X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f X-Recipient: geda-user AT delorie DOT com X-Original-DKIM-Signature: v=1; a=rsa-sha256; c=relaxed/relaxed; d=gmail.com; s=20120113; h=date:from:to:subject:message-id:mail-followup-to:references :mime-version:content-type:content-disposition:in-reply-to :user-agent; bh=4nwz6bcCH428LGg0BCXFSGFcqOUne9yYmygJyg1lL4U=; b=pP3gFO1JFbz/ZhP6C4Qzgo+aGdbChjAFKhY9zT3jdtV7JHRjmWL5ygWthW7AnTJ5yd NMfxrP+G8Bd6ffK/Ow5PMcLckfs31YH//WkAEjpL5fmQEQqR7KuKpsHnpv2LGGUui+VX Z7gwBjB/6IkqnRMF8Gds/h23s7aGm7ISfrm57J+aZEUuPqqDEizw54++HMl4Jq+bTNsh eZoWEgJr4Pi1AqOuybxOHsBx8Ue8gDImsvQoalefcDcb5Jzi0CvWUs0NYqx/22Xks4Lj vDCW1EYryQPR/Lkgbx0ybWMeNOlfHkZzndNxT9h5nsgWMoboCgIxBPU1CLtbVbA/8Au1 2Mlg== X-Received: by 10.152.43.110 with SMTP id v14mr36644111lal.4.1435941184383; Fri, 03 Jul 2015 09:33:04 -0700 (PDT) Date: Fri, 3 Jul 2015 19:33:02 +0300 From: "Vladimir Zhbanov (vzhbanov AT gmail DOT com) [via geda-user AT delorie DOT com]" To: geda-user AT delorie DOT com Subject: Re: [geda-user] Language conventions: component vs. package vs. device... Message-ID: <20150703163302.GA19536@localhost.localdomain> Mail-Followup-To: geda-user AT delorie DOT com References: MIME-Version: 1.0 Content-Type: text/plain; charset=utf-8 Content-Disposition: inline In-Reply-To: User-Agent: Mutt/1.5.23 (2014-03-12) Reply-To: geda-user AT delorie DOT com Errors-To: nobody AT delorie DOT com X-Mailing-List: geda-user AT delorie DOT com X-Unsubscribes-To: listserv AT delorie DOT com Precedence: bulk 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