Re: gEDA-user: drc errors

[Carlos Nieves Ónega <cnieves@xxxxxxxxxx>]

Hi Marc,
the gschem user guide
(http://geda.seul.org/docs/current/gschem/node18.html) says:
---- begin gschem user guide note
You can label nets by using the label= attribute. Do not attach more
than one label= to a net. You only need to attach the label= attribute
to one net segment. Different nets (i.e. multiple net segments which
aren't connected together) which have the same attribute label= attached
to them are also considered electrically connected. You will not get any
indication of this connection by gschem, but the netlister (gnetlist)
considers nets with the same label= attribute electrically connected.
---- end gschem user guide note

In gschem, if you give two different nets the same name, you are
electrically connecting them. So the situation you have in your
schematic is that all nets you named are the same net: all of them are
shorted!!!

This is the first error. When you correct this, there will be two more
errors:
ERROR: Net has only one connected pin: unnamed_net4
ERROR: Net has only one connected pin: unnamed_net2

Since this message doesn't seem to be clear enough, I have changed it in
CVS to:
ERROR: Net 'unnamed_net4' is connected to only one pin.

If you don't give a name to a net, gschem will name it as unnamed_net1,
unnamed_net2, and so on. This doesn't mean that you have to name every
net in your design!!!.
That error means that you have the net unnamed_net4 which is connected
to only ONE pin. The same happens with unnamed_net2.
Maybe you don't know what nets are those, but a quick look at your
schematic and you will realize that pins 1 and 8 of U2 are not connected
to anywhere, so they are the cause of that error.
If you want a pin to remain unconnected, but you don't want the drc2
reports it, place the misc/nc-* symbol connected to it. This is the 'no
connect' symbol.

Finally, there is another error:
ERROR: Pin(s) with pintype 'output': U2:6 
	are connected to pin(s) with pintype 'power': U1:2 V1:2 U2:4 
In general, you shouldn't connect an output pin to a power pin, since it
is usually a conflict: which one will be stronger and set the value of
the net?. In the case of your schematic, you want them to be connected
as is, so you can ignore that error and go on.

It seems like you are a newbie to electronic design programs in general.
I think you can spend some hours just reading the docs, trying simple
examples, and learning how you can use gschem, before going on. Every
program and every subject has a basic vocabulary you should learn in
order to be able to use it.

If it is useful to you, there is another gnetlist backend named 'geda'.
It will output the components and connections of your schematic. 
Use it as 'gnetlist -g geda your_schematic.sch -o output.txt' and review
the file output.txt. It is useful to review the connections.

Best regards,

Carlos


El sÃb, 14-01-2006 a las 23:15 +0000, Marc escribiÃ:
> well drc only asked me to name the tracks there was no mention they had 
> to be different
> 
> what should i do rename them all differently
> 
> Marc :)