net= attribute mini-HOWTO 1. What is the net= attribute used for? 2. What is the format of the net= attribute? 3. How do you actually use the net= attribute 4. Caveats / Bugs 5. Example 6. Final notes The information in this document is current as of 19991011. 1. What is the net= attribute? The net= attribute is used to specify power, ground, and/or arbitrary nets in the gEDA system. The net= attribute is used instead some of the other systems of specifying power/ground (such as having power/ground pins on symbols or power boxes). Some devices have lots of power/ground pins and having all of these pins on the symbol would increase its size and make it unmanageable. The net= attribute is the power/ground specification of choice in the gEDA system because of its simplicity and versatility. Now having said all this, you can have power/ground pins on a symbol, but gnetlist will probably not recognize these nets connected to these pins as separate power/ground nets. Please keep this in mind as you draw symbols. 2. What is the format of the net= attribute? Attributes in the gEDA are simple text items which are in the form name=value. All proper attributes follow this form. Attribute names are always lower case, but the value can be upper or lower case. gnetlist and friends are case sensitive. Typically net/signal names by default are upper case. Attribute can be attached to an object or in certain cases (like the net= attribute) can be free floating (not attached to anything). The free floating attributes are also called toplevel attributes. The net= attribute is a text item which takes on the following form: net=signalname:pinname,pinname,pinname,... Where: net= The attribute name (always the same, lowercase) signalname The signal or net being defines (like +5V, GND, etc...) pinname The pin name (or number) which is assigned to this signal/net (or pin names/numbers) The signalname cannot contain the : character (since it's a delimiter). The pinname is the pin name (A1, P2, D1, etc...) or pin number (1, 2, 5, 13, etc...). The pinname cannot contain the , character (since it's also a delimiter). pinnames are typically the same sort of numbers/names like the pin#=# attribute (if your familiar with that attribute). You can only have ONE signalname per net= attribute, but you can have as many pinnames/numbers as you want. 3. How do you actually use the net= attribute You can place the net= attribute in several places. Here's the list so far: - Inside a symbol either as an attached attribute or an unattached attribute (toplevel attribute). Example which creates power/gnd nets: net=GND:7 or net=+5V:14 - Outside a symbol (which is instantiated on a schematic) attached as an attribute to override an existing net= created net/signal. Suppose a symbol has a net=GND:7 inside it already; attaching this to the symbol: net=AGND:7 overrides the GND net (on pin 7) calling it AGND and connects/associates it to pin 7. - Outside or inside a symbol to connect a net to a visible pin automatically. This is still untested and still might have some undesirable (negative) side effects. Use with caution. - Attached to one of those special power/gnd symbol (like vcc/gnd/vdd) and you can change what that symbol represents. You could change the ground symbol to create a net called DIGITAL_GND without editing the symbol (net=DIGITAL_GND:1). In the current symbol (19991011) library there are symbols named vdd-1.sym, vcc-1.sym, vee-1.sym, etc... which do not have a net= attribute inside, so you must attach the net= attribute yourself (in the schematic). There also symbols named 5V-minus-1.sym, 12V-plus-1.sym, 9V-plus-1.sym etc... which have the appropriate net= attribute in them already (can be overridden though). You can use these symbol as examples of how to use the net= attribute. You can have as many net= attributes as you want. Just remember that net= attributes attached to the outside of a symbol override any equivalent internal (inside the symbol) net= attributes. If you run into a case where this doesn't work, please let ahvezda@geda.seul.org. In fact, send any bug reports to that individual. 4. Caveats / Bugs The net= attribute/mechanism is fairly new, so there are bound to be bugs (many bugs). Here are some of the identified issues: - As of 19991011 almost all of the symbols in the standard library do not have the net= attribute or any other power/ground specifiers. Hopefully this will be updated sometime (any volunteers?). - Attach a special power symbol (vcc/gnd) to a already named net will alias (rename) that net to the signalname specified in the net= attribute (in/attached to the vcc/gnd symbol). You can override this (so the reverse is true) by playing with the "net-naming-priority". Be careful with this. There might be other "aliasing" issues which have not been identified yet. - Creating a net= attribute which associates a signal name with a pin which is already visible on the symbol, is probably a bad idea. This does work, but all the ramifications have not been explored yet. - It is probably a bad idea to have the same net= attribute attached several times. Ales has not formalized what happens in this case. Just remember that the net= attribute on the outside of a symbol should override the internal one. 5. Example Here's a schematic which uses standard symbols (note: the 7400 does not have the net= attribute inside yet). This schematic consists of a 7400 with the net= attributes attached for power and ground, One of the input pins grounded using a gnd symbol and the other at a logic one using the vcc symbol (with an attached net= attribute). One of the input net is labeled, but as you will see, the netname is replaced by the net= signal name (see above for more info on this). The output is pulled up with a pull up resistor which has power specified using the +5V symbol. [ Maybe insert picture of schematic as well ] -- Cut here -- v 19991011 C 38700 58100 1 0 0 7400-1.sym { T 39000 59000 5 10 1 1 0 uref=U100 T 38900 59500 5 10 1 1 0 net=GND:7 T 38900 59300 5 10 1 1 0 net=+5V:14 } N 38700 58800 37400 58800 4 { T 37600 58900 5 10 1 1 0 label=NETLABEL } N 37400 58800 37400 59200 4 N 38700 58400 37400 58400 4 N 37400 58000 37400 58400 4 C 37300 57700 1 0 0 gnd-1.sym C 37200 59200 1 0 0 vcc-1.sym { T 36800 59200 5 10 1 1 0 net=+5V:1 } N 40000 58600 41600 58600 4 { T 41200 58700 5 10 1 1 0 label=OUTPUT } C 40700 58800 1 90 0 resistor-1.sym { T 40800 59200 5 10 1 1 0 uref=R1 } N 40600 58800 40600 58600 4 N 40600 59900 40600 59700 4 C 40400 59900 1 0 0 5V-plus-1.sym -- Cut here -- gnetlist (using the geda netlist format) run using this sample schematic outputs this: -- Cut here -- START header gEDA's netlist format Created specifically for testing of gnetlist END header START components R1 device=RESISTOR U100 device=7400 END components START renamed-nets NETLABEL -> +5V END renamed-nets START nets +5V : R1 2, U100 14, U100 1 GND : U100 7, U100 2 OUTPUT : R1 1, U100 3 END nets -- Cut here -- Notice how NETLABEL was renamed (aliased to the +5V net). 6. Final notes Send all bugs to ahvezda@geda.seul.org or geda-dev@geda.seul.org (mailing list, please subscribe first) [I'm sure there's more to say here]