I just would like to ask a question about how you handle TO-220 footprints (& the like)...
There are a number of ways to handle this kind of part. I'll give my favorite first.
Two pads are placed in the footprint for the tab. One is a through-hole pad and the other is a surface pad to create the heat-sink area. These pads are in contact. If they had the same center, one would only need one pad, but they don't share the same center. Protel does not allow off-center pads, one of the major shortcomings of the product (not too difficult to live with or I'm sure it would have been fixed).
The tab is the 4th "pin" for the TO-220 part, typically it is connected internally to pin 2. Instead of adding a fourth pin (and fifth pin) to the schematic part, I number the tab pins as "2".
Under some conditions, Protel does not handle duplicate pin numbers correctly. As a precaution, it is a good idea in general to reload the net list or resynchronize before presuming that a DRC is correct. If there are any macros created, there is an anomaly of some kind that might require attention. Other than this (which is a bug), there is no reason not to do what I've suggested. It automatically creates the solder mask opening.
However, an alternate procedure is to place a fill on the top layer for what would above been the fifth pin. Another fill is then placed in the appropriate position on the top solder mask layer. Fills, by the way, normally are plotted as flashes, they are not drawn, so every different fill size creates a different aperture definition, not usually a significant issue.
The extra features should be part of the footprint so that they will move with the part.
Another approach is to add 4th and 5th pins to the schematic symbol. This is straightforward. Sometimes designers hide the names on those pins and place them in the same position as pin 2, which will cause Protel to automatically add a connect dot at the end of pin 2; the extra pins are otherwise invisible. It is a fairly neat way to solve the problem. (Don't "hide" the pins, they will automatically be assigned the net which is their name.... that might be fine in *this* schematic, if you name then GND or whatever net is needed, but it might not work on another, and you can really confuse a designer who inherits your files.)
As a way to make the part bulletproof from a DRC point of view, a track might be added to the footprint shorting pin 2 to the tab structure. This track will not automatically be assigned the correct net upon netlist transfer, one might need to run Update Free Primitives from Component Pads in the Netlist Manager to assign the net. Once the track has the correct net, it will keep it through subsequent transfers. You could manually edit the track to the proper net, but you'll have to unlock primitives for the footprint first.... Remember to relock 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *