MediaWiki API result

{
    "batchcomplete": "",
    "continue": {
        "gapcontinue": "Show_me_your_sp00nz",
        "continue": "gapcontinue||"
    },
    "warnings": {
        "main": {
            "*": "Subscribe to the mediawiki-api-announce mailing list at <https://lists.wikimedia.org/mailman/listinfo/mediawiki-api-announce> for notice of API deprecations and breaking changes."
        },
        "revisions": {
            "*": "Because \"rvslots\" was not specified, a legacy format has been used for the output. This format is deprecated, and in the future the new format will always be used."
        }
    },
    "query": {
        "pages": {
            "239": {
                "pageid": 239,
                "ns": 0,
                "title": "SM Barbie's Page",
                "revisions": [
                    {
                        "contentformat": "text/x-wiki",
                        "contentmodel": "wikitext",
                        "*": "'''Hi there!'''\n\nI am SM_Barbie (well ok I'm not) and\n# I live outside .nl\n# I want kaas\n# I have HFF.\n\nbye now."
                    }
                ]
            },
            "404": {
                "pageid": 404,
                "ns": 0,
                "title": "SPICE3-hacking primer",
                "revisions": [
                    {
                        "contentformat": "text/x-wiki",
                        "contentmodel": "wikitext",
                        "*": "__NOEDITSECTION__\n[[category:support]]\n\n[[File:Spice3girls.jpg|frame|the original Spice developers]]\n\n== Why, and what (not) to expect here ==\n\nI heard a lot about SPICE, and never used it outside of one of its many fuzzy packages, e.g. PSpice.\nGoogling by accident showed that SPICE-models representing simple circuits can be extremely short, so let's try.\n\n* If you spot an obvious mistake, please tell or change this page. \n* My goal here was clearly to simulate small and isolated parts of circuits using mainly passive components; a simple setup can be hacked together and simulated, well, within tens of seconds, really. \n* A lot of funny plots are about to greet your eyes. SPICE can do a '''lot''' more than all this. For example, subcircuits and actual component-models are not shown, since that's where I draw the line - I'll use a graphical front-end for that.\n* I use the '''ngspice''' incarnation on a NetBSD system, plotting directly to my monitor. I have not actually tested these examples on other SPICE3-incarnations.\n* No redundant text - learn by example, please, or '''RTFM''' (see below).\n\n== Real docs ==\n\nI don't like the original SPICE3 docs; I guess everything is explained, but it feels incoherent and IMHO it could have been twice as long without being too long.\n\n=== Original user's manual ===\n\n* [http://www.thedigitalmachine.net/reference/Spice_3f3_Users_Manual.pdf (an) original SPICE3 User's Manual]\n* [http://bwrc.eecs.berkeley.edu/Classes/IcBook/SPICE/ The Spice Page, with clickable version of the official user's manual]\n* [http://newton.ex.ac.uk/teaching/cdhw/Electronics2/userguide/ ...and another clickable version, elsewhere]\n\n=== Not-so-official documentation ===\n\n* [http://www.freeda.org/doc/SPICE/spice.pdf 2007 SPICE docs by Michael Steer for the fREEDA multi-physics simulator]\n* [http://ngspice.sourceforge.net/docs/ngspice-manual.pdf a recent ngspice manual (version 22plus)]\n\n=== Tutorials and introductions ===\n\n* [http://seit.unsw.adfa.edu.au/staff/sites/hrp/teaching/docs/spicetutorial.pdf very nice and short walkthrough of simulation of a circuit]\n* [http://www.seas.upenn.edu/~jan/spice/spice.overview.html SPICE - A Brief Tutorial; didn't read this one yet]\n* [http://zone.ni.com/devzone/cda/tut/p/id/5413 SPICE Simulation Fundamentals, didn't read this myself yet]\n\n=== Miscellaneous stuff ===\n\n* [http://www.ecircuitcenter.com/SPICEsummary.htm short SPICE devices and statements reference sheet]\n* [http://www.emwonder.com/spicemodels a lot of SPICE models/subcircuits for existing components]\n* [http://ngspice.sourceforge.net/ ngspice official site]\n\n== Examples ==\n\nTo 'run' these examples, copy-paste the given text to a file, then issue \"ngspice ''the_file_name''\", assuming you are using ngspice. And out will come a plot (or more plots) to the screen.\n\n=== Piece-wise linear: voltage-source with V/t-curve consisting of line segments ===\n\n{|\n | [[Image:1_pwl.png]]\n |\n<pre>\ntransient analysis: (P)iece-(W)ise (L)inear voltage-source\n\n*** Voltage source shows different ramps using 'pwl()'\n*\n*   Parms are tuples ( t, V ); i.o.w. at time 't', voltage is 'V'.\n*   Intermediate points are calculated using linear interpolation.\n\nv a 0 pwl( 0 -2   1m 6   2m 6  4m 5   4.001m 4   10m 0 )\nra a b 1k\nrb b 0 1k\n\n*** Show only the first 5 ms in steps of 1 us\n\n.control\ntran 1u 5m\nplot a b\n.endc\n\n.end\n</pre>\n |}\n\n=== AC (frequency-) analysis of a simple low-pass filter ===\n\n{|\n |[[Image:2_ac.png]]\n |\n<pre>\nAC-analysis: low-pass filter, 159 Hz cutoff freq\n\n*** Voltage-source has AC-component of 1V amplitude\n\nv a 0 dc 1 ac 1\nr a b 1k\nc b 0 1u\n\n*** Simulate using decade variation, 10 points per decade, \n*   with frequency varying from 0.1 Hz to 1 kHz\n\n.control\nac dec 10 .1 1k\nplot b\n.endc\n\n.end\n</pre>\n |}\n\n=== Initial conditions: giving a component an initial value ===\n\n{|\n |[[Image:3_ic.png]]\n |\n<pre>\ntransient analysis: discharging a cap with initial condition\n\n*** The cap has an (I)nitial (C)ondition of 1V\n\nr a 0 1k\nc a 0 1u ic=1\n\n*** Simulate first 10 ms in steps of 10 us, and (U)se initial conditions\n\n.control\ntran 10u 10m uic\nplot a\n.endc\n\n.end\n</pre>\n |}\n\n=== DC-sweep: ramp a (voltage-)source from start- to end-value ===\n\n{|\n |[[Image:4_dcsweep.png]]\n |\n<pre>\nDC-analysis: sweep on voltage source\n\n*** No need to specify voltage source properties since we'll do that in simulation\n\nv a 0\nr1 a b 1k\nr2 b 0 2k\n\n*** Sweep voltage source from 1 V to 3 V in steps of 0.1 V\n\n.control\ndc v 1 3 .1\nplot a b\n.endc\n\n.end\n</pre>\n |}\n\n=== Current-measurement using a dummy voltage-source (0V) ===\n\n{|\n |[[Image:5_imeas_1.png|thumb|Current through cap while charging]]\n |[[Image:5_imeas_2.png|thumb|Voltage over cap while charging]]\n |\n<pre>\ntransient analysis: current-measurement using 0V voltage source\n\n*** Dummy (0 V) voltage-source 'vsense' between resistor and cap\n\nv a 0 dc 1\nr a b 1k\nvsense b c dc 0\nc c 0 1u\n\n*** Show current through dummy voltage source, and (effectively) cap voltage\n*\n*   CAVEAT: 'uic' _must_ be added, else cap behaves as open circuit\n\n.control\ntran 10u 10m uic\nplot i( vsense )\nplot b\n.endc\n\n.end\n</pre>\n |}\n\n=== Pulsed source using nonzero rise- and fall-times ===\n\n{|\n |[[Image:6_pulse.png]]\n |\n<pre>\ntransient analysis: pulsed voltage-source\n\n*** Very convenient way to specify pulse-shaped stimulus.\n*\n*   Parms are <V_initial> <V_pulsed> <T_delay> <T_rise> <T_fall> <T_width>\n*   Intermediate points are calculated using linear interpolation.\n\nv a 0 pulse( 1 2 1m 2m .5m 2m )\n\n.control\ntran 10u 10m\nplot a\n.endc\n\n.end\n</pre>\n |}\n\n=== Physical pushbutton switch using helper voltage-source ===\n\n{|\n |[[Image:7_switch.png]]\n |\n<pre>\ntransient analysis: voltage-controlled switch over a resistor\n\n*** Simple 1:1 voltage-divider with N.O. pushbutton over 2nd resistor\n\nv a 0 1\nr1 a b 1k\nr2 b 0 1k\n\n*** Switch 's' with normal properties (e.g. threshold at 0V).\n*\n*   Voltage source generates a 'sloped' pulse crossing the\n*   0V-level, closing and opening the switch.\n\ns b 0 x 0\nvs x 0 dc 0 pulse( -.1 .1 2m 1m 2m 2m )\n\n*** Plot voltage over 2nd resistor and switch-control voltage\n\n.control\ntran 10u 10m\nplot b x\n.endc\n\n.end\n</pre>\n |}\n\n=== Voltage-controlled voltage-source as sad excuse for opamp-model ===\n\n{|\n |[[Image:8_vcvs.png]] Ok, admittedly this is a very boring graph; shown is the VCVS output-voltage, being exactly at 0.5 V. The voltage at 'b' is not plotted, but since no extra load on the 1:1 voltage-divider is created, it would also be at 0.5 V.\n |\n<pre>\ntransient analysis: VCVS with unity gain\n\n*** Simple 1:1 voltage divider acts as voltage-source with 1k \n*   internal resistance and 1k load (Vb = Vv / 2 )\n\nv a 0 1\nr1 a b 1k\nr2 b 0 1k\n\n*** VCVS with control-voltage Vb feeds r3, but doesn't \n*   add load to above circuit. This is an extremely simple\n*   (and wrong) way to model a voltage-follower or analog buffer.\n\ne c 0 b 0 1\nr3 c 0 1k\n\n.control\ntran 10u 10m\nplot c\n.endc\n\n.end\n</pre>\n |}\n\n----\n\nHave fun -- [[User:Michai|Michai]]"
                    }
                ]
            }
        }
    }
}