symbols/footprints.  It  
> would never really be a good idea to expect to stick one into the  
> other, I mean, what if you change packages or something?  I guess you  
> could up rev the schematic or whatnot, but I'd prefer that bit of  
> things to be divorced.


this is where I really disagree.  If you change the package, then you 
are changing the part.  The vendor part number is different, the package 
is different, it is not uncommon for the pinout to be different.  The 
new package has different thermal characterstics.  In short, you have 
changed the design and I'm a strong believer in the schematic being the 
controlling source for a board design.

> So, in order to go from gschem to pcb, we have the step of gsch2pcb,  
> or the 'new' xgsch2pcb.  What if the gui was extended such that you  
> get a list of parts, maybe even a window with a zoomed in part of the  
> schematic highlighting the part you currently have selected, with  
> another part of the screen showing possible footprints for this  
> device?  Maybe even tie it into a database off gedasymbols to make use  
> of all the good work happening there?  So, you pick a footprint, maybe  
> get a preview of what it looks like and a little text box with  
> details.  Then, you could step through and pick footprints for pcb.   
> If you explicitly specify a footprint the 'old' way via footprint= in  
> gschem, you could have it skip this pick step.  Once you are done,  
> there ya go, footprints populated for pcb to pull in with a netlist.   
> You could even go back and change footprints, just like if you were to  
> change the schematic footprint= and re-gsch2pcb.
> 
> Then, you'd just need to maintain a mapping of symbol -> footprint  
> somewhere.  I'd love to see this be able to tie into a filesystem, a  
> database, and even gedasymbols as sources.

its not just that.  You'd need to maintain a list that deals with part 
number differences, pinout differences, etc.

But the good thing about the current system is it does not preclude you 
from using heavy symbols which I pretty much exclusively do.

> Of course, that all sounds like work and whatnot, but I'd be willing  
> to help out.
> 
> -Steve
> 
> 
> On Dec 5, 2007, at 3:03 PM, Dave N6NZ wrote:
> 
>> Steve Meier wrote:
>>> Dave,
>>>
>>>
>>>
>>> I have been thinking that the way to do back annotation is to add a
>>> schematic level attribute that is attached to a symbol. Something  
>>> like
>>>
>>> C 8500 9600 1 180 0 big_fpga-1.sym
>>> {
>>> T 8300 9100 5 10 1 1 180 0 1
>>> refdes=U1
>>> T -100 -100 5 10 1 1 180 0 1
>>> pinswap=a12,g13
>>> }
>>>
>>> This could then be used when viewing the schematic or generating a
>>> netlist to swap the two pins.
>> This seems like a good idea.  In fact, it strikes me as very similar  
>> to
>> the "slots" concept.  With slots, we have "numslots", "slot", and
>> "slotdef".  Perhaps pin swapping has an orthogonal set of attributes.
>> Of course, pin swapping interacts with slot swapping -- think of our  
>> old
>> friend the 74xx00 -- four slots, each with swappable inputs within  
>> the slot.
>>
>> I suppose today one could define 8 slots for a 7400, sounds a little
>> odd, but the point is you would only use 4 of them at a time.  Each  
>> slot
>> would be defined twice -- once for each possible swap. Obviously, this
>> leads to combinatorial explosion, but for practical parts it might be
>> OK.  I think the right answer is that slots map pinseq #'s onto  
>> logical
>> pins, and "swaps" map the logical pins onto physical pins, which
>> requires an extra layer of symbolic pin names in between slots and  
>> swaps
>> that does not currently exist.
>>
>> I like the idea of the netlister being able to read a file of slot=N  
>> and
>> swap=N attributes and generate the netlist accordingly.  Then after  
>> the
>> layout is done, gschem could import the same file to update the
>> attributes to accomplish back-annotation.
>>
>> And let's not forget my desire to target multiple package pin-outs --
>> but I think that can be handled by creative use of slots, although  
>> its a
>> bit of a hack.
>>
>> -dave
>>> Steve Meier
>>>
>>> On Wed, 2007-12-05 at 10:13 -0800, Dave N6NZ wrote:
>>>> Steve Meier wrote:
>>>>> Eventually, I would also like to see being able to define the logic
>>>>> level for a group of pins, can the pins be used differentialy? if  
>>>>> so
>>>>> which pins are paired? Can we swap pins if so which ones?
>>>> The pin swapping question brings up another of my pet peeves --  
>>>> when the
>>>> same part comes in packages with different pin outs, it needs  
>>>> different
>>>> symbols.  Although -- last night it occurred to me that I could use
>>>> slots to fake that out.  Even if the part isn't slotted, I could  
>>>> define
>>>> a slot for each package pin out.
>>>>
>>>> But it really points out the fact that there is a level of  
>>>> abstraction
>>>> missing in the current symbol definition, and that interacts with  
>>>> back
>>>> annotation from what ever PCB layout tool you are using.  Maybe the
>>>> netlister needs to be enhanced to be a more interactive tool  
>>>> instead of
>>>> a one-way translator to make all the work well.
>>>>
>>>> -dave
>>>>
>>
>> _______________________________________________
>> geda-user mailing list
>> geda-user@xxxxxxxxxxxxxx
>> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
> 
> 
> 
> _______________________________________________
> geda-user mailing list
> geda-user@xxxxxxxxxxxxxx
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
> 




_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user