[hpsdr] Kicad

[Philip Covington]

Hi Phil,

See answers below:

On 4/3/06, Phil Harman <pvharman at arach.net.au> wrote:
> ***** High Performance Software Defined Radio Discussion List *****
>
> I've stated to draw the Janus circuit diagram in Kicad and run into a few
> newbie questions:
>
>
>
>   1.. If I insert a multi part opamp (e.g. quad opamp LM324) then each
> instance , UxA, UxB, UxC, UxD, has   power supply connections. Is there away
> to turn these off so there is only one supply connections shown - if not is
> it OK to just connect power and ground to one opamp or does the same supply
> have to go to all four?

How I have handled it is to go into the library editor for the LM324
part and select Part A.  I then use the pin editor (right click on pin
and the select edit) on the power pins and deselect "common to units".
 Now only part A will display the power pins, parts B through D do
not.

>   2.. I can't find a 3.5mm stereo jack socket  in the components list. Do I
> have to create one or is there a conversion program available so I can
> import one from say Protel?

There are some libraries converted over from Orcad and Eagle.  I will
look for a 3.5mm jack in those and get back with you.

>   3.. Is there a more detailed  explanation of how to create multiple
> schematics and  pass global signals between them? Do I have to run wires to
> the global labels or can I just refer to them on each different page?
> I'm sure there will be more questions as I move forward but these are the
> main ones at the moment.

Lately, I avoid multiple sheets in Kicad because it is a nightmare
keeping it straight after you have been away from it a while.  If you
use multiple sheets you need to place hierarchical symbols and then
place glabel ports to the symbol (as I recall)... otherwise like named
glabels on different sheets do not get connected because a sheet
number is appended to them.  For example if you have a glabel on sheet
1 named "MyLabel" and a glabel on sheet 2 also named "MyLabel" then
the schematic file refers to these as MyLabel_1 and MyLabel_2.  When
you run the netlister you will get different nets.   This is why I
think that you have to explicitly connect these names though the
hierarchical symbols, label ports, and wires.  What a PITA!

> 73's  Phil...VK6APH

The other really annoying thing in Kicad is that you do not have a
list of netnames already defined that you can pick from when adding a
label.  It would be nice if Kicad would fill a list or combo box with
the already defined net names.  I have been meaning to add this
functionality (Kicad makes it hard since nets are not really defined
until the netlister processes the schematic file... until that point
all objects just have a associated text name that determines the net
they get connected to).  If you look at the schematic file you can see
how Kicad creates labels with the sheet name appended.

All this stuff can be fixed... but I haven't found the time to do it yet.

73 de Phil N8VB

 1144076747.0