At 09:39 AM 2/3/2002 -0800, Tony Karavidas wrote:
>I have a schematic that uses an array of SPST switches and LEDs.
>On the PCB, I want to potentially keeps these as integrated parts, or
>possibly as separate LEDs and switches.
>
>How can I draw one schematic and still have the flexibility to use either
>physical configuration? If I keep the LED and switch arrays separate in the
>sch, then annotation will make two parts (D1 and SW1) for each switch with a
>built-in LED.

What you have on the schematic does not prevent you from assembling a board 
in whatever imaginative way you might invent. In other words, you have 
flexibility.

However, if you want automatic linking with a footprint, it's not easy to 
do what you are suggesting. We have no provision for alternate footprints, 
only various workarounds. For example, you can double-pad a single part so 
that each pad has differing possible locations. Unstated above was the 
physical relationship of the pads in question. Would the single parts, 
properly arranged, also serve for the combined part ("integrated part")? If 
so, then one way to treat this would be to put individual parts on the 
schematic and then arrange and *group* the invididual parts on the PCB. 
Protel 99SE supports component groups, which will move together as a unit.

Another approach, hinted at above, is to have a single footprint (and thus 
a single schematic symbol) that represents all the optional pad position.


>If I make a special sch symbol that contains an LED and a switch, the
>schematic is ugly as hell, and THEN I can't use a separate switch and
>separate LED.

Who says you can't? If the single footprint will accomodate both, you can 
do either one. As to ugly, there is no reason for the special schematic 
symbol to look much different from the discrete symbols, if that is what 
you like. To double-pad a pin, if desired, place two pins, and you might 
hide the name and number for one of them. This will create, on the 
schematic, a junction, a clue that something unusual is present here.

You could also arrange the integrated part and individual parts so that 
they are on top of each other on the schematic -- if the integrated part 
has been created to accomodate this. This too will create junction dots. On 
the PCB, one would place both the integrated part and the individual parts, 
the assembly is then merely a standard alternate insertion problem. 
("Insert U1 OR insert S1,S2,S3,DS1,DS2,DS3.")

Reading back to the original question, I want to consider the problem which 
may be Mr. Karavidas' actual problem. (I originally placed, perhaps, too 
much emphasis on his mention of the "array.") I have a part which I might 
use which is an integrated switch and LED. I might also use, instead, the 
same switch without the LED, and then a separate LED.

Since the switch is one switch, I presume that the switch footprint is 
identical either way.

The schematic should show, in my opinion, the integrated switch plus an 
LED. The LEDs are optional insertion if switches without LEDs are used. No 
special techniques would be used, no double-padding or double-pinning. This 
would be completely clear if a note explains the option. To assemble the 
integrated option, instructions are given not to insert the LEDs.

[EMAIL PROTECTED]
Abdulrahman Lomax
Easthampton, Massachusetts USA

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