Mail Archives: geda-user/2015/07/03/12:33:14
On Fri, Jul 03, 2015 at 04:56:21PM +0200, Roland Lutz wrote:
> While refactoring gnetlist, I've encountered a few quasi-synonymous terms
> which seem to refer to subtly different concepts:
>
> component <-> device <-> netlist <-> package <-> symbol
>
> Not being a native speaker, I'd like to ask you what you mean when using
> these terms, and what you understand to be the difference between them.
>
> Also, what's the difference between a pin and a net, and between a uref and
> a refdes? (If it's the same thing, why are there two different names
> for it?)
>
I am not a native speaker, either. However, since I've translated
several pages of the geda site with these terms and needed to do this
correctly, I can (I hope) make it clear for you and if you still in
doubt, provide you with some links where they are explained (by your
request, I don't have enough time to do it just now). And you can always
search the wiki.geda-project.org pages for the terms you need using the
search field at the top-right corner of any page. There is also a
glossary page.
So, let's begin:
'symbol' is a graphical schematic representation of the device and the
file for the same representation in electronic documents (*.sym)
'component' is an instantiation of a symbol in a schematic. So, if the
schematic has one hundred of resistors, which we call 'components',
they all can be represented by one symbol in the schematic (say,
resistor-2.sym)
'device' is the device name. There are many possible devices in the real
world. Say, all resistors are represented by the same device -
resistor. There are various devices (device names) for integrated
circuits, say, 4004, LM7805 and so on. The device attribute in
gschem schematics is used mostly for simulation purposes.
'package' is a physical package of a device, its physical body with
pins, or its reflection on the screen or paper sheet. Examples:
TO92 for transistors, DIP14 for some integrated circuits and so on.
The term is often used in the context of PCB.
N.B.: In the geda-gaf and pcb sources all these terms can be used as
interchangeable in some contexts. So you can see, for example, that
somebody has used 'symbol' or 'package' instead of 'component' and vice
versa, and so on. Sometimes, you can find the term 'complex' which means
'component' (as a complex object) in many C sources. In the gnetlist
source files some of these words may be used as names of corresponding
attributes.
'net' ('Netz' in German) is a graphical (and electronic)
representation of a real wire in a complex aggregate, or a track on
PCB which electrically connects some devices.
'pin' is a real connector on a device which connects the device body
with PCB, or the usually white colored gschem primitive object
connecting symbols with nets in schematics.
In the context of the gschem symbol both words ('net' and 'pin') can
represent a physical pin. The only difference is that the term 'pin'
always represents an existing object on a schematic - the real symbol
pin, while 'net' is an attribute of the form 'net=value' which says:
"there are one more pin on the real symbol, which is not shown here, but
is connected to the net with the name 'value'". For example, 7400-1.sym
has no power pins and they will not be shown on schematics. Many users
consider not convenient to always see all pins. So we just add the
attribute 'net=GND:7', which means that the symbol pin 7 must be
connected to the net GND (a wire on a breadboard or a track on PCB).
Otherwise, the 'net=' attribute could be realized a hidden net, and
'net=value:pin_number' in a symbol is equal to the attribute
'netname=value' attached to a real net on the schematic and a pin with
pin number equal to pin_number attached to that net.
HTH,
Vladimir
- Raw text -