diff options
Diffstat (limited to 'help/C/oregano.xml')
| -rw-r--r-- | help/C/oregano.xml | 447 |
1 files changed, 447 insertions, 0 deletions
diff --git a/help/C/oregano.xml b/help/C/oregano.xml new file mode 100644 index 0000000..5d36977 --- /dev/null +++ b/help/C/oregano.xml @@ -0,0 +1,447 @@ +<?xml version="1.0"?> +<!DOCTYPE article PUBLIC "-//OASIS//DTD DocBook XML V4.1.2//EN" + "/usr/share/xml/docbook/custom/mathml/1.0/dbmathml.dtd" + [ + <!ENTITY legal SYSTEM "legal.xml"> + <!ENTITY appversion "0.1"> + <!ENTITY manrevision "0.1"> + <!ENTITY date "15 November 2009"> + <!ENTITY app "<application>Oregano</application>"> +]> +<article id="index" lang="en"> + <articleinfo> + <title><application>Oregano</application> User's Guide</title> + <copyright> + <year>2009</year> + <holder>Marc Lorber</holder> + </copyright> + <copyright> + <year>2003</year><year>2004</year> + <holder>LUGFi</holder> + </copyright> + <copyright> + <year>1999</year><year>2001</year><year>2002</year> + <holder>Richard Hult</holder> + </copyright> + <publisher> + <publishername> LUGFI </publishername> + </publisher> + + <authorgroup> + <author> + <firstname>Marc</firstname> <surname>Lorber</surname> + <affiliation> + <address><email>Lorber.Marc@wanadoo.fr</email></address> + </affiliation> + </author><author> + <firstname>Ricardo</firstname> <surname>Markiewicz</surname> + <affiliation> + <address><email>rmarkie@fi.uba.ar</email></address> + </affiliation> + </author> + </authorgroup> + <revhistory> + <revision> + <revnumber>Oregano Manual V 0.1</revnumber> + <date>2009</date> + <revdescription> + <para role="author">Marc Lorber</para> + </revdescription> + </revision> + <revision> + <revnumber>Oregano Manual V 0</revnumber> + <date>2004</date> + <revdescription> + <para role="author">Ricardo Markiewicz</para> + </revdescription> + </revision> + </revhistory> + + <releaseinfo> + Oregano is a tool for schematic capture and simulation + of electronic circuits. It simplifes design of simple circuits + by letting the user draw the circuit and then simulate its + electrical characteristics. + + This document is mostly meant to be an introduction + for someone who already is familiar with circuit simulation + and wants to try out Oregano. + </releaseinfo> + <!-- An address can be added to the publisher information. If a role is + not specified, the publisher/author is the same for all versions of the + document. --> + + &legal; + <!-- This file contains link to license for the documentation (GNU FDL), and + other legal stuff such as "NO WARRANTY" statement. Please do not change + any of this. --> + + <legalnotice> + <title>Feedback</title> + <para>To report a bug or make a suggestion regarding the + <application>Oregano</application> application or + this manual, follow the directions in the <ulink + url="ghelp:oregano-feedback" type="help">Oregano Feedback Page</ulink>. + </para> + </legalnotice> + </articleinfo> + + + +<!-- ============= Document Body ============================= --> + + <sect1 id="Spice"> + <title><emphasis>Spice</emphasis>: circuit simulation program</title> + <para><emphasis>Spice</emphasis> is a general-purpose circuit simulation program for nonlinear DC, nonlinear + transient, and linear AC analyses. Circuits may contain resistors, capacitors, inductors, + mutual inductors, independent voltage and current sources, four types of dependent sources, + lossless and lossy transmission lines (two separate implementations), switches, uniform + distributed RC lines, and the five most common semiconductor devices: diodes, BJTs, JFETs, + MESFETs, and MOSFETs.</para> + <para><emphasis>Spice</emphasis> has built-in models for the semiconductor devices, and the user need specify + only the pertinent model parameter values. The model for the BJT is based on the + integral-charge model of Gummel and Poon; however, if the Gummel-Poon parameters are not + specified, the model reduces to the simpler Ebers-Moll model. In either case, charge-storage + effects, ohmic resistances, and a current-dependent output conductance may be included. The + diode model can be used for either junction diodes or Schottky barrier diodes. The JFET model + is based on the FET model of Shichman and Hodges. Six MOSFET models are implemented: MOS1 + is described by a square-law I-V characteristic, MOS2 [1] is an analytical model, while MOS3 + [1] is a semi-empirical model; MOS6 [2] is a simple analytic model accurate in the short-channel + region; MOS4 [3, 4] and MOS5 [5] are the BSIM (Berkeley Short-channel IGFET Model) and BSIM2. + MOS2, MOS3, and MOS4 include second-order effects such as channel-length modulation, + subthreshold conduction, scattering-limited velocity saturation, small-size effects, and + charge-controlled capacitances.</para> + <sect2 id="analyses-types"> + <title>Types of analyses</title> + + <sect3 id="dc-analyses"> + <title>DC analyses</title> + <para>The DC analysis portion of <emphasis>Spice</emphasis> (.DC) determines the DC operating point of the circuit + with inductors shorted and capacitors opened. The DC analysis options are specified on the .DC, + .TF, and .OP control lines. A DC analysis is automatically performed prior to a transient analysis + to determine the transient initial conditions, and prior to an AC small-signal analysis to determine + the linearized, small-signal models for nonlinear devices. If requested, the DC small-signal value + of a transfer function (ratio of output variable to input source), input resistance, and output + resistance is also computed as a part of the dc solution. The DC analysis can also be used to + generate dc transfer curves: a specified independent voltage or current source is stepped over a + user-specified range and the DC output variables are stored for each sequential source value. + </para> + </sect3> + + <sect3 id="ac-analyses"> + <title>AC Small-Signal Analysis</title> + <para>The AC small-signal portion of <emphasis>Spice</emphasis> (.AC) computes the AC output variables as a function of + frequency. The program first computes the DC operating point of the circuit and determines linearized, + small-signal models for all of the nonlinear devices in the circuit. The resultant linear circuit is + then analyzed over a user-specified range of frequencies. The desired output of an AC small-signal + analysis is usually a transfer function (voltage gain, trans-impedance, etc). If the circuit has only + one AC input, it is convenient to set that input to unity and zero phase, so that output variables + have the same value as the transfer function of the output variable with respect to the input.</para> + </sect3> + + <sect3 id="transient-analysis"> + <title>Transient analysis</title> + <para>The transient analysis portion of <emphasis>Spice</emphasis> (.TRAN) computes the transient output variables as a + function of time over a user-specified time interval. The initial conditions are automatically + determined by a DC analysis. All sources which are not time dependent (for example, power supplies) + are set to their DC value. The transient time interval is specified on a .TRAN control line. </para> + </sect3> + + <sect3 id="pole-zero-analysis"> + <title>Pole-Zero Analysis</title> + <para>The pole-zero analysis portion of <emphasis>Spice</emphasis> (.PZ) computes the poles and/or zeros in the small-signal + AC transfer function. The program first computes the DC operating point and then determines the linearized, + small-signal models for all the nonlinear devices in the circuit. This circuit is then used to find the + poles and zeros of the transfer function. + </para> + <para>Two types of transfer functions are allowed: one of the form (output voltage)/(input voltage) and + the other of the form (output voltage)/(input current). These two types of transfer functions cover all + the cases and one can find the poles/zeros of functions like input/output impedance and voltage gain. + The input and output ports are specified as two pairs of nodes. + </para> + <para>The pole-zero analysis works with resistors, capacitors, inductors, linear-controlled sources, + independent sources, BJTs, MOSFETs, JFETs and diodes. Transmission lines are not supported. + </para> + <para>The method used in the analysis is a sub-optimal numerical search. For large circuits it may + take a considerable time or fail to find all poles and zeros. For some circuits, the method becomes + "lost" and finds an excessive number of poles or zeros. + </para> + </sect3> + + <sect3 id="small-signal-distorsion-signal"> + <title>Small-Signal Distortion Analysis</title> + <para>The distortion analysis portion of <emphasis>Spice</emphasis> (.DISTO) computes steady-state harmonic and + intermodulation products for small input signal magnitudes. If signals of a single frequency are + specified as the input to the circuit, the complex values of the second and third harmonics are + determined at every point in the circuit. If there are signals of two frequencies input to the circuit, + the analysis finds out the complex values of the circuit variables at the sum and difference of the input + frequencies, and at the difference of the smaller frequency from the second harmonic of the larger + frequency. </para> + <para>Distortion analysis is supported for the following nonlinear devices: diodes (DIO), BJT, JFET, + MOSFETs (levels 1, 2, 3, 4/BSIM1, 5/BSIM2, and 6) and MESFETS. All linear devices are automatically + supported by distortion analysis. If there are switches present in the circuit, the analysis continues + to be accurate provided the switches do not change state under the small excitations used for distortion + calculations. </para> + </sect3> + + <sect3 id="sensistivity-analysis"> + <title>Sensitivity Analysis</title> + <para><emphasis>Spice</emphasis> will calculate (.SENS) either the DC operating-point sensitivity or the AC small-signal + sensitivity of an output variable with respect to all circuit variables, including model parameters. + <emphasis>Spice</emphasis> calculates the difference in an output variable (either a node voltage or a branch current) + by perturbing each parameter of each device independently. Since the method is a numerical approximation, + the results may demonstrate second order affects in highly sensitive parameters, or may fail to show very + low but non-zero sensitivity. Further, since each variable is perturb by a small fraction of its value, + zero-valued parameters are not analyized (this has the benefit of reducing what is usually a very large + amount of data). </para> + </sect3> + + <sect3 id="noise-analysis"> + <title>Noise Analysis</title> + <para>The noise analysis portion of <emphasis>Spice</emphasis> (.NOISE) does analysis device-generated noise for the given + circuit. When provided with an input source and an output port, the analysis calculates the noise + contributions of each device (and each noise generator within the device) to the output port voltage. + It also calculates the input noise to the circuit, equivalent to the output noise referred to the specified + input source. This is done for every frequency point in a specified range - the calculated value of the noise + corresponds to the spectral density of the circuit variable viewed as a stationary gaussian stochastic + process. </para> + <para>After calculating the spectral densities, noise analysis integrates these values over the specified + frequency range to arrive at the total noise voltage/current (over this frequency range). This calculated + value corresponds to the variance of the circuit variable viewed as a stationary gaussian process. + </para> + </sect3> + </sect2> + + <sect2 id="temperatures-analysis"> + <title>Analyses at different temperatures</title> + <para>All input data for <emphasis>Spice</emphasis> is assumed to have been measured at a nominal temperature of 27°C, which + can be changed by use of the TNOM parameter on the .OPTIONS control line. This value can further be + overridden for any device which models temperature effects by specifying the TNOM parameter on the model + itself. The circuit simulation is performed at a temperature of 27°C, unless overridden by a TEMP parameter + on the .OPTIONS control line. Individual instances may further override the circuit temperature through + the specification of a TEMP parameter on the instance. + </para> + <para>Temperature appears explicitly in the exponential terms of the BJT and diode model paras. In + addition, saturation currents have a built-in temperature dependence. The temperature dependence of the + saturation current in the BJT models is determined by: + </para> + <center> + <para>I<subscript>S</subscript>(T<subscript>1</subscript>) = I<subscript>S</subscript>(T<subscript>0</subscript>)*(T<subscript>1</subscript><superscript>XTI</superscript>/T<subscript>0</subscript>) + *exp(q*E<subscript>G</subscript>*(T<subscript>1</subscript>*T<subscript>0</subscript>)/(k*T<subscript>1</subscript>-T<subscript>0</subscript>)) </para> + </center> + <para>where k is Boltzmann's constant, q is the electronic charge, E<subscript>g</subscript> is the energy gap which is a model + parameter, and XTI is the saturation current temperature exponent (also a model parameter, and usually + equal to 3). + </para> + <para>The temperature dependence of forward and reverse beta is according to the formula: + </para> + <para>B(T<subscript>1</subscript>) = B(T<subscript>0</subscript>)* T<subscript>1</subscript><superscript>XTB</superscript>/T<subscript>0</subscript></para> + <pre> + XTI + |T | | E q(T T )| + 1 g 1 0 + I (T ) = I (T ) |--| exp|-----------| + S 1 S 0 + |T | |k (T - T )| + 0 1 0 + </pre> + <para>COUCOUCOUCOUCOIU</para> + + <mml:mrow> + <mml:mi>x</mml:mi> + <mml:mo>=</mml:mo> + <mml:mfrac> + <mml:mrow> + <mml:mrow><mml:mo>-</mml:mo><mml:mi>b</mml:mi></mml:mrow> + <mml:mo>±</mml:mo> + <mml:msqrt> + <mml:mrow> + <mml:msup><mml:mi>b</mml:mi><mml:mn>2</mml:mn></mml:msup> + <mml:mo>-</mml:mo> + <mml:mrow><mml:mn>4</mml:mn><mml:mi>a</mml:mi><mml:mi>c</mml:mi></mml:mrow> + </mml:mrow> + </mml:msqrt> + </mml:mrow> + <mml:mrow><mml:mn>2</mml:mn><mml:mo>⁢</mml:mo><mml:mi>a</mml:mi></mml:mrow> + </mml:mfrac> +</mml:mrow> + + <para>COUCOUCOUCOUCOIU</para> + + <para>where T<subscript>1</subscript> and T<subscript>0</subscript> are in kelvin, and XTB is a user-supplied model parameter. Temperature effects + on beta are carried out by appropriate adjustment to the values of BF, ISE, BR , and ISC (<emphasis>Spice</emphasis> model + parameters BF, ISE, BR, and ISC, respectively). + </para> + <para>Temperature dependence of the saturation current in the junction diode model is determined by: </para> + <para>I<subscript>S</subscript>(T<subscript>1</subscript>) = I<subscript>S</subscript>(T<subscript>0</subscript>)*(T<subscript>1</subscript><superscript>XTI</superscript>/T<subscript>0</subscript>) + *exp(q*E<subscript>G</subscript>*(T<subscript>1</subscript>*T<subscript>0</subscript>)/(k*T<subscript>1</subscript>-T<subscript>0</subscript>)) </para> + + <pre> + XTB + |T | + 1 + B(T ) = B(T ) |--| + 1 0 + |T | + 0 + </pre> + + + <para>where N is the emission coefficient, which is a model parameter, and the other symbols have + the same meaning as above. Note that for Schottky barrier diodes, the value of the saturation current + temperature exponent, XTI, is usually 2. + </para> + <para>Temperature appears explicitly in the value of junction potential, U (in <emphasis>Spice</emphasis> PHI), for all the + device models. The temperature dependence is determined by: + </para> + + <pre> + XTI + --- + N + |T | | E q(T T ) | + 1 g 1 0 + I (T ) = I (T ) |--| exp|-------------| + S 1 S 0 + |T | |N k (T - T )| + 0 1 0 + </pre> + <para>where k is Boltzmann's constant, q is the electronic charge, Na is the acceptor impurity density, + Nd is the donor impurity density, Ni is the intrinsic carrier concentration, and Eg is the energy gap. + </para> + <para>Temperature appears explicitly in the value of surface mobility, M0 (or UO), for the MOSFET model. + The temperature dependence is determined by: + </para> + <para>R(T) = R(T<subscript>0</subscript>) [1 + TC<subscript>1</subscript> (T - T<subscript>0</subscript> ) + TC<subscript>2</subscript> (T - T<subscript>0</subscript>)<superscript>2</superscript>] + </para> + <pre> + + | N N | + a d + kT |------ | + U(T) = -- log 2 + q e |N (T) | + i + </pre> + + + <para>The effects of temperature on resistors is modeled by the formula: + </para> + <para>I<subscript>S</subscript>(T<subscript>1</subscript>) = I<subscript>S</subscript>(T<subscript>0</subscript>)*(T<subscript>1</subscript><superscript>XTI</superscript>/T<subscript>0</subscript>) + *exp(q*E<subscript>G</subscript>*(T<subscript>1</subscript>*T<subscript>0</subscript>)/(k*T<subscript>1</subscript>-T<subscript>0</subscript>)) </para> + <pre> + M (T ) + 0 0 + M (T) = ------- + 0 1.5 + | T| + |--| + |T | + 0 + </pre> + + + + <para>where T is the circuit temperature, T<subscript>0</subscript> is the nominal temperature, and TC<subscript>1</subscript> and TC<subscript>2</subscript> are the first- + and second-order temperature coefficients. + </para> + </sect2> + + <sect2 id="convergence"> + <title>Convergence</title> + <para>Both dc and transient solutions are obtained by an iterative process which is terminated when both + of the following conditions hold: + </para> + <orderedlist> + <listitem> + <para>The nonlinear branch currents converge to within a tolerance of 0.1% or 1 picoamp (1.0<superscript>-12</superscript>A), whichever + is larger.</para></listitem> + <listitem><para>The node voltages converge to within a tolerance of 0.1% or 1 microvolt (1.0<superscript>-6</superscript>V), whichever is larger. + </para> + </listitem></orderedlist> + <para>Although the algorithm used in <emphasis>Spice</emphasis> has been found to be very reliable, in some cases it fails to + converge to a solution. When this failure occurs, the program terminates the job. + </para> + <para>Failure to converge in dc analysis is usually due to an error in specifying circuit connections, + element values, or model parameter values. Regenerative switching circuits or circuits with positive feedback + probably will not converge in the dc analysis unless the OFF option is used for some of the devices in the + feedback path, or the .NODESET control line is used to force the circuit to converge to the desired state. + </para> + </sect2> + + + </sect1> + + <sect1 id="getting-started"> + <title>Getting Started with Oregano</title> + + <para>When you first start &app;, you will be presented to an + empty sheet, where you can place circuit components and connect + them with wires. To place a component, also known as 'part', + first select one in the part browser on the right hand side of + the application window. Then press the 'Place' button, or double-click + the selected part. You can also drag the part preview and drop it + on the sheet.</para> + + <figure id="general-view"> + <title>&app; oregano: main window</title> + <screenshot><graphic fileref="figures/oregano-main-window.png" format="PNG"></graphic> + </screenshot> + </figure> + + <para>When you have some parts placed on the sheet, you can start + connecting them with wires. Select the wire tool on the toolbar, + and click on the sheet where you want the wire to start. Then + click where you want to fixate the wire.</para> + + <para>Make sure you connect at least one ground node to the circuit, + as this is neccessary to perform a simulation.</para> + + </sect1> + + <sect1 id="editing"> + <title>Editing the Circuit</title> + + <para>There are a few accelerator keys that can help editing the + circuit:</para> + + <variablelist> + <varlistentry><term>Ctrl-A</term><listitem><para>Select all objects on the sheet</para> + </listitem></varlistentry> + + <varlistentry><term>Ctrl-Shift-A</term><listitem><para>Deselect all objects</para> + </listitem></varlistentry> + + <varlistentry><term>r</term><listitem><para>Rotate the selected objects 90 degrees clockwise</para> + </listitem></varlistentry> + + <varlistentry><term><Del></term><listitem><para>Delete the selected objects</para> + </listitem></varlistentry> + + <varlistentry><term>l</term><listitem><para>Place the currently selected part</para> + </listitem></varlistentry> + + </variablelist> + + <para>Parts and wires can be selected by clicking on them, and by holding the + Shift-key while clicking, you can select multiple parts and wires. You can + also select objects by 'rubber-banding': hold down the mouse button while dragging + the pointer over the objects that you wish to select.</para> + + </sect1> + + <sect1 id="simulation"> + <title>Simulation</title> + + <para>When you have a circuit and wish to run a simulation, either press the + simulate button on the toolbar or select + <guimenu>Tools</guimenu>-><guimenuitem>Simulation</guimenuitem>. + The simulation then starts and you can follow the progress on the dialog box + that pops up.</para> + + <para>If you want to change the simulation parameters, select + <guimenu>Settings</guimenu>-><guimenuitem>Simulation Settings</guimenuitem>. + </para> + + </sect1> +</article> |