How do you deal with unused pins on schematic symbols when the symbol is only electrically connected to fewer pins than the physical device or footprint has? Some of the more difficult parts to configure are devices that electrically connect like the TO220 , a 3 leaded device with a electrically connected heat sink 'TAB'. Do you treat it as a pin? How do you show it on the schematic?
I would usually show a pin for the tab - I have a couple of versions of stuff like TO220's - a simple three pin that is used when the device is free standing and upright, a four pin version when the device is lead formed and lies flat to the PCB and then others that reflect the pinning of heatsinks that I am using. These Sch parts then match up directly with appropriate versions of the PCB parts and the PCB and Sch synch easily. Sometimes I don't bother with showing heatsink pins on the Sch and just patch up the heatsink pad nets manually once I start the PCB (I almost always have different versions of the TO-220+heatsink in my PCBLib though - this ensures I give the required clearances and I only need work out the mechanics once.)
P2004 has further improved the use of multiple pads on a PCB footprint with the same designator, but there seems to still be a problem when you update a PCB footprint from a library that causes some pain when working this way.
I have seen folks stack the pins one on top of the other to force a 'connect dot' on the schematic to graphically look like a 3 pin device but actually connect the tab to the center pin. Other devices like diodes that are packaged in SOT-23 packages can only use 2 out of the 3 available pins, but the schematic symbol for a diode is a 2 pin device, which may be connected between pin 1 and pin 3 of the SOT-23. It might be convenient to run a trace through the unconnected lead on the SOT-23 (pin 2) for layout sake, but it will generate an error on your board when you run DRC...
SOT23 diodes - I show the unused pin and place a small set of lines that spell out NC (as in no connect). I use lines as text in SchLib symbols P99SE and DXP does flip or rotate correctly when placed on a sch - the line do. I think this issue was fixed in P2004.
Generally I think that if there is an electrical connection on a device then there should be a matching pin on the Sch. I try to give as much information to the ERC (and people) as possible. I put nc pins on my Sch symbols. I often change the ERC matrix to warn if any pin is unconnected and then place NoERC markers on stuff that should not be connected.
This is what I do. I gather some people don't like my schematics as they complain of too much information. People doing the design reviews and testing (usually me) seem to like them.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *