[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]

Re: gEDA-user: Using underlying schematics

I use gnetlist to generate the netlist.

gnetlist -gPCB -o HierarchySimple.net HierarchySimple.sch

note just give gnetlist the top level schematic.

Steve Meier


Steve Meier wrote:

Peter,

Try this.....

First edit the system-commonrc file.. Mine is found in
/usr/local/share/gEDA.

Add the following lines

(source-library ".")
(source-library-search ".")

Then create a project directory and insert the following attached files
HierarchySimple.sch, HierarchySimple1.sch and HierarchySimple2.sch

Put the following symbol files into a symbol directory such as
/usr/local/share/gEDA/sym/local

HierarchySimple1.sym and HierarchySimple2.sym

Change Directory to your project directory.

run gschem HierarchySimple.sch

Click on the HierarchySimple1 symbol

hit <Shift>H
hit d

you should now be looking at the page HierarchySimple1.sch

hit <Shift>H
hit u

you should now be at the top page

hit <Shift>H
hit s

you should now be looking at HierarchySimple.sym
click on the edit menu option pull down to the Show/Hide Inv Text

The key thing for hierarchy is the interconnect io symbols in the lower
level schematics and the io pins in the symbol files. Take a good look
at those.

Best Wishes,

Steve Meier

On Tue, 2004-11-30 at 03:08, Peter Brett wrote:


Hi there,

I'm just getting started using gschem, and I've got a subcircuit schematic I want to incorporate several times into a higher-level schematic.  I've created a symbol for the subcircuit, but I can't work out how to make a pin on the symbol correspond to an input or output of the subcircuit.  TFM doesn't seem to offer any clues...

Hope someone can help me out in my confusion!

Thanks,

Peter Brett

--
SLE System Display Group
mailto:peter.brett@sharp.co.uk
http://www.sle.sharp.co.uk/research/sop/



------------------------------------------------------------------------

v 20040111 1
C 13200 71100 1 0 0 74541-1.sym
{
T 14900 74100 5 10 1 1 0 6 1
refdes=U1
}
N 15200 73800 16500 73800 4
C 16500 73700 1 0 0 output-2.sym
{
T 17400 73900 5 10 0 0 0 0 1
net=MyPin:1
T 17400 73800 5 10 1 1 0 1 1
value=MyPin
T 16500 73700 5 10 0 0 0 0 1
refdes=MyPin
}


------------------------------------------------------------------------

v 20040111 1
C 13200 71100 1 0 0 74541-1.sym
{
T 14900 74100 5 10 1 1 0 6 1
refdes=U1
}
C 8300 73700 1 0 0 input-2.sym
{
T 8300 73900 5 10 0 0 0 0 1
net=YourPin:1
T 8800 73800 5 10 1 1 0 7 1
value=YourPin
T 8300 73700 5 10 0 1 0 0 1
refdes=YourPin
}
N 9700 73800 13200 73800 4


------------------------------------------------------------------------

v 20040111 1
C 61100 52800 1 0 0 HierarchySimple1.sym
{
T 61400 53100 5 10 1 1 0 0 1
refdes=S1
}
C 68700 52700 1 0 0 HierarchySimple2.sym
{
T 69300 53100 5 10 1 1 0 0 1
refdes=S2
}
N 66400 57100 68900 57100 4


------------------------------------------------------------------------

v 20040111 1
B 600 700 4300 4800 3 0 0 0 -1 -1 0 -1 -1 -1 -1 -1
{
T 1600 5100 5 10 1 1 0 0 1
description=HierarchySimple1
}
T 300 300 8 10 1 1 0 0 1
refdes=S1
P 5300 4300 4900 4300 1 0 0
{
T 5300 4300 5 10 1 1 0 0 1
pinnumber=1
T 4300 4300 5 10 1 1 0 0 1
pinlabel=MyPin
}
T 1200 5900 8 10 0 0 0 0 1
source=HierarchySimple1.sch


------------------------------------------------------------------------

v 20040111 1
T 1300 6800 8 10 0 0 0 0 1
source=HierarchySimple2.sch
B 600 700 4300 4800 3 0 0 0 -1 -1 0 -1 -1 -1 -1 -1
{
T 1600 5100 5 10 1 1 0 0 1
description=HierarchySimple2
}
P 200 4400 600 4400 1 0 0
{
T 200 4400 5 10 1 1 0 0 1
pinnumber=1
T 700 4400 5 10 1 1 0 0 1
pinlabel=YourPin
}
T 600 400 8 10 1 1 0 0 1
refdes=S1