Circuit-breaker SPICE model

Circuit-Breaker Model for Over-Current Protection Simulation of DC Distribution Systems.

T. ROBBINS
TELSTRA RESEARCH LABORATORIES
BOX 249 ROSEBANK MDC, CLAYTON VICTORIA 3168, AUSTRALIA
Email: t.robbins@trl.oz.au

 

Abstract: This article describes an electrical model of a thermalmagnetic circuit-breaker that can accurately simulate characteristic behaviour over a wide range of overcurrents, including operation in the magnetic region. The model has been validated against measured waveforms from both a high-current DC test facility and a distributed power system rack. The circuit-breaker model can be coupled with other distribution component models to simulate the protection performance in telecommunications DC distribution systems.

 

1.Introduction

The design and analysis of over-current protection for telecommunication DC power systems can be greatly assisted by the use of a computer-aided simulation tool. However, a simulation is only as accurate as the component models and element values used to represent the real world. This article reports on the development of a circuit-breaker model that can accurately represent circuit-breaker behaviour over a wide range of overcurrents.

The performance of protection, distribution and storage devices significantly affects both the reliability and safety of the DC power system. Voltage excursions caused by an over-current instance can cause electronic equipment to malfunction due to over-voltage, and disrupt service due to under-voltage. Poor discrimination between protection devices can cause upstream device operation, resulting in major interruption to service. The rapid advancement of both computing power and analogue circuit simulation programs derived from SPICE software provides a relatively user-friendly environment for over-current protection design and analysis. This is advantageous as telecommunications power distribution systems are often large and complex, and developing an equivalent circuit model for a power system is not a trivial task.

The circuit-breaker model described in this article implements the enhanced modelling functions available with PSpice’s Analog Behavioural Modelling to include circuit-breaker current, time and arcing dependent characteristics. This model complements and extends previously published modelling work [1-2] by Telstra Research Laboratories on other power system components.

 

2.Circuit-Breaker Characteristic Operation

A typical thermal-magnetic circuit-breaker operates (trips) in two distinct modes; the thermal mode occurs for device currents from 1 up to about 10-15 times the rated setting current, and the magnetic mode occurs for all current levels above the thermal operating region. Characteristic current-time curves for the device operating in the thermal region can be approximated by an equation where i n t equals a constant, whereas in the magnetic region the operating time (typically <20ms) is not well defined in device data curves and specifications, as test circuits are based on rectified AC power sources which have typical rise times exceeding a few milliseconds.

The circuit-breaker model presented in this paper has been developed for a 125A moulded device (10kA fault rating), which is commonly used to protect individual battery strings within Telstra’s distributed power supplies.

For device operation in the thermal region, the characteristic i n t form of the current-time curve can be obtained from the device specification curve as shown in Figure 1. A value of n = 3.5 gives an adequate fit over the range of currents within the thermal operating region.

Fig.1 125A circuit-breaker current-time operating boundary curves (courtesy of GEC ALSTHOM AUSTRALIA).

Fig.1 125A circuit-breaker current-time operating
boundary curves (courtesy of GEC ALSTHOM
AUSTRALIA).

 

 

For device operation in the magnetic region, characteristic current-arc voltage-time behaviour has been observed for the circuit-breakers operating in a high-current DC test facility over a range of current levels and circuit time constants. At the start of such a fault instance, the current passing through the closed circuit-breaker contacts increases to a level where magnetic activation forces the contacts to open. As the contacts start to open an arc is developed which is inherently unstable and a complex voltage-current characteristic occurs as the arc progresses through to extinction.
For the 125A circuit-breaker operating in the magnetic region, the contacts are forced open when the current level typically rises above 2-4kA. Circuit-breaker operation was measured over a range of circuit conditions, such as:

· fast rates of current rise exceeding 10kA/ms, which resulted in short pre-arcing times of about 0.15- 0.2ms (eg. results from a test circuit with 5.4kA prospective current and 0.26ms time constant are shown in Figure 2).

· high prospective current levels exceeding 10kA, which result in pre-arcing times around 0.9ms for circuit time constants of about 1.2ms, as shown in Figure 3. It should be noted that special oscilloscope probing and current shunt techniques are required to record clean waveforms in the high transient noise environment that occurs in a high current test facility.

Fig.2 Measured current and voltage waveforms for a 125A circuit-breaker operating in 54VDC test circuit with 5.2kA prospective current and 0.25ms prospective time constant; 1kA/div current, 20V/div voltage and 0.5ms/div.

Fig.2 Measured current and voltage waveforms for
a 125A circuit-breaker operating in 54VDC test circuit
with 5.2kA prospective current and 0.25ms prospective
time constant; 1kA/div current, 20V/div voltage and
0.5ms/div.

Fig. 3 Measured current and voltage waveforms for a 125A circuit-breaker operating in 54VDC test circuit with about 12kA prospective current and about 1ms prospective time constant; 1kA/div current, 50V/div voltage and 0.5ms/div.

Fig. 3 Measured current and voltage waveforms for
a 125A circuit-breaker operating in 54VDC test circuit
with about 12kA prospective current and about 1ms
prospective time constant; 1kA/div current, 50V/div
voltage and 0.5ms/div.

FuseCircuit-breaker Model

Fuse Model For Over-Current Protection Simulation of DC Distribution Systems.

T. Robbins
Telecom Australia Research Laboratories
770 Blackburn Road, Clayton, 3168
Australia

 

Abstract: The design and analysis of over-current protection for telecommunication DC power systems can be greatly assisted by the use of a computer-aided simulation tool. This article reports on the development of a fuse model for SPICE derived software that can accurately represent characteristic fuse parameters. The fuse model can also be adapted to represent the operation of circuit breakers.

 

1.Introduction

The design and analysis of over-current protection for telecommunication DC power systems can be greatly assisted by the use of a computer-aided simulation tool. However, a simulation is only as accurate as the component models and element values used to represent the real world. This article reports on the development of a fuse model that can accurately represent fuse characteristics. The fuse model can also be adapted to represent the operation of circuit breakers.
The performance of over-current protection devices significantly affects both the reliability and safety of the DC power system. Voltage excursions resulting from the operation of a fuse during a short circuit can cause electronic equipment malfunction due to over-voltage, and disrupt service due to under-voltage. Poor discrimination between protection devices can cause upstream device operation, resulting in major interruption to service.

The rapid advancement of both computing power and analogue circuit simulation programs derived from SPICE software provide a user-friendly environment for over-current protection design and analysis. This environment is advantageous as telecommunications power distribution systems are often large and complex, and developing an equivalent circuit model for apower system is not a trivial task.

The analysis of DC distribution systems using computer simulation has been shown to provide fair agreement between simulated and experimental results [1,2,3]. However, the fuse models developed have not been able to accurately represent fuse characteristics. Typical parameters for a fuse operating in a circuit with a given time constant and prospective current are rated current ir, peak current ip, pre-arcing time tp, arcing time ta, total operating time tt= tp + ta, pre-arcing i²t (i²t)p, arcing i²t (i²t)a and total operating i²t (i²t)t= (i²t)p + (i²t)a. Figure 1 illustrates some of these parameters. The prospective current for a circuit is the maximum current that would be reached if the fuse did not operate.

The i²t or current-squared time rating is a commonly used fuse characteristic when operating current levels are much higher that the rated fuse current ir. The circuit time constant defines the ratio L/R, where L and R are the effective circuit inductance and resistance components in series with the fuse and energy source.

 

 

Typycal fuse parameters

Fig 1. Typycal fuse parameters

A fuse model is developed in Section 2 and model validation is undertaken in Section 3. Section 4 discusses the development of other DC power system component models for application to the analysis of over-current protection, and the paper is summarised in Section 5.

GPM-SurgeGenerator_page3_image4

SPICE simulation of a Combo Wave Generator.

Thanks for this article to ssleandro

 

In this article we ‘ll se how to implement a template for a Combination Wave Generator that can be a Surge Generator, a Line Impedance Stabilization Networks (LISN), motor control, ripple current, etc. This model can be very useful for hardware engineers which can utilize it in their projects to speed up project development. The platform used for the simulation is PSpice but
it can easily replicated in other SPICE simulation software.

 

The simplified model of the GPM consists of an High-Voltage source U, a charging resistor Rc, an energy storage capacitor Cc. This part of circuit is connected by a switch to 2 Pulse duration shaping resistors Rs, an impedance matching resistor Rm and a Rise time shaping indutor Lr, as in the picture below

 

 

GPM-SurgeGenerator_page3_image1

 

typical values of this components are:  Cc=7.76μF,  Rs1=14.8 Ohm,  Rm=1.05 Ohm,  Lr=9.74μH,  Rs2=23.3 Ohm. The peak voltage on Rs2 can be 1KV, 2KV,..6KV.

 

In the following schematic we set the high voltage with the initial condition of the CapacitorCc, for example for 6KV, we set 6300 in the PSpice IC field of the Cc component. We can adjust the time in U1 to make surge hit at 90/270 degree or whatever phase we want.

 

GPM-SurgeGenerator_page4_image1

 

GPM-SurgeGenerator_page4_image2

 

 

Calibration of Surge Generator.

The IEC/EN 61000-4-5 standars requires the following waveform of open-circuit voltage with no Coupling/Decoupling network (CDN) connected

 

GPM-SurgeGenerator_page5_image1

 

This is the result of the simulation that shows a voltage waveform that fullfills requirementof IEC/EN 61000-4-5

 

GPM-SurgeGenerator_page5_image2

 

 

Below the image of the waveform of short-circuit current with no CDN connected

 

GPM-SurgeGenerator_page6_image2

 

and here again the simulated results:

 

GPM-SurgeGenerator_page6_image1

 

Ipeak is about 1.5KA, T1 is 8uS and T2 is 20uS. The effective coupling impedance is 2Ohm. The simulated current waveform fulfills requirement of IEC/EN 61000-4-5 standards.

OrCAD PSpice Video Tutorials

Topic Video
Getting started with OrCAD Capture
OrCAD PSpice how to perform a Bias point analysis 1
OrCAD PSpice how to perform a Bias point analysis 2
OrCAD PSpice, how to perform a transient analysis
How to mark Voltage and Currents in OrCAD PSpice
How to perform a DC Sweep Analysis in PSpice OrCAD
Performing an AC Sweep Analysis in PSpice OrCAD
Using the Monte Carlo Analysis in PSpice OrCAD
Worst-Case Circuit Analysis with PSpice
A Differential Amplifier Analyzed with PSpice
How to design the current source for a Differential Amplifier with PSpice
A complete video tutorial from the schematic to the PCB layout with OrCAD PCB Editor

SPICE modeling of Magnetic Core from Datasheet

Vittorio Carboni

Department of Electronics and Automatic, University of Ancona 1999/2000

SPICE simulations and analisys by Ing. Cristoforo Baldoni

1. Switching  power supply: Choice of ferrite

2. Simplified calculation of the transformer

3. Transformer for Flyback converter: Calculation example

4. Transformer for Forward converter :Calculation example

5. Windings: Supports, wires and insulation

 

On what

How

With what

Skin and proximity effects

6. Let’ s complete the design of the flyback transformer

Primary

Secondary

Conclusions

7. Appendix

8. SPICE modeling of ETD49 N67 core from datasheet

9. Bibliography

 

1. Switching  power supply: Choice of ferrite

The first step in the design of the transformer is the choice of the ferrite as physical form,  type of material and dimensions. It’s a very important choice that characterizes the project as all subsequent calculations based on it. An error of assessment may lead, at the end of designing, to realize, for example, that the dimensions are not suitable: this means start again with considerable lost of time and resources.

The ferrites are characterized by very low losses at high frequencies, they are made with alloys of iron oxides and other metals such as zinc and manganese. The material is pulverized together with insulating oxides and then modeled using techniques typical of ceramics. This allows to make ferrites with a great variety of shapes and sizes and tolerances very restricted about magnetic and mechanically characteristics. They, also, can be machined with precision after the operation of the cooking.

The ferrites typically have a density of the saturation flux between 3 and 5 kGauss, also the presence of oxides increases its specific resistivity at very high levels thus allowing to reduce losses due to eddy currents. The available shapes include bars, toroids, EE EI and UI cores. The Curie temperature TC, namely the temperature at which the material loses its ferromagnetic properties, is between 100 and 300 ° C, depending on the type of material; the phenomenon is reversible, reducing the temperature to below the TC material regains its properties.

For low to medium power transformers E-Series is the best choice. As the acronym suggests, the magnetic core is composed of two elements in the shape of E. The two pieces forming the magnetic circuit, are slipped into the holder of the windings and locked in place with the clips and / or bonded with Araldite or other epoxy adhesives. The three contact surfaces of the half-cores are machined so as to reduce the roughness and therefore contain to negligible size the not intentional air gap . In some cases the air gap is desired, this can be obtained realizing the central column of the half-core shorter than outer ones.

figure1

Figure 1 – Example of assembling of a kit composed of the support for the windings, a pair of ferrites of ETD type and a pair of fastening clips. (FERRITES and Accessories, Siemens Matsushita Components)

It’s possible choose from a catalog of half-cores with air gap calibrated. For the ferrite type ETD49, for example, we can have 4 values of the air gap: 0.20 +- 0.02 mm, 0.50 +- 0.05 mm, 1.00 +- 0.05, 2.00 +- 0.05 mm.

Coupling a half-core with air gap with another without, or also with air gap, also of different value, it is possible to obtain numerous combinations.

The ferrites of series E and ETD are widely used, so are easy to find. The catalog Siemens Matsushita indicates that the materials available for the E-series are different and coded with the initials N27, N67, N87, N49, N30, T37. The choice of material to use is correlated with the switching frequency: the type N27 is suitable for power applications in a frequency band of switching up to 100KHz, N67 is suitable for similar application, but the frequency range is between 100KHz and the 300KHz. Table 1 shows the possible applications for different materials. The E series has the classical central square column, other families in the same series are available for special applications such as the best known:

ETD stands for Economic Transformer Design, with circular cross-section of the center column

EFD stands for Economic Flat Design transformer for applications with space vertical content.

table1

Table 1 – Some parameters for the type ferrites ETD (FERRITES and Accessories, Siemens Matsushita Components).

Table 2 – Maximum permissible temperature rise for different materials (FERRITES and Accessories, Siemens Matsushita Components).

Table 3 – Thermal resistance for different types and sizes of ferrite (FERRITES and Accessories, Siemens Matsushita Components).

The most important parameters for a correct choice of the ferrite are:

1. Maximum power (Ptrans)

2. Type of converter (Forward, Flyback, Push-Pull)

3. Switching frequency and maximum permissible temperature

4. maximum volume

To make the choice you might consider that the manufacturer, as a rule, always indicates the limit values, so if it is not pressing the issue of costs, it is a good idea to choose on the table, the type immediately above the one that delivers the requested power. This will avoid,later in the phase of winding, to discover that the number of turns calculated, with the wire section calculated does not enter for lack of space in the throat of the support of the windings. This precaution is especially recommended if the transformer should be wrapped in accordance with the safety standards (minimum distances between the different layers of the windings, using wire with double insulation etc..).

It follows an example of calculation of a switching transformer in [1]; the approach to this type of  calculation is in many passages forcibly empirical, in many other simplified. On the other hand a completely theoretical discussion would result in a significant waste of resources without the benefits of improved performance.

SPICE modeling of a JFET from Datasheet

In this article we’ ll see how to find the parameters used to describe the mathematical behaviour of JFET (Junction Field Effect Transistors).The syntax for the N-channel model is:

model ModelName NJF( par1=a par2=b………parn=x)

while for the P-channel model is:

model ModelName PJF( par1=a par2=b………parn=x)

Where par1 par2… parn are the parameters that allow us to model the equations of the JFET transistor.

The main parameters for modeling the JFET are listed below in this table:

 

Parameters Description Units Default Value
AF Flicker noise exponent no unit dimension 1.0
ALPHA Ionization coefficient 1/V 1e-006
BETA Transconductance coefficient A/V^2 0.0001
BETATCE BETA exponential temperature coefficient %/°C -0.5
CGD Zero-bias gate-drain p-n capacitance F 1e-012
CGS Zero-bias gate-source p-n capacitance F 1e-012
FC Forward-bias depletion capacitance coefficient no unit dimension 0.5
IS Gate p-n saturation current A 1e-014
ISR Gate p-n recombination current parameter A 0
KF Flicker noise coefficient no unit dimension 1e-018
LAMBDA Channel-length modulation 1/V 1e-006
M Gate p-n grading coefficient no unit dimension 0.5
N Gate p-n emission coefficient no unit dimension 1.0
NR Emission coefficient for ISR no unit dimension 2.0
PB Gate p-n potential V 1.0
RD Drain ohmic resistance Ohm 1.0
RS Source ohmic resistance Ohm 1.0
VK Ionization knee voltage V 1.0
VTO Thresold voltage V -2.0
VTOTC VTO temperature coefficient V/°C -0.0025
XTI IS temperature coefficient no unit dimension 3.0

SPICE modeling of a BJT from Datasheet

BJT bipolar transistors require a certain number of parameters to get a good model.The syntax for this model is:

.model ModelNameNPN (par1=a par2=b………parn=x)

for PNP case:

.model ModelNamePNP (par1=a par2=b………parn=x)

where par1 par2…….parn are the parameters that allow to model equations of the BJT.

The main parameters for a reasonable modeling of the behavior of the component are summarized in the following table:

Parameters Description Units Default Value
IS Transport saturation current A 1e-16
XTI IS temperature effect exponent no unit dimension 3.0
EG Bandgap voltage (barrier height) eV 1.11
VAF Forward Early voltage V Infinite
BF Ideal maximum forward beta no unit dimension 100
ISE Base-emitter leakage saturation current A 0
NE Base-emitter leakage emission coefficient no unit dimension 1.5
IKF Corner for forward-beta high-current roll-off A Infinite
NK High-current roll-off coefficient no unit dimension 0.5
XTB Forward and reverse beta temperature coefficient no unit dimension 0
BR Ideal maximum reverse beta no unit dimension 1.0
ISC Base-collector leakage saturation current A 0
NC Base-collector leakage emission coefficient no unit dimension 2.0
IKR Corner for reverse-beta high-current roll-off A Infinite
RC Collector ohmic resistance Ohm 0
CJC Base-collector zero-bias p-n capacitance F 0
MJC Base-collector p-n grading factor no unit dimension 0.33
VJC V 0.75
FC Forward-bias depletion capacitor coefficient no unit dimension 0.5
CJE Base-emitter zero-bias p-n capacitance F 0
MJE Base-emitter p-n grading factor no unit dimension 0.33
VJE Base-emitter built-in potential V 0.75
TR Ideal reverse transit time sec 1e-8
TF Ideal forward transit time sec 0
ITF Transit time dependency on Ic A 0
XTF Transit time bias dependence coefficient no unit dimension 0
VTF Transit time dependency on Vbc V Infinite
RB Zero-bias (maximum) base resistance Ohm 0

SPICE modeling of a Diode from Datasheet

Modeling in SPICE& a diode is not a trivial work. Although the operation of the diode is quite simple, extract a model from datasheet takes some time.Every component has its own syntax defined in SPICE , in the case of the diode:

.model ModelName D (par1=a par2=b………parn=x)

where par1 par2 …. parn are characteristic parameters of diode.

we can sum up the set of main parameters in the following table:

Parameter Description Unit Default value
BV Reverse breakdown knee voltage V Infinite
CJO Zero-bias p-n capacitance F 0
EG Bandgap voltage eV 1.11
FC Forward-bias depletion capacitance coefficient no unit dimension 0.5
IBLV Low-level reverse breakdown knee corrent A 0
IBV Reverse breakdown knee corrent A 1e-10
IKF High-injection knee current A Infinite
IS Saturation corrent A 1e-14
ISR Recombination current parameter A 0
M p-n grading coefficient no unit dimension 0.5
N Emission coefficient no unit dimension 1.0
NR Emission coefficient for ISR no unit dimension 2.0
RS Parasitic resistance Ohm 0
TT Transit time sec 0
VJ p-n potential V 1.0
XTI IS temperature exponent no unit dimension 3.0

All these parameters are used by SPICE to describe the behavior of the diode in the different situations of signal, for example in direct polarization in DC that, forward current will be:

ID = IS*(e^(VD/(N*Vt))-1)

where VD is the forward voltage, Vt = k * T / q is the thermal voltage equal to 0.026 V at 27 degrees Celsius.

The so-called recombination current is instead calculated as

Irec = ISR*(e^(VD/(N*Vt))-1).

Other equations from the given parameters describing the capacitance of the junction, its evolution with temperature and more.

At this point we have to derive the various parameters from the datasheet of the component. Assume we want to model a silicon diode 1N4148. The extraction of the parameters of the table from the values reported in the datasheet, is not immediate for almost none of the parameters.look at the values of our interest in datasheet:

data1

From the table we can get BV which is equal to VRM, in other cases reported as Vbr, or in the case of Zener diode Vz.

data2

From this second table we see that the maximum leakage current at 25 degrees is Ir = 5 uA.We can take IBV as equal to 10 times Ir. Usually for this type of diodes the value of IBV is around 100uA. For Zener diodes Ir can be called Izk, or in other cases as Ibr.

CJO can be directly equal to the value specified in the datasheet as Cj or Ctot, in this case is 4pF.