[hpsdr] Kicad

[Philip Covington]

Phil,

If you get the latest HPSDR.lib out of SVN, there is two new symbols:
JACK_MONO and JACK_STEREO.

I haven't found PCB decals for these yet so I might have to create them.

73 de phil N8VB


On 4/3/06, Philip Covington <p.covington at gmail.com> wrote:
> 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
>

 1144079875.0