Добавил:
Опубликованный материал нарушает ваши авторские права? Сообщите нам.
Вуз: Предмет: Файл:
Скачиваний:
68
Добавлен:
06.06.2017
Размер:
3.31 Mб
Скачать

BETA2 = IC1/(IBIAS-IOFF/2)

IEE = (((BETA1+1)/BETA1)+((BETA2+1)/BETA2))IC1

RE1 = ((BETA1+BETA2)/(BETA1+BETA2+2))(RC1-VT/IC1) RE2 = RE1

RP = (|VCC|+|VEE|)2/(PD-|VCC|2IC1-|VEE|IEE) RE = VAF/IEE

BJT1IS = 1E-16

BJT2IS = BJT1IS(1+VOFF/VT)

JFET input stage

IC1 = SRPC2/2

IEE = C2SRN

CE = C2(SRN/SRP-1)

RE = VAF/IEE

RE1 = 1

RE2 = 1

BETA1 = 0.5GA2/IEE

BETA2 = BETA1

RP = (|VCC|+|VEE|)2/PD

RO2 = ROUTDC - ROUTAC

GCM = 1/(CMRRRC1)

GB = RC1A/RO2

VLP = IOSC1000

VLN = VLP

VC = VCC - VPS

VE = -VEE + VNS

Controlled source equations I(GA) = GA(V(A1)-V(A2)) I(GCM)= GCMV(CM)

I(F1) = GBI(VS1)-GBI(VC)+GBI(VE)+GBI(VLP)-GBI(VLN) V(E1) = (V(VCC)+V(VEE))/2

V(H1) = 1000(I(VS2))

V(VS1)= 0.0 (Only used to measure current) V(VS2)= 0.0 (Only used to measure current)

Note that the Level 2 and 3 models use Gain Bandwidth (GBW), not Unity Gain Frequency (F0), as an input parameter. They correctly produce both the specified phase margin and unity gain at the frequency F0. In general, F0 < GBW. This is an enhancement to the standard Boyle model which produces the specified phase margin but not unity gain at the frequency F0.

457

Pulse source

Schematic format

PART attribute <name>

Examples

P1

MODEL attribute <model name>

Example

RAMP

The PULSE source is similar to the SPICE PULSE independent voltage source, except that it uses a model statement and its timing values are defined with respect to T=0.

Model statement forms

.MODEL <model name> PUL ([model parameters])

Example

.MODEL STEP PUL (VZERO=.5 VONE=4.5 P1=10n P2=20n P3=100n

+ P4=110n P5=500n)

Model parameters

 

 

Name

Parameter

Units

Default

VZERO

Zero level

V

0.0

VONE

One level

V

5.0

P1

Time delay to leading edge

S

1.0E-7

P2

Time delay to one-level

S

1.1E-7

P3

Time delay to trailing edge

S

5.0E-7

P4

Time delay to zero level

S

5.1E-7

P5

Repetition period

S

1.0E-6

458 Chapter 22: Analog Devices

Equations

The waveform value is generated as follows:

From

To

Value

0

P1

VZERO

P1

P2

VZERO+((VONE-VZERO)/(P2-P1))(T-P1)

P2

P3

VONE

P3

P4

VONE+((VZERO-VONE)/(P4-P3))(T-P3)

P4

P5

VZERO

where From and To are T values, and T=TIME mod P5. The waveform repeats every P5 seconds. Note that P5 ≥ P4 ≥ P3 ≥ P2 ≥ P1.

Figure 22-18 Sample waveform for model parameters vzero=1 vone=4 P1=.1u P2=.2u P3=.4u P4=.5u P5=1u

459

Resistor

SPICE format

Syntax

R<name> <plus> <minus> [model name] <value> [TC=<tc1>[,<tc2>]]

Examples

R1 2 3 50

R2 7 8 10K

<plus> and <minus> are the positive and negative node numbers. The polarity references are used only for plotting or printing the voltage across, V(RX), and the current through, I(RX), the resistor.

Schematic format

PART attribute <name>

Examples

R5

CARBON5

VALUE attribute

<value> [TC=<tc1>[,<tc2>]]

Examples 50

10K

50K*(1+V(6)/100)

FREQ attribute <fexpr>

Examples 2K+10*(1+F/1e9)

MODEL attribute [model name]

Example

RMOD

460 Chapter 22: Analog Devices

VALUE attribute

<value> may be a simple number or an expression involving time-domain variables. The expression is evaluated in the time domain only. Consider the expression:

100+V(10)*2

V(10) refers to the value of the voltage on node 10 during a transient analysis, a DC operating point calculation prior to an AC analysis, or during a DC analysis. It does not mean the AC small signal voltage on node 10. If the DC operating point value for node 10 was 2, the resistance would be evaluated as 100 + 2*2 = 104. The constant value, 104, is used in AC analysis.

FREQ attribute

If <fexpr> is used, it replaces the value determined during the operating point. <fexpr> may be a simple number or an expression involving frequency domain variables. The expression is evaluated during AC analysis as the frequency changes. For example, suppose the <fexpr> attribute is this:

V(4,5)*(1+F/1e7)

In this expression, F refers to the AC analysis frequency variable and V(4,5) refers to the AC small signal voltage between nodes 4 and 5. Note that there is no time-domain equivalent to <fexpr>. Even if <fexpr> is present, <value> will be used in transient analysis.

Stepping effects

The VALUE attribute and all of the model parameters may be stepped. If VALUE is stepped, it replaces <value>, even if <value> is an expression. The stepped value may be further modified by the temperature effect.

Temperature effects

There are two different temperature factors, a quadratic factor and an exponential factor. The quadratic factor is characterized by the model parameters TC1 and TC2, or <tc1> and <tc2> from the parameter line. The exponential factor is characterized by the model parameter TCE.

If [TC=<tc1>[,<tc2>]] is specified on the parameter line, <value> is multiplied by a temperature factor, TF.

TF = 1+<tc1>(T-Tnom)+<tc2>(T-Tnom)2

461

If [model name] is used and TCE is not specified, <value> is multiplied by a temperature factor, TF.

TF = 1+TC1(T-Tnom)+TC2(T-Tnom)2

TC1 is the linear temperature coefficient and is sometimes given in data sheets as parts per million per degree C. To convert ppm specs to TC1 divide by 1E6. For example, a spec of 3000 ppm/degree C would produce a TC1 value of 3E-3.

If [model name] is used and TCE is specified, <value> is multiplied by a temperature factor, TF.

TF = 1.01TCE•(T-Tnom)

If both [model name] and [TC=<tc1>[,<tc2>]] are specified, [TC=<tc1>[,<tc2>]] takes precedence.

T is the device operating temperature and Tnom is the temperature at which the nominal resistance was measured. T is set to the analysis temperature from the Analysis Limits dialog box. TNOM is determined by the Global Settings TNOM value, which can be overridden with a .OPTIONS statement. T and Tnom may be changed for each model by specifying values for T_MEASURED, T_ABS, T_REL_GLOBAL, andT_REL_LOCAL. See the .MODEL command for more on how device operating temperatures and Tnom temperatures are calculated.

Monte Carlo effects

LOT and DEV Monte Carlo tolerances, available only when [model name] is used, are obtained from the model statement. They are expressed as either a percentage or as an absolute value and are available for all of the model parameters except the T_parameters. Both forms are converted to an equivalent tolerance percentage and produce their effect by increasing or decreasing the Monte Carlo factor, MF, which ultimately multiplies the final value.

MF = 1 ± tolerance percentage /100

If tolerance percentage is zero or Monte Carlo is not in use, then the MF factor is set to 1.0 and has no effect on the final value.

The final resistance, rvalue, is calculated as follows:

rvalue = <value> * R * TF * MF

462 Chapter 22: Analog Devices

Model statement form

.MODEL <model name> RES ([model parameters])

Example

.MODEL RM RES (R=2.0 LOT=10% TC1=.015)

Model parameters

 

 

 

Name

Parameter

Units

Default

R

Resistance multiplier

 

1.0

TC1

Linear temperature coefficient

°C-1

0.0

TC2

Quadratic temperature coefficient

°C-2

0.0

TCE

Exponential temperature coefficient

%/°C

0.0

NM

Noisemultiplier

 

1.0

T_MEASURED

Measured temperature

°C

 

T_ABS

Absolute temperature

°C

 

T_REL_GLOBAL

Relative to current temperature

°C

 

T_REL_LOCAL

Relative to AKO temperature

°C

 

Noise effects

Noise in resistors is due to the random thermal motion of the carriers and is not affected by the presence of direct DC current as in shot noise. It is modeled with an ideal thermal noise current calculated as follows:

I = NM * sqrt(4*K*T/rvalue )...( per unit bandwidth)

NM, multiplies the resistor noise current. A value of zero effectively eliminates the noise contribution from all resistors that use the model.

463

S_Port ( S-Parameter two-port )

Schematic format

PART attribute <name>

Example

SP1

FILE attribute <file name>

The FILE attribute specifies the path and name of the S-parameter file.

Example

E:\mc7\data\Gg10v20m.s2p

The S_PORT source provides a way of modeling devices using S-parameters. Typically these are provided by RF suppliers in a text file as a table of values for S11, S12, S21, and S22. The file typically looks like this:

!SIEMENS Small Signal Semiconductors

!BFG194

!Si PNP RF Bipolar Junction Transistor in SOT223

! VCE = -10 V

IC = -20 mA

 

 

 

! Common Emitter S-Parameters:

August 1996

# GHz S MA R 50

 

 

 

 

 

! f

S11

 

S21

S12

S22

 

 

! GHz

MAG

ANG

MAG ANG

MAG ANG

MAG ANG

0.010

0.3302

 

-25.4 35.370 169.9 0.0053

85.3

0.9077

-10.0

0.020

0.3471

 

-48.2 33.679 161.6 0.0108

77.5

0.8815

-19.8

0.050

0.4525

 

-95.0 27.726 139.2 0.0226

61.4

0.7258

-43.7

0.100

0.5462 -131.5 19.023 118.7 0.0332

52.2 0.5077 -68.7

0.150

0.5723 -149.4 13.754 106.4 0.0394

49.1 0.3795 -84.8

0.200

0.5925

-159.8 10.787

99.1 0.0443

50.1

0.3068

-95.0

0.250

0.6023

-167.0

8.757

93.4 0.0497

51.2 0.2581 -104.8

0.300

0.6089

-172.2 7.393 89.0 0.0552

52.4 0.2298 -112.2

0.400

0.6166

 

179.7

5.617

82.1 0.0661

54.2 0.1930 -125.5

...

 

 

 

 

 

 

 

 

464 Chapter 22: Analog Devices

MC7 converts the S-parameters to Y-parameters and then implements the S_PORT source as a set of four Laplace table sources. The Y-parameters are calculated directly from the S-parameters using the following standard formulas (See "Microwave Circuit Design", by Vendelin, Pavio, and Rhoda page 16).

D = ((1+S11)*(1+S22)-S12*S21)

y11 = ((1-S11)*(1+S22)+S12*S21) / D

y12 = -2*S12 / D

y21 = -2*S21 / D

y22 = ((1+S11)*(1-S22)+S12*S21) / D

The S_PORT model looks like this:

Figure 22-19 S_PORT Equivalent Model

465

S (Voltage-controlled switch)

SPICE format

S<name> <plus output node> <minus output node> +<plus controlling node> <minus controlling node> +<model name>

Example

S1 10 20 30 40 RELAMOD

Schematic format

PART attribute <name>

Example

S1

MODEL attribute <model name>

Example

RELAY

This four-terminal voltage-controlled switch is controlled by the voltage across the two input nodes. The switch impedance is calculated from the input voltage and impressed across the output nodes.

RON and ROFF must be greater than zero and less than 1/Gmin.

A 1/Gmin resistor is placed between the controlling nodes to avoid floating nodes.

Do not make the ratio ROFF/RON larger than about 15 decades. The 15 digits of precision used by the simulator can not make meaningful use of a spread greater than 15 in the ratio.

Do not make the transition region, VON-VOFF, too small as this will cause an excessive number of time points required to cross the region. The smallest allowed values for VON-VOFF is (RELTOL(max(VON,VOFF))+VNTOL).

Model statement forms

.MODEL <model name> VSWITCH ([model parameters])

466 Chapter 22: Analog Devices

Соседние файлы в папке Micro-Cap v7.1.6
  • #
    06.06.20171.32 Кб60model.CNT
  • #
    06.06.201776.72 Кб62MODEL.HLP
  • #
    06.06.20173.72 Кб60NETHASP.INI
  • #
    06.06.2017450 б59os.dat
  • #
    06.06.2017545 б63READ.ME
  • #
    06.06.20173.31 Mб68RM.PDF
  • #
    06.06.2017226.69 Кб61setup.bmp
  • #
    06.06.201795 б59SETUP.INI
  • #
  • #
    06.06.201749 б60setup.lid
  • #
    06.06.20172.04 Mб59Standard.cmp