Table of Contents
- 1. Warning
- 2. Installation
- 3. Starting of the program
- 4. Workflow and data flow
- 5. Overview screen layout
- 6. Number format
- 7. Schematic editor
- 8. Diagrams
- 9. Analysis tables
- 10. Formula component
- 11. Text component
- 12. Small signal analysis / frequency analysis (AC)
- 13. Small signal models
- 14. Analysis
- 15. Feedback Analysis
- 16. Examples
- 17. Small signal parameter determination
- 18. What's coming in the release
- 19. Appendix
- 20. Bibliography
1 Warning
This is an experimental prototype. Expect the software to crash, the computer to freeze and have to be restarted. Do not leave other applications running, which may cause damage or data loss. No guarantee is given for the functionality of the software or correctness of the results. You install and use the software at your own risk.
2 Installation
2.1 Requirements
- PC with at least 4 GB RAM
- Mouse
- Windows or Linux 64-Bit
- Current Browser (FF 93, Chrome 95.0.4638.69, Edge 92.0.902.62)
2.2 Linux
See Demo.
2.3 Windows
See Demo.
3 Starting of the program
- Open a command line (shell)
- Start ./sylinaserver in the command line
- Open localhost:7788 in the browser
4 Workflow and data flow
With the Sylina prototype it is important to have an idea of how the parts of the software work together, since wrong user input is often not yet checked.
Sylina consists of a solver and a browser window (GUI). The solver gets the circuit with the values and the desired analysis method from the GUI. It performs the analysis and returns the results on request. To do this, it stores various data internally.
Figure 1: overview and data flow
In Figure 1 a typical process is represented by the numbers.
- Load selected circuit The necessary data is collected in the analysis dialog.
- Analyze The circuit and the analysis method is sent to the solver, which carries out the analysis. The data is stored in the solver.
- Set Values Sets the values for the components in the solver. This is used to weight the results and draw curves.
- The results are queried for formulas or curves and displayed in the GUI. The data in the solver is also accessed for formula transformations such as toR.
- Curves are generated from the formula table or the formulas.
The second step, Analyze, is crucial. It is the actual analysis and computationally intensive. If it fails, no solution can be found.
The prototype does not yet coordinate the steps and does not warn of wrong processes. The user has to take care that the analysis, setting values and querying results are based on the same data in the solver.
5 Overview screen layout
Figure 2: Drag & Drop a formula onto a row
Menu | Submenu | Action |
---|---|---|
Circuit | Add Circuit | Add circuit editor |
Tools | Open tool dialog | |
Models | Open models dialog | |
Diagrams | Bode | Add Bode diagram |
PZ | Add PZ diagram | |
Nyqusit | Add Nyquist diagram | |
Text | Add text component | |
Formula | Add formula component | |
Analyze | Open the analysis dialog | |
Log | Open and start the log dialog |
The screen is organized into rows, columns and items. The items are circuits, diagrams, tables, formulas and texts.
When a new element is created, it is inserted on a new line. The position of the new line is either after the line with the element that triggered the action or after the top visible line.
The rows can be moved up and down using drag & drop.
Elements can be moved to a new line or positioned in an existing line using drag & drop.
The positioning is not entirely free. This allows for quick arranging. The layout is more based on a document than on the usual window/dialog scheme.
This puts all the circuits, diagrams, formulas, and annotations on one page for analysis.
6 Number format
The decimal seperator is the dot . in Sylina.
A digital group seperator does not exist.
The following formats are allowed
Examples | |
---|---|
integer | 123 |
decimal | 3.14 |
E notation | 1.23e3 |
Abbreviations like in SPICE e.g. k, u, m for kilo, mirco and milli are not allowed.
This abbreviations will be available in the release version.
7 Schematic editor
Figure 3: Add a circuit editor
Circuit | Add Circuit adds a circuit component.
With Circuit | Tools or a right click with the mouse in the circuit editor opens the tool dialog.
Figure 4: Circuit editor and tool dialog
First, an action is selected, which is then executed when you click in the editor. E.g. adding a transistor or rotating an element.
The zoom and clear actions are carried out immediately.
If there are several circuit editors, exactly one is selected. Recognizable by the red header. The actions of the tool dialog apply to the selected circuit editor.
A circuit editor is selected by clicking in the circuit editor.
Items in the tool dialog
Icon | Key | Action | Icon | Key | Action | Icon | Key | Action |
---|---|---|---|---|---|---|---|---|
Esc | Neutral | r | Resistance | Voltage controlled current source | ||||
+ | Zoom in | l | Inductance | Current controlled voltage source | ||||
- | Zoom out | c | Capacitor | Nullor element | ||||
0 | Normal size | g | Ground component | DC voltage | ||||
e | Edit values | Net component | AC voltage | |||||
m | Move element | n | NPN transistor | Voltage measurement | ||||
t | 90° rotation | p | PNP transistor | DC current | ||||
v | Vertical mirroring | Opamap | AC current | |||||
h | Horizontal mirroring | JNFET | Current measurement | |||||
Del | Delete item | NMOS | Input impedance measurement | |||||
Multiple selection | PMOS | Transformer 2 windings | ||||||
Clear circuit | Diode | Transformer 3 windings | ||||||
w | New connection | Voltage controlled voltage source | GFT component | |||||
Text component | Current controlled current source | Tian component |
7.1 Add elements
An element is selected in the tool dialog or by the corresponding key.
With a click in the circuit editor, the element is then created at this position.
7.2 Create connections
Figure 5: Draw connection
To establish connections, Wire is selected or the w key is pressed. By clicking in the editor and moving the mouse, the connection is drawn with a right-angled course. One click keeps the last kink.
Double-click to end drawing of the current connection.
When the connection touches an element's pin, the two are connected.
To link the current connection to another connection, click on it.
If the pins of elements are on top of each other, they are also connected. But be careful if an element is moved, this connection is lost.
7.3 Select / move elements
Elements can be selected and moved with or the m key.
Clicking on the element selects it. A selected element turns blue.
Multiple elements can be selected by pressing the Ctrl key at the same time. The selection is canceled by clicking on the blank area of the circuit.
Figure 6: Select and move connecting wire
A connecting wire is selected and moved.
The connections are lost.
Figure 7: Select and move connection point
A connection point is selected and moved.
The connected connection wires are also moved.
The direct connection to pins of elements is lost.
Figure 8: Select and move resistance
A resistance is selected and moved.
The connected connecting wires are also moved.
7.4 Rotate / Mirror elements
Rotate is selected with or the t (turn around) key.
Clicking on an element rotates it by 90°.
selects mirroring on the vertical axis.
selects mirroring on the horizontal axis.
Clicking on an element mirrors it accordingly.
7.5 Edit values
There are two options for editing elements.
Figure 9: Element Value
With the edit mode is selected.
Clicking on the element opens the editing dialog.
Figure 10: Table with values
With Circuit | Values, a table with all elements of the circuit is added to the editor. The values can be changed there.
Multiple data sets can be stored in the table. The name of the data set is in the combo box. With Save, the data set in the table is applied to the circuit and becomes the active data there. Delete deletes the data set. At least one set must be preserved.
You can change the name of the data set in the combo box. If the data set with the name already exists, the values in this data set are saved with Save. If the data set with the name does not exist, a new data set with this name is created.
The name of the active data set is displayed in the circuit editor header.
When analysing a circuit, the active data set is used.
8 Diagrams
There are Bode, Nyquist and pole-zero diagrams.
One diagram is active at a time. Clicking on the diagram activates it.
A new curve is drawn in the active diagram. If no corresponding diagram exists, a new diagram is created.
8.1 Bode plot
Figure 11: Bode plot
The magnitude is displayed in the upper part.
The axis can be scaled logarithmically, in dB or linearly.
The frequency axis can be displayed in angular frequency rad/s or as frequency Hz.
In the lower part, the phase is displayed in degrees.
With Zoom, an area can be enlarged with the mouse.
With Fit, the axes are set in such a way that all curves are visible.
When a new curve is added to the diagram, the axes are not adjusted. The curves can be made fully visible by Fit or manually in the configuration dialog.
The configuration dialog opens with Config or a right-click in the diagram.
Figure 12: Bode axes configuration
The axes for the Bode diagram can be set in the Axes tab of the configuration dialog.
With Apply, the set values are applied to the diagram.
Field | Description |
---|---|
min | Start value for the respective axis |
max | End value for the respective axis |
ticks | Spacing of the labeled points on the axis. |
For logarithmic scales it is a factor, for linear scales it is an amount | |
mticks | Distance of the unlabeled points on the axis |
unit | Rad/s or Hz for the frequency axis |
type | Logarithmic, dB or linear |
Figure 13: Bode configuration dialog graph
In the Graphs tab, the name of the curve and the color can be changed.
With X the curve is deleted.
8.2 Nyquist plot
Figure 14: Nyquist plot
The Nyquist plot is a parametric representation of the transfer-function.
The real part is horizontal and the imaginary part is vertical. The curve runs from the start frequency to the end frequency.
The axes are linear.
The presentation is very simple. Orbits at infinity and mirror image of negative frequencies are not shown.
Since only a limited number of points are calculated, it can sometimes look a bit angular. This can be improved by recalculating the curve for a smaller frequency range. See also Release.
With Zoom, an area can be enlarged with the mouse.
With Fit, the axes are set in such a way that all curves are visible.
The configuration dialog opens with Config or a right-click in the diagram.
Figure 15: Nyquist configuration dialog axes
Field | Description |
---|---|
min | Start value for the x and y axis |
max | End value for the x and y axis |
ticks | Spacing of the labeled points on the axes/curve |
mticks | Distance of the unlabeled points on the axes/curve |
unit | Rad/s or Hz for the frequency label of the curve |
With Apply, the set values are applied to the diagram.
Figure 16: Nyquist configuration dialog graph
In the Graphs tab, the name of the curve and the color can be changed.
With X the curve is deleted.
8.3 Pole-Zero plot
Figure 17: Pole-Zero plot
The poles and zeros of the transfer-function are displayed here.
The real part is horizontal and the imaginary part is vertical.
The axes are linear.
With Zoom, an area can be enlarged with the mouse.
With Fit, the axes are set in such a way that all curves are visible.
The configuration dialog opens with Config or a right-click in the diagram.
Figure 18: PZ configuration dialog axes
Field | Description |
---|---|
min | Start value for the x and y axis |
max | End value for the x and y axis |
ticks | Distance between the labeled points on the x and y axis |
mticks | Distance between the unlabeled points on the x and y axis |
With Apply, the set values are applied to the diagram.
Figure 19: Pole-Zero values
In the configuration dialog Tab Graphs the name and the color of the poles and zeros can be changed.
With X the poles and zeros are deleted.
With Values the numerical values of the poles and zeros are displayed in a text component.
9 Analysis tables
Figure 20: Table of results
Above the table is the name with the frequency for the weighting.
The table shows the numerator terms on the left and the denominator terms on the right.
Menu opens a dialog with which the selected terms can be displayed in a formula.
Menu | Description |
---|---|
Select all | All terms in the table are selected |
Unselect | Reset the selection |
Menu | Opens the table dialog |
Field | Description |
---|---|
cb | Checkbox to select a row |
tn*s | Weight of the term with the frequency calculated in the numerator |
td*s | Weight of the term with the frequency calculated in the denominator |
exn | Exponent of the s terms |
tn | Weight of the term without frequency |
Numerator | Term in the numerator |
Denominator | Term in the denominator |
Figure 21: Table dialog
On the left you can see the table dialog, which was opened by clicking on Menu.
The table can be edited further when the dialg is open.
With To Formula the selected terms from the table are displayed in a formula.
The name appears in the formula with Name := ….
The two lines with Select are only there to conveniently make a selection. With Select, the corresponding number in the numerator and denominator is selected in the table.
Element | Description |
---|---|
Select all | All terms in the table are selected |
Unselect all | All terms are reset |
To Formula | The selected terms are displayed in a formula component |
Source | Associated table with [number] |
Name | Name of the formula |
numerator terms | Number of terms in the numerator that are selected with Select |
denominator temrs | Number of terms in the denominator that are selected with Select |
Select | See line numerator terms / denominator terms |
10 Formula component
Figure 22: Formula
A formula appears in the formula component. The actual formula can be preceded by a name with name :=.
Text and Html can be used to switch between a pure text view and a structured Html view.
Under the Formula menu are listed actions that are performed on the formula. The result appears in a new formula.
Some actions use the data in the solver. These must match the formula. See also Workflow.
Menu | Submenu | Description |
---|---|---|
Text | Display as text | |
Html | Display formatted as Html | |
Formula | plot | Opens the plot dialog |
simplify | Formula is simplified. Mainly by reduction. | |
toR | Conductances (GRx) are converted into resistances and the formula is simplified | |
RR | Open RR dialog for RR analysis | |
normalize | The formula is brought to the form | |
subst | Variables in the formula are replaced | |
eval term | Variables in the formula are replaced with numbers. order is preserved | |
eval | Entire formula is calculated and displayed as numbers (except s). | |
collect s | The formula is displayed sorted by the exponent of s. | |
clone | The same formula is displayed in a new formula. |
Prototype. The transformations of the formulas sometimes lead to strange representations. E.g. signs are not reduced or obvious simplifications are not made.
11 Text component
The text component simply displays text. You can switch between plain text and html. See also Release.
12 Small signal analysis / frequency analysis (AC)
Sylina does a symbolic small signal analysis in the frequency domain for linear circuits. With Spice, this corresponds to the numerical AC analysis. The result is a transfer-function in the frequency domain with the Laplace variable s.
Common analysis methods in electronics is analysis in the time domain (transients) and small signal analysis in the frequency domain. For the interpretation and application of the results, one must be clear about the advantages and disadvantages of the respective analysis methods.
In small signal analysis, non-linear components such as semiconductors are linearized at the operating point. The non-linear components are replaced by linear models. The analysis is then carried out on this linearized circuit. The results are only valid as long as the components show a sufficiently linear behavior with regard to voltage and current around the operating point. So normally only for small signals.
Despite this limitation, the analysis is usefull because the results are much easier to manipulate. One obtains a rational polynomial in s.
When analysing in the time domain, one obtains a system of differential equations that can often only be solved numerically.
13 Small signal models
With Circuit | Models opens a dialog with the existing models.
In the following, only a small selection of the models is shown. See the models table for a complete list.
13.1 Elementary components
The elementary components are R, L, C, VCVS, VCCS, CCVS, CCCS, nullor, voltage source and current source.
They are used to perform the actual analysis and the small signal models are built from them.
13.2 NPN, PNP
Figure 23: Small signal model npnvi
npnvi is a simple model for a transistor.
13.3 Operational amplifier
Figure 24: Ideal opamp
The ideal operational amplifier is modeled with a nullor. In the resulting formula the operational amplifier does not appear as an amplification factor or similar quantity. There it is taken into account with its ideal properties in the "structure".
If it is to be considered as an active element in an RR analysis, a model with explicit gain (such as opvg) must be chosen.
Figure 25: Opamp with gain and input and output resistance
opvgr is an operational amplifier with input and output resistance and gain.
Figure 26: Opamp with single pole
In the opvlp1rc model, a pole is created with an RC element and shielded from the output with a nullor.
The parameters for determining the pole are the gain and the frequency w1 in rad/s at which the pole becomes effective.
Figure 27: Parameters for the single pole opamp
The following relationship applies
The values of an opamp with open gain of 1e6 and a pole at 62.8 rad/s give a
13.4 Transformer
There are many ways to model transformers. See Albach.
SYLINA only analyses linear small signal models. i.e. non-linear factors such as hysteresis and saturation are not taken into account.
13.4.1 Two windings
Figure 28: Ideal transformer
An ideal transformer only transforms the voltage and current ratios of the primary and secondary side.
In contrast to a real transformer, direct voltages and direct currents are also transmitted.
An ideal transformer is used in many models to build a more realistic model.
Figure 29: Model t2wa
This model consists of a leakage inductance Ls and a magnetizing inductance Lp and an ideal transformer.
The following relationships exist with the coupling factor k and the self-inductances L1 and L2:
Figure 30: Model t2wb
The t2wb model is based on the matrix
The connection between the coupling factor k and the self-inductances L1 and L2 is as follows:
Figure 31: Model t2wc
The t2wc model is basically the same as the t2wa model. However, L1, L2 and k are input parameters and Ls, Lp and n are calculated internally from them.
The parameter k is only valid in the range 0 < k < 1.
I.e. Ls or Lp must not become zero.
13.4.2 Three windings
The models for a three-winding transformer are similar to those for two-windings.
The following relationships are used.
The coupling factors must be so that Ls1, Ls2, Ls3 and Lh do not become zero.
14 Analysis
The analysis dialog is opened in the main menu with Analyze.
14.1 Important prerequisites for the analysis
For the analysis, it is necessary that the components in the circuit have a unique name. E.g. two resistors may not have the same name 'R1'.
Furthermore, at least one ground component (GND) must be present. Without a GND component, the analysis will produce meaningless results.
If the circuit is separated by components such as a transformer, VCVS or nullor, several GND's may be necessary. Circuit seperation can also be caused by analysis components such as ZIN.
If in doubt, it is better to place several GND components to force a defined potential.
In the SYLINA prototype, it must be ensured that the entries are correct. There are no warnings for invalid values.
14.2 Analysis init tab
On the Init tab, Load selected circuit is used to load the data of the active circuit into the analysis dialog.
Figure 32: Analysis dialog
Field | Description |
---|---|
Circuit | Name of the loaded circuit |
Analyze | Selection Input->Output for a transfer-function |
or an analysis element from the circuit. | |
Depending on the selection, the following entries change | |
Input | Input source |
Output | Output measurement |
Method | Name of the analysis if an analysis item is selected |
Optional additional fields | Depending on the analysis and method |
Advanced Settings EET: | (must be empty for normal analysis) |
Open | List of elements to be removed |
Short | List of elements to be shorted |
Nullify out | For an NDI, the output pins for a nullator |
Nullify in | For an NDI, the input pins for a norator |
The analysis is started with Analyze. This is the critical action. Plots or formulas can only be generated later if Analyze is successful.
In the Messages list at the bottom of the dialog you will see a nr Send Analyze init. After a successful analysis, a nr Receive Analyze init Success appears. The SYLINA prototype has to wait for the answer.
If successful, the numerical values of the components in the circuit are then set in the solver with Set Values. Numerical values are necessary for plots, but also to weight the symbolic terms.
14.3 Analysis formula tab
Figure 33: Analysis dialog formula
After the Analyze has been successfully carried out in the Init tab, the result can be shown in a table in the Formula tab.
Field | Description |
---|---|
Name | Name for the generated result table |
num terms | Number of terms in the result numerator |
den terms | Number of terms in the denominator for the result |
s | Frequency at which the result is weighted |
in (rad/s) or f (Hz). |
With Statistic, information about the solution is shown in the Messages list. Among other things, the number of terms in the numerator and denominator. This allows you to better estimate how many terms make sense in the resulting formula table.
Depending on the circuit, there can be thousands of terms in the solution. But such a large number makes no sense for a formula. Therefore it is better to load only a small number of terms into the result table.
With To table, the result table is created with the specified number of terms. See analysis table.
14.4 Analysis Plot Bode/PZ tab
Figure 34: Analysis dialog plot Bode/PZ
Various curves can be generated in the Plot Bode/PZ tab.
The complete solution that is stored internally is taken into account. These curves can thus be used as a reference to compare approximate solutions with.
A new curve is drawn in the respective active diagram. If no corresponding diagram exists, a new diagram is created.
In the diagram, the axis may have to be adjusted (Fit) so that the curve is fully visible.
Element | Description |
---|---|
Bode | Generates a Bode diagram |
Nyquist | Generates a Nyquist diagram |
PZ | Generates a pole-zero diagram |
Name | Name of the curve |
from..to.. | Frequency range in which the curve is calculated |
Color | Color for the curve |
14.5 Analysis Plot RR tab
Figure 35: Analysis dialog RR
A curve for the return ratio (RR) analysis can be drawn here as a Bode or Nyquist plot. See Analysis RR for details.
The denominator of the complete solution is the network determinant . From this, the RR can be determined according to Bode.
With entries in Num zero and Den zero it is determined for which active component a complete or partial RR is generated.
In the usual analysis, Num zero is empty and Den zero contains an active component or all active components.
If there are multiple components, the names are separated by spaces.
Element | Description |
---|---|
RR Bode | Generates a Bode curve for RR |
RR Nyquist | Generates a Nyquist curve for RR |
Name | Name of the curve in the diagram |
Num zero | For a partial RR, the names of the active elements in the numerator to be zeroed |
Den zero | The names of the active elements in the denominator to be zeroed |
from..to.. | Frequency range in which the curve is drawn |
Color | Color of the curve |
15 Feedback Analysis
15.1 General Feedback Theorem GFT
See Middlebrook GFT chapter 13, page 35, 43.
The relevant formulas are:
where T is the loop gain. Depending on the circuit and the injection point, simplified equations result.
With the GFT component the subexpressions and can be determined. The desired expressions can then be formed with this.
For an example see simple feedback circuit GFT.
15.2 Tian
See Tian.
After that, the formula for the loop gain is:
The subexpressions and can be determined with the TIAN component. T can then be derived from this.
15.3 Return Ratio (RR)
A transfer-function can be represented as a rational polynomial in s.
The denominator of the transfer-function is the so called network determinant .
This is independent of the input sources of the circuit and only determined by the topology of the circuit. Voltage sources are shorted and current sources are opened. Different transfer-functions have the same network determinant if the topology of the circuit stays the same.
The network determinant is used in the return ratio (RR) calculation.
I.e. first a transfer-function is determined and the denominator of this is used as the network determinant.
15.3.1 Single loop
Normal feedback analysis works with a single loop.
You look for a place where you interrupt all feedback paths.
If that doesn't work, look for a dominant loop and break it. The remaining loops are considered as stable and are ignored.
In the return ratio analysis, an active element is neutralized purely algebraically (set to zero) and a loop calculation is carried out. You calculate the return difference and the return ratio, which are related as follows:
Return Difference and Return Ratio .
For single loops, the RR corresponds to the loop gain.
For an example see simple feedback circuit RR.
15.3.2 Multiple loops
With multiple loops, it is not possible to interrupt all feedback paths at one point. Normal feedback analysis is therefore not possible. Most of the time you then focus on a dominant loop.
However, the return ratio (RR) analysis is possible. Using the Return Difference (RD) leads to simpler expressions.
Partial return differences can be formed. This is done by neutralizing a subset of the active elements.
A complete RD can be formed with (with three active elements):
If you want to calculate the complete T, most of it cancels out and you get
In order to form the partial RR, you specify in the RR dialog which active elements in the numerator and denominator are to be deactivated. For a single loop or for a complete RR, you only enter elements for the denominator (See Figure 35).
Example:
In a circuit there are three active elements Q1, Q2 and Q3.
The partial T is to be determined when Q1 is already neutral and Q3 remains active. Q2 is the element to be examined. That makes:
For this analysis, enter Q1 in the numerator and Q1 Q2 in the denominator in the dialog.
16 Examples
16.1 Simple common emitter amplifier
Figure 36: Common emitter amplifier
Three analyses are drawn in the circuit.
The transfer-function Vout/Vin, the input resistance Zin and the output resistance Zout.
For Zin and Zout, the ZIN analysis component is used.
Figure 37: Small signal parameters Q1
The small signal parameters for the npn transistor Q1, determined from a Spice simulation. See parameters from Spice.
Figure 38: Small signal model npnvi2
The small signal equivalent circuit for the npnvi2 model.
16.1.1 Transfer-function
To determine the transfer-function, the input source and the output measurement are specified in the analysis dialog.
Figure 39: Analysis dialog
Load selected circuit
Select analysis method
Select input source and output measurement
Then press the Analyze button. Wait until the response "Receive…" comes in the message text below. Now press the Set Values button.
Figure 40: ce1 plot dialog
Switch to the Plot Bode/PZ tab and enter a function name, start and end frequency and then press the Bode button.
Figure 41: ce1 Bode plot
The Bode plot appears. This is the complete solution. So no approximation. The plot is the reference for simplified formulas.
Figure 42: ce1 formula dialog
You can now develop a formula on the Formula tab. With the Statistic button you get the number of terms in the numerator and denominator in the message text. If this is in the range of less than 100 terms, you can still work well with the entire expression. The To table button outputs the expression in a table. The frequency at which the formula is to be developed is also specified. A favorable frequency can be found using the Bode plot.
20 terms for numerator and denominator were selected. The values in the table are weighted at 10e6 rad/s.
Figure 43: ce1 table
As a test, one can first select everything in the table with Select all and plot to compare the curve with the complete curve. This is the red curve.
Figure 44: ce1 table and plot
If this curve looks good, you can only select the values with the large values and then plot them. For the green curve, 1 term in the numerator and three terms in the denominator were chosen. This fits quite well around the chosen frequency of 10e6 rad/s and also includes the pole at around 100e6 rad/s.
Figure 45: Tabel formula dialog
From this, the formula is now displayed via To Formula.
Figure 46: Formula straight from the table
The first formula (Fig. 46) is still not reduced and with conductances for the resistors.
Figure 47: After simplify
The second formula (Fig. 47) is simplified with Simplify.
Figure 48: After toR
The third formula (Fig. 48) is given by toR with impedances and is also simplified.
From the formula one sees that the gain at 10e6 rad/s is mainly determined by -(RC * gm$Q1) and the pole at 100e6 rad/s by CBC$Q1 * RC.
In this case, you can also output the exact formula. However, this becomes large even with this small circuit.
16.2 Input impedance / output impedance common emitter amplifier
Figure 49: Common emitter amplifier
The analysis components Zin and Zout are already included in the circuit for determining the input and output resistance.
Analysis components are usually in a neutral state where the circuit is not affected. If they are used for analysis, the circuit will be adjusted accordingly.
Figure 50: ZIN neutral state
The ZIN component in the neutral state.
Figure 51: ZIN active state
The ZIN component in the active state.
Figure 52: Analysis Zin dialog
The selection of the ZIN component in the analysis dialog.
Figure 53: Zin and Zout plot
The Bode plot for the input resistance Zin and the output resistance Zout.
In the following the frequency 10e3 rad/s is selected for the formula.
A formula table is generated at 10e3 rad/s and the largest term in the numerator and denominator is selected from the table. The formula is formed from this and converted into impedances (toR). This gives the following formulas.
Figure 54: Simplest Zin and Zout formulas
This is of course only the simplest approximation, but fits very well in the mid frequency range.
16.2.1 Differential amplifier
Figure 55: Differential amplifier
The circuit is not completely symmetrical. RC1 and RC2 are slightly different and so are CBC$Q1 and CBC$Q2. This is particularly noticeable in the common mode gain.
First, the differential gain is examined. With an Analyse Vin-Vout | Set Value | Plot Bode the exact differential gain is plotted.
Figure 56: Exact differential gain
This is fairly flat in the middle frequency response. To develop a formula, the weighted table is created at 100e3 rad/s.
Figure 57: Differential gain at 100e3 rad/s.
Figure 58: Approximate differential gain at 100e3 rad/s
For a simple formula, two terms each in the numerator and denominator are selected and output as a formula. With toR this formula is simplified. The value fits well for the middle frequency range.
Figure 59: Circuit in common mode (CM).
For common mode gain, the connection is changed to CM. See red circle. CM is a net label, i.e. CM at Vin and CM on the right are connected. This means that Vin is routed equally to both inputs. The rest of the values remain unchanged.
Figure 60: Exact common mode gain
With an Analyse Vin-Vout | Set Value | Plot Bode the exact common mode gain is plotted (1: cm blue).
Ideally, the common mode gain should be very small. Here it is already quite large due to small asymmetries (RC, CBC). At 20e6 rad/s it goes close to 0.8.
For 100e3 rad/s and 20e6 rad/s the weighted tables are created and terms are selected. The selected terms are checked in the Bode plot. In Figure 60, the red curve is for the 100e3 rad/s selection and the green curve for the 20e6 rad/s selection in the tables.
Figure 61: Weighted table at 100e3 rad/s.
Figure 62: Weighted table at 20e6 rad/s.
This gives the following two approximate formulas.
Figure 63: Simple approximate formula at 100e3 rad/s.
Figure 64: Approximate formula at 20e6 rad/s.
If you take a closer look, you can see that the common mode amplification is 0 for a symmetrical circuit according to the formulas. In a real circuit, there are of course always small asymmetries.
16.3 Extra Element Theorem (EET) & Co
There are a number of analysis methods in which modified circuits are generated from a circuit and simpler analysis are used from them. The overall result is then formed from the simpler partial results.
One of them is the Extra Element Theorem (EET) [MidEET], [Vorp], [BassoLin]. Sylina supports the analysis with the EET (still very simple implemented in the prototype).
Figure 65: EET circuit
This is the circuit to be examined. C1 is the extra element.
Figure 66: H0 dialog
To determine H0, capacitor C1 is removed.
This is done by entering C1 in the Open field.
Then the transfer-function from Vin to Vout is determined.
Figure 67: H0 formula
The table and formula for H0.
Figure 68: Zd dialog
For the determination of Zd, C1 is left removed and the resistance across C1 is determined. The component Zc1 is used for this.
Figure 69: Zd table
The table and formula for Zd. Zd is 0.
Figure 70: Zn dialog
The analysis dialog for the determination of Zn. C1 and Vin are removed. Vin must be removed because a voltage source will be shorted if not used directly in the analysis. A nullor is placed across the input Vin and the output Vout for the null double injection.
Figure 71: Zn null double injection NDI by nullor
Here you can see that C1 and Vin are removed and the Nullor is connected. The output is nulled and the corresponding voltage/current is injected at the input by the norator. The resistance is determined via C1 with Zc1. Current is injected through Zc1 as a second source.
Figure 72: Zn table
The table and formula for Zn.
The complete transfer-function according the EET is calculated as follows:
mit und
The following formulas in Fig. 73 are from the direct determination of the transfer-function with Sylina. As you can see, the results agree.
Figure 73: Transfer-function determined directly
16.4 Active filter
Figure 74: Active filter
The circuit is a state variable filter. It has low pass (LP), band pass (BP) and high pass (HP) outputs.
Figure 75: Bode plot
The three transfer-functions for LP, BP and HP in the Bode plot.
Figure 76: Pole-Zero plot
The pole-zero plot for the bandpass.
At 100 rad/s the formula tables and from them the formulas for the LP, BP and HP are formed.
Figure 77: Low pass formula
Figure 78: Highpass formula
Figure 79: Bandpass formula
Note the minus signs in the numerator and denominator [18].
16.5 Feedback analysis GFT
See Middlebrook GFT for details.
With the GFT component the subexpressions and can be determined.
Figure 80: Simple feedback circuit
In the circuit above, GFT1 is at an ideal injection point just after a controlled voltage source. There is only one loop and also no signal path from output to input in the main branch via E2 to E1. The Tvfwd method is therefore sufficient to determine the loop gain. A voltage is injected in between X and W, and the returned voltage between W and Y is measured. Vin has 0V.
Figure 81: GFT Tvfwd dialog
The component GFT1 and the method Tvfwd are selected in the analysis dialog. Then Analyze and Set Values are pressed.
Figure 82: Plot dialog
The values for the Bode plot are set in the Plot Bode/PZ tab.
Figure 83: GFT Tvfwd Bode plot
And with a click on Bode, the Bode plot is drawn.
Figure 84: GFT Tvfwd Nyquist plot
Clicking on Nyquist displays the Nyquist plot.
The circuit has a phase margin of 15 degrees. I.e. it will oscillate lightly. There is a pole at about 100e3 and 1e6 rad/s through R1,C1 and R2,C2. C3 provides a zero at about 100e6 rad/s and a pole at 1e9 rad/s.
Figure 85: GFT Tvfwd formula
16.6 Feedback analysis return ratio (RR)
The same circuit is analysed with RR as before with the GFT.
Figure 86: Simple feedback circuit
Figure 87: Vin Vout analysis
First a normal transfer-function is derived, here Vin to Vout.
Figure 88: Formula table dialog
The transfer-function is created in a table with To table.
Figure 89: RR formula from table
All entries in the table are selected first. The values for the RR analysis are set in the RR tab in the table menu.
For a complete RR, the active elements E1 and E2 are entered in Den zero.
The formula is then created by clicking on Formula.
Figure 90: RR formula with -1 term at the end
The formula is first created as with the return difference F. This is because you may want to continue working with F.
If one is only interested in RR the formula has to be simplified with simplify or toR.
Figure 91: RR formula after several simplifications and toR
This is the same formula developed by GFT Tvfwd. In general, both methods do not give the same solution. This is the case here because the circuit is so simple, has an ideal injection point, and there is only one loop. Bode Plot and Nyuist Plot are of course the same as in the GFT example.
16.7 Colpitts oscillator
A loop gain analysis with GFT and RR is performed with a Colpitts oscillator.
Figure 92: Colpitts oscillator circuit
Since a transfer-function is required for RR, the current source Iin is included. It is important that such a source does not affect the circuit when it is inactive. A current source is open when inactive.
Figure 93: Colpitts transfer-function Vout/Iin
The Bode plot of the transfer-function Vout / Iin.
Figure 94: Colpitts RR dialog
The values for the RR analysis.
The active element J1 must be entered in the Den zero field.
Figure 95: Colpitts RR and GFT Tvfwd Bode plot
The Bode plot of the RR analysis in blue.
Another Tvfwd analysis of GFT1 is shown in red.
The curves are almost identical up to 100e6 rad/s.
The reason is that we have almost a single loop and an ideal injection point for GFT1.
This is only disturbed at higher frequencies by the parasitic capacitances in J1.
Figure 96: Colpitts RR and GFT Tvfwd Nyquist plot
The Nyquist plot for the RR and Tvfwd.
The curve is angular because only a few points are calculated and these are simply connected.
The critical point at -1 is encircled and the circuit is unstable.
However, this is desirable for an oscillator.
16.8 Transformer
Only the linear behavior of transformers is analysed.
Figure 97: Circuit with ideal transformer
An ideal transformer T1 with two serial resistors Rs1 and Rs2 and a load RL.
Figure 98: Parameters for the ideal transformer
The ideal transformer T1 has a 1:10 ratio from primary to secondary.
Figure 99: Model for the ideal transformer
The small signal model for the ideal transformer. The primary voltage is transformed 1:n to the secondary side. The current with 1 : 1/n.
Figure 100: Bode plot for the ideal transformer
The transfer-function from Vin to Vout in blue and the input resistance zin in red.
Figure 101: tfid formula
The transfer-function Vin to Vout. Rs1 forms a voltage divider together with the transformed impedance from the output. This only achieves a transfer factor of approx. 9.
Figure 102: zinid formula
The resistances on the secondary side are transformed with 1/n^{2} to the primary side and appear there with 10.01 ohms.
Now the transformer T1 is replaced by the model t2wa.
Figure 103: t2wa model
The t2wa model has a main inductance Lp and a leakage inductance Ls and an ideal transformer.
Figure 104: Parameters for the transformer model t2wa
The parameters for the transformer T1 with the model t2wa.
Figure 105: tf1 Bode
The Bode plot of the transfer-function Vin to Vout with the transformer model t2wa.
The transfer-function is now clearly frequency dependent.
Figure 106: tf1 approx
An approximate formula at 10e3 rad/s. No difference to the complete solution can be seen in the Bode plot.
Figure 107: zin1 Bode
The Bode plot for zin with the model t2wa for T1. The complete solution in blue and an approximate solution in red.
Figure 108: zin1 approx
A formula for an approximate solution at 10e3 rad/s. No difference to the complete solution can be seen in the Bode plot.
17 Small signal parameter determination
Sylina does a small signal analysis.
To do this, the circuit is linearized at the operating point and the parameters for the small-signal models used must be set.
Very simple approximations for determining these parameters for a BJT, a MOSFET and a JFET are given below.
See [Thompson], [Tietze/Schenk], [Vladimirescu].
Even if you get specific values for the parameters from the data sheets, curves or SPICE parameters, you should always be aware of the device variation and the dependence of the parameters on the voltages, currents and temperature.
Figure 109: Active region of a transistor
The approximations apply to the active region of the transistors and only to individual transistors. The influence of the substrate on integrated circuits is not taken into account.
The circuit is at the desired operating point and, in particular, the collector current or drain current of the transistor is known.
17.1 Small signal models
The parameters are determined for the following small-signal models.
17.1.1 BJT
Figure 110: NPN BJT small signal model
Formula for IC
17.1.2 MOSFET
Figure 111: NMOSFET small signal model
Formula for ID in the active region
17.1.3 JFET
Figure 112: JNFET small signal model
Formula for ID in the active region
17.2 Determination based on experience
At the beginning of a circuit design, there are often no special components and therefore no data sheets or SPICE models.
In this case one will often use typical values. It is reasonable to differentiate between small signal transistors and power transistors.
In the further course of the design, these values are refined and special types are selected.
17.2.1 BJT, typical values
Parameter | Small signal transistor | Power transistor |
---|---|---|
Ic | 1 mA | 1 A |
gm | 0.038 S | 38 S |
beta | 100..400 | 50..200 |
V_{BE} | 0.7 V | 0.7..1 V |
RBE | 5 kOhm | 5 Ohm |
Rx | 20..500 Ohm | 0.1..50 Ohm |
CBE | 20 pF | 20 nF |
CBC | 2 pF | 2 nF |
Ro | 100 kOhm | 100 kOhm |
17.2.2 MOSFET, typical values
parameter | Small signal transistor | Power transistor |
---|---|---|
Id | 10 mA | 1 A |
gm | 0.05 S | 2 S |
CGD | 4 pF | 200 pF |
CGS | 20 pF | 2000 pF |
RDS | 50 kOhm | 50 kOhm |
For small Id currents note the subthreshold effect.
17.2.3 JFET, typical values
Parameter | Small signal transistor |
---|---|
Id | 1 mA |
gm | 0.005 |
CGD | 2 pF |
CGS | 4 pF |
RDS | 50 kOhm |
17.3 Determination with a data sheet
17.3.1 BJT data sheet
Model | From the | ||
---|---|---|---|
parameter | Determination | Data sheet | Notes |
gm | . is the desired current in the operating point. | ||
RBE | or | , is the small-signal current gain with large device variation | |
Ro | is Early voltage | ||
Rx | 1. estimate | 20..500 Ohm | |
2. | Collector base time constant if given in the data sheet. | ||
CBC | For C_{obo} there is often a curve with values over the reverse voltage V_{BC}. | ||
CBE | The pn junction BE is in the forward direction. As a result, the value of Cibo does not fit well. | ||
and there is also the diffusion capacity. Therefore, CBE is determined via fT. |
17.3.2 MOSFET data sheet
Model | From the | ||
---|---|---|---|
parameter | Determination | Data sheet | Notes |
gm | 1. | is the desired current at the operating point | |
has large device variation | |||
2. | Curves | ||
RDS | 1. read from curves | ||
2. estimate | |||
CGD | large device variation | ||
CGS | large device variation |
17.3.3 JFET data sheet
Model | From the | ||
---|---|---|---|
parameter | Determination | Data sheet | Notes |
gm | is the desired current at the operating point | ||
is with | |||
has large device variation | |||
RDS | 1. read from curve | ||
2. estimate | |||
CGD | large device variation | ||
CGS | large device variation |
17.4 Determination with SPICE models
If SPICE models exist, it is better to run an .OP simulation and read the model parameters from it. The non-linearities are then taken into account. See OP-simulation.
The approximate formulas given are imprecise, especially for the capacitances.
17.4.1 BJT SPICE
Model | SPICE- | ||
---|---|---|---|
parameter | Determination | Parameter | Notes |
gm | . is the desired current at the operating point. | ||
RBE | BF | BF is the current gain. | |
Rx | Rx = RB | RB | |
Ro | VAF | VAF is Early voltage. | |
CBC | CJC, VJC, MJC | , smaller with larger . | |
Reverse pn-junction. | |||
VJC=0.75, MJC=1/3 | |||
CBE | 1. From simulation or data sheet | ||
2. | CJE, VJE, MJE | , smaller with larger . | |
TF | Forward pn-junction. | ||
CB is the difffusion capacitor. | |||
VJE=0.75, MJE=1/3 |
17.4.2 MOSFET SPICE
Model | SPICE | ||
---|---|---|---|
parameter | Determination | Parameter | Notes |
gm | KP, VTO | If W,L are not given then | |
RDS | LAMBDA | ||
CGD | CGD = CGDO * W | CGDO | Default W=100e-6 with LTspice. see .OPTIONS defw |
CGS | CGS = CGSO * W | CGSO | Default W=100e-6 with LTspice. see .OPTIONS defw |
17.4.3 JFET SPICE
Model | SPICE | ||
---|---|---|---|
parameter | Determination | Parameter | Notes |
gm | BETA | ||
RDS | LAMBDA | ||
CGD | Cgd | reverse pn-junction | |
CGS | Cgs | reverse pn-junction |
17.5 Small signal parameters from a SPICE simulation
With an .OP simulation, the small-signal parameters can be determined by simulation. This takes the non-linearities into account.
17.5.1 ngspice
In the following you can see the call of ngspice with an OP analysis and the output of the values for the diode d1. For detailed output see appendix Determining the operating point with Spice.
1: $: ngspice 2: $: ... 3: $: ngspice 15 -> source diode1.net 4: $: ... 5: $: ngspice 16 -> op 6: $: ... 7: $: ngspice 17 -> show d1 8: $: ...
17.5.2 LTspice
An OP analysis must be performed in LTspice. The result is then in the error log (View | SPICE Error Log).
Figure 113: LTspice OP analysis
17.5.3 Summary parameters with Sylina, ngspice and LTspice
In the table, the Sylina model parameters are compared with ngspice and LTspice OP values.
Model/Parameter | Sylina | ngspice | LTspice |
---|---|---|---|
Diode | R | 1/gd | Req |
C | cd | CAP | |
NPN, PNP | gm | gm | Gm |
RBE | 1/gpi | Rpi | |
CBE | cpi | Cbe | |
CBC | cmu | Cbc | |
beta | gm/gpi | BetaAC | |
Rx | 1/gx | Rx | |
Ro | 1/go | Ro | |
Re | 1/gm | 1/Gm | |
NMOS, PMOS | gm | gm | Gm |
RDS | 1/gds | 1/Gds | |
CGS | cgs | Cgsov | |
CGD | cgd | Cgdov | |
JFET | gm | gm | Gm |
RDS | 1/gds | 1/Gds | |
(M=1/2, PB=1) | CGS | Cgs | |
CGD | Cgd |
For detailed examples see appendix Determining the operating point with Spice.
18 What's coming in the release
- Better layout. More modern, lighter.
- Improved formula operations.
- Cursors for plots.
- Copy curves between diagrams.
- SPICE for determining the working point.
- Better subst for formulas.
- Editor for small signal models.
- Export to CAS (maxima, sympy,…).
- Export/import of netlists for SPICE.
- Weighted table for RR.
- Weighted table of formulas.
- Step and impulse response, numerical as a plot.
- root loci.
- Graphic elements in the circuit diagram (lines, circles,…).
- hierarchical schematics.
19 Appendix
19.1 Table of small signal models
Component | Model | Method | Description |
---|---|---|---|
Diode | dr | simply a R | |
Diode | drc | R and C | |
GFT | GFT | Hinf | see Middlebrook |
GFT | GFT | Tifwd | |
GFT | GFT | Tirev | |
GFT | GFT | Tnifwd | |
GFT | GFT | Tnirev | |
GFT | GFT | Tnvfwd | |
GFT | GFT | Tnvrev | |
GFT | GFT | Tvfwd | |
GFT | GFT | Tvrev | |
JNFET | jnfet1 | JNFET with Rpi, Cpi, Cu, gm, Ro | |
NMOS | nmos1 | NMOS with Rpi, Cpi, Cu, gm, Ro | |
PMOS | pmos1 | PMOS with Rpi, Cpi, Cu, gm, Ro | |
NPN | npnvi | Voltage controlled with Rpi, Cpi, Cu, gm | |
NPN | npnvi2 | Current controlled with extra Rx und Ro | |
NPN | npnt1 | T-Modell with beta, RE | |
NPN | npnii3 | Current controlled Rpi, beta, Ro | |
NPN | npnii4 | Current controlled with beta | |
PNP | pnpvi | Voltage controlled with Rpi, Cpi, Cu, gm | |
PNP | pnpvi2 | Voltage controlled with extra Rx und Ro | |
PNP | pnpt1 | T-Modell with beta, RE | |
PNP | pnpii3 | Current controlled Rpi, beta, Ro | |
PNP | pnpii4 | Current controlled with beta | |
OPAMP | opvid | Ideal Opamp | |
OPAMP | opvg | Opamp with gain | |
OPAMP | opvgr | Opamp with gain and input and output resistance | |
OPAMP | opvlp1rc | Opamp with a low pass from R,C | |
OPAMP | opvlp2rc | Opamp with two low passes from R,C | |
OPAMP | opvslp1 | Opamp with a low pass as formula | |
OPAMP | opvslp2 | Opamp with two low passes as formula | |
TRAFO | t2id | Ideal transformer with 2 windings | |
TRAFO | t2wa | Transformer with leakage and main inductance, n | |
TRAFO | t2wb | Transformer with L1, L2, M | |
TRAFO | t2wc | Transformer with L1, L2, k | |
T3W | t3id | Ideal transformer with 3 windings | |
T3W | t3wa | With leakage and main inductance, n2, n3 | |
T3W | t3wb | With L1,L2,L3,M12,M13,M23 | |
T3W | t3wc | With L1, L2, L3, k12, k13, k23 | |
TIAN | TIAN | Delta | See Tian |
TIAN | TIAN | Y1 | |
TIAN | TIAN | Y2 | |
ZIN | ZIN | Input impedance with Z = V/I |
19.2 Operating point determination with Spice
1: diode1.net 2: V1 N001 0 5 3: R1 N002 N001 4k 4: D1 N002 0 diode1 5: .op 6: .model diode1 D(IS=2.5n RS=.5 N=1.752 CJO=4p) 7: .end
1: ngspice 15 -> source diode1.net 2: 3: Circuit: * diode1.net 4: 5: ngspice 16 -> op 6: Doing analysis at TEMP = 27.000000 and TNOM = 27.000000 7: 8: No. of Data Rows : 1 9: ngspice 17 -> show d1 10: Diode: Junction Diode model 11: device d1 12: model diode1 13: thermal 0 14: vd 0.588959 15: id 0.00110262 16: gd 0.0243323 17: cd 6.16009e-12
1: Circuit: * diode1.net 2: 3: --- Diodes --- 4: Name: d1 5: Model: diode1 6: Id: 1.10e-03 7: Vd: 5.90e-01 8: Req: 4.11e+01 9: CAP: 6.16e-12
1: bjt1.net 2: R1 N001 N003 27k 3: R2 N003 0 10k 4: RC N001 out 1k 5: RE N004 0 220 6: Q1 out N003 N004 0 BJT1 7: V1 N001 0 5 8: V2 N002 0 AC 1 9: C1 N003 N002 10u 10: .op 11: .MODEL BJT1 NPN (IS=1e-14 VAF=100 BF=200 CJC=8e-12 CJE=12e-12 RB=10 RC=0.3 RE=0.2) 12: .end
1: ngspice 18 -> source bjt1.net 2: 3: Circuit: * bjt1.net 4: 5: ngspice 19 -> op 6: Doing analysis at TEMP = 27.000000 and TNOM = 27.000000 7: 8: No. of Data Rows : 1 9: ngspice 20 -> show q1 10: BJT: Bipolar Junction Transistor 11: device q1 12: model bjt1 13: ic 0.00260947 14: ib 1.29012e-05 15: ie -0.00262237 16: vbe 0.679635 17: vbc -1.13268 18: gm 0.100863 19: gpi 0.000498792 20: gmu 1e-12 21: gx 0.1 22: go 2.58024e-05 23: cpi 1.91279e-11 24: cmu 5.90451e-12 25: cbx 0 26: csub 0
1: Circuit: * bjt1.net 2: --- Bipolar Transistors --- 3: Name: q1 4: Model: bjt1 5: Ib: 1.29e-05 6: Ic: 2.61e-03 7: Vbe: 6.80e-01 8: Vbc: -1.13e+00 9: Vce: 1.81e+00 10: BetaDC: 2.02e+02 11: Gm: 1.01e-01 12: Rpi: 2.00e+03 13: Rx: 1.00e+01 14: Ro: 3.88e+04 15: Cbe: 1.91e-11 16: Cbc: 5.90e-12 17: Cjs: 0.00e+00 18: BetaAC: 2.02e+02 19: Cbx: 0.00e+00 20: Ft: 6.41e+08
1: jnfet1.net 2: J1 out N003 N004 jnfet1 3: V1 N001 0 12 4: V2 N002 0 AC 1 5: RL N001 out 2.2k 6: Rs N004 0 220 7: Rg N003 0 1Mega 8: C1 N003 N002 1u 9: .op 10: .MODEL jnfet1 NJF(IS=0.25p VTO=-1.5 BETA=3.0m RD=10 RS=10 CGS=4p CGD=4p) 11: .end
1: ngspice 18 -> source jnfet1.net 2: 3: Circuit: * jnfet1.net 4: 5: ngspice 19 -> op 6: Doing analysis at TEMP = 27.000000 and TNOM = 27.000000 7: 8: No. of Data Rows : 1 9: ngspice 20 -> show j1 10: JFET: Junction Field effect transistor 11: device j1 12: model jnfet1 13: vgs -0.581767 14: vgd -6.4099 15: ig -7.49163e-12 16: id 0.00252945 17: is -0.00252945 18: igd -6.6599e-12 19: gm 0.0055094 20: gds 0 21: ggs 1.00015e-12 22: ggd 1e-12
1: Circuit: * jnfet1.net 2: --- JFET Transistors --- 3: Name: j1 4: Model: jnfet1 5: Id: 2.53e-03 6: Vgs: -5.56e-01 7: Vds: 5.88e+00 8: Gm: 5.51e-03 9: Gds: 0.00e+00 10: Cgs: 3.18e-12 11: Cgd: 1.47e-12
20 Bibliography
- Manfred Albach, Induktivitäten in der Leistungselektronik, Springer Vieweg, 2017
- Christophe P. Basso, Linear Circuit Transfer Functions, Wiley, 2016
- Hendrik W. Bode, Network Analysis and Feedback Amplifier Design, van Nostrand, 1945
- Robert Fox, http://www.fox.ece.ufl.edu/Multiple-Loop_Feedback.html, 2014
- LTspice®, www.analog.com
- R. D. Middlebrook, Measurement of loop gain in feedback systems, International Journal of Electronics (volume 38, no. 4, 485-512), 1975
- R.D. Middlebrook, EET Chapter 8, 12, https://web.archive.org/web/20160401041428/http://ardem.com/D_OA_Rules&Tools/index.asp
- R. D. Middlebrook, GFT Chapter 13, https://web.archive.org/web/20160401041428/http://ardem.com/D_OA_Rules&Tools/index.asp
- R. D. Middlebrook, The GFT: A Final Solution for Design-Oriented Feedback Analysis, Ardem DVD, 2013
- R. D. Middlebrook, Technical Therapy for Analog Circuit Designers, Ardem DVD, 2013
- ngspice, http://ngspice.sourceforge.net/
- Marc Thompson, Intuitive Analog Circuit Design, Newnes, 2014, 2nd edition
- M. Tian, V. Visvanathan, J. Hantgan, K. Kundert Striving for Small-Signal Stability, Circuits & Devices, 2001
- U. Tietze, Ch. Schenk Halbleiter-Schaltungstechnik, Springer, 2010, 13. Aufl.
- A. Vladimirescu, THE SPICE BOOK, Wiley, 1994
- Vatché Vorperian, Fast analytical techniques for electrical and electronic circuits, Cambridge University Press, 2002
Last Change 2022-04-29