At 04:21 PM 3/13/01 -0700, Gordon Price wrote:
>Ladies & Gents,
>         How do you globally fix hidden power pins(from Protel library parts)
>that go to a net called "Vcc", to go to a fully defined and existing layer
>that has a net name of "+3.3V" ????

Two ways:

(1) Edit the library part so that the pin name has +3.3V instead of VCC.
(2) Unhide the pins in the sheet editor and explicitly connect the pins to 
the power net you want to use.

The second method is probably better. Some of us firmly believe that hidden 
pins should never be used. I'm not quite so radical, but they do have a 
point, or, more accurately, several points.

>         I have a power plane named "+3.3V" and can get my own parts to
>connect to the plane but can't get Vcc nets(from Protel library parts) to
>connect to the +3.3V net.

Of course not. Assuming that you have a separate VCC net on the board, say 
+5V, then you must keep the nets separate. When you have multiple power 
voltages, the use of hidden pins becomes hazardous. They are only really 
useful when only one voltage is used to connect to hidden pins.

>  If I place a net reference of Vcc on the +3.3V net
>the auto router runs traces instead of connecting to the defined power

What net name was assigned to the power plane? I'd guess VCC. You 
successfully renamed VCC to +3.3V, but perhaps you did not change the power 
plane net assignment to +3.3V. (That is done in the stack manager in Protel 

>  It would be nice to have more than one net name be able to go to a
>given power plane and net. Where am I missing the boat???

The boat is a boat called "Net Names are Unique." As I recall (and from 
what was said above) you can rename nets on a sheet. It's a little fussy. I 
don't remember the rule: if I place a power object and connect it to a 
piece of wire with a net label on it, I think one of them has precedence 
over the other.

But in the end, in what goes to the PCB, you have only one net with one 
name. There is no provision for anything else, and anything else would be 
*very* confusing.

>         I can't for the life of me understand with the prevalence of
>different supply voltages of chips, why Protel uses hidden power pins and
>fixed net names. I am using +1.8V, +3.3V and +5V on one board.

It's a library control problem. Do you want the users to be able to edit 
pin attributes in the sheet editor? Some CAD programs allow this, some do 
not. I think most do not, and Protel is with the majority. I'd rather that 
it be allowed, but any edit to a pin in the sheet editor should set a flag 
that can then be used to generate an edited pin report. Another report 
should give the names of all hidden pins in a design with information about 
the part to which the pin belongs.

The advantages of this:

(1) We could unhide pins, edit the name, and rehide them if we really want 
to have hidden power pins.
(2) We could change the electrical attribute of "I/O" pins in programmable 
parts to match the configuration as used, and thus get the advantages of 
improved electrical rules checking for those nets.

I do not suggest, however, that we be able to edit pin *numbers*. This is 
far too dangerous. If we really need to edit pin numbers, then we should 
make a new symbol.

Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To join or leave this list visit:
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
* Contact the list manager:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to