New Models Simulate RF Circuits - Intusoft

New Models Simulate RF Circuits
Its no news to those who simulate that the accuracy of SPICE is
directly related to the accuracy of the models. What may be news
is that simulation of high frequency circuits well into the gigahertz
range is now possible due to the introduction of some new RF
SPICE models.
To illustrate the improved simulation accuracy, the RF models
were used to analyze a 500 MHz oscillator (Figure 1). The
oscillator generates a relatively high power output with a very
distorted output waveform (typical at power levels over the 1-
2mW range). The simulation goals were to study the start-up
characteristics, oscillating frequency and amplitude, and the
resulting harmonic distortion. Two simulations were run. The first
using the standard Gummel-Poon BJT model and simple inductor
chokes and a second using an improved 2N5109 model along
with a new Intusoft RF bead model from the RF Device Library.
Above approximately 100-200 MHz, the built-in SPICE BJT
model, based on the Gummel Poon model, fails to accurately
predict the real device performance. The BJT must be remodeled
as a subcircuit (Table 1) in order to accurately model the package
and bond wire parasitics which are of greater significance at
higher frequencies. The improved model includes the package
parasitics and matches the s-parameters up to 2 GHz. The RF
library was created by Analog & RF Models, specialists in the
creation of RF models, for Intusoft [1].
R3
1K
15
CG
1 100PF 2
VIN
PWL
14
LS2
3NH
CCO
12PF
V(15)
RL VOUT
50
R2 10E6
X2
DN5441
RGC
1K
STARTUP
CIRCUITRY
CBC
22PF
16
LS1
3NH
17
LT
20NH
V(3)
START
RTI 10K
18 30
VCC RBU
8V 2.2K
LBX
3NH
RBL
1K
D1
DN4148
VVT
4V
8
13
12
LSP 170NH
XLSP
B9112
V(7)
VPOWER
LCX
5NH
11
LEX
5NH
V(3)
START
CEX
5PF
6
X1
QN5109
5
3
22
CB1 10PF
7 9LB1
3NH
CB2
47PF
LB2
3NH
LEC 170NH
XLEC
B9112
REX
47
4
LB1, LB2, LS1, and LS2 are
parasitic inductances for the
capacitors. LBX, LCX, and
LEX represent the additional
lead inductance beyond the
plane where the manufacturer
measured the transistor
s-parameters. LEC and LSP
are RF chokes. The varactor
includes parasitic capacitance
and inductance inside
the subcircuit.
1 2 4
3
5
VARACTOR
Figure 1, A 500 MHz oscillator and RF Bead (shaded area) test circuit.
Page 1

Modeling An RF Bead
Although SPICE does contain a model for a nonlinear inductor it
does not have a built-in bead model. Fortunately, one can be
created using the a nonlinear magnetics model and passive
elements. The new model, as shown in Figures 1 & 2, accurately
simulates the impedance vs. frequency response and the change
in impedance vs. temperature. The change in impedance with DC
bias is also modeled due to the addition of the core model instead
of a simple inductor. The bead model gives a very low DC
impedance while providing a large impedance at higher frequencies.
The model used here is for a ferrite bead made of a medium
permeability nickel zinc material from Fair-Rite, P#2743009112.
Other types of beads including beads on leads, wound beads and
surface mount beads can be found in the RF library [2].
180
180
1
Z (2743003112) in Ohms
140
100.0
60.0
Z (2743009112) in Ohms
140
100.0
60.0
2
3
4
20.0
20.0
1MEG 10MEG 100MEG 1G
Impedance (Ohms) vs. Frequency in Hz
Figure 2, The Intusoft RF Bead model simulates the proper impedance vs.
frequency characteristics. The graph displays the response for several devices.
Starting An Oscillator
Simulation of oscillators present a variety of challenges, not the
least of which is getting the oscillator to oscillate. When ISSPICE
performs an AC or Transient analysis it first performs a DC
analysis in order to establish the starting initial operating point for
the circuit. If a stable operating point is found, which is the goal of
the DC analysis, the oscillator may not oscillate during the
transient (time domain) analysis unless some random disturbance
is encountered.
There are a number of ways to start an oscillator; each with
varying results and consequences (Figure 3). The method chosen
here was to introduce a voltage pulse into the circuit, specifically,
at the emitter of the transistor (VIN 1 0 PWL...). Another
possible method is to insert a current pulse somewhere in the
resonant portion of the circuit, for example at LT (I1 18 17 PULSE
.01 0). If the DC analysis does not converge, a sign that the circuit
Page 2

Input Current Pulse At Time 0
1
Input Voltage Pulse
4
Ramping The Power Supply
2
UIC Transient Option
No Starting Help Given
3
5
5.0000N 15.000N 25.000N 35.000N 45.000N
TIME in Secs
Figure 3, Comparison of the various methods of “thumping” an oscillator to get it
started show a current pulse at LT to be the most effective for this circuit.
is unstable and may want to oscillate without any help, the UIC
keyword can be issued in the .TRAN statement. For example,
.TRAN .1NS 50NS UIC. This will cause the simulation to proceed
directly to the Transient analysis bypassing the DC analysis. The
.IC and “IC=” parameters can then be used to set initial transient
conditions and unbalance the oscillator. One problem with using
UIC is that no DC operating point will be produced inhibiting study
of the circuit bias. The last method is similar to the first and
involves ramping of the power supply (VCC 8 0 PULSE 0 8V 0
5NS). This method may not work well, however, due to the bypass
capacitors. In general, when ramping a source, make sure to give
the ramp a realistic slope in order to avoid “timestep too small”
errors. The first two methods are the most often recommended as
the other methods may not work or may introduce transient startup
residues [3].
Circuit Modeling
The oscillator circuit was first simulated with two inductor chokes,
LSP and LEC (Figure 1), and a standard .MODEL statement for
the 2N5109 transistor. In SPICE, the standard representation for
a transistor uses the Gummel-Poon model. Various parameters
in the SPICE .MODEL statement are altered in order to cause the
“generic nature” of the Gummel-Poon template to represent a
particular device.
In a second simulation, the chokes were each replaced with the
new RF bead model. The simple transistor model was replaced
with a subcircuit representation. Since the Gummel-Poon model
can not adequately represent BJT behavior above approximately
200MegHz, a composite model must be assembled. The SPICE
subcircuit, containing a BJT model and various parasitic elements,
is utilized for this purpose.
Page 3

When simulating in SPICE it is best to use a subcircuit representation
for a device rather than forcing model parameters to have
unreasonable values. If model parameters are used outside their
physical bounds, the model may work well in one area, but
incorrectly in another. For example, the device may behave
properly during the AC small signal analysis, but poorly during the
nonlinear transient analysis. Some vendors who produce SPICE
model use this approach and the user should beware. Models for
RF transistors that are going to be used for both linear and
nonlinear analysis can not be produced this way. A subcircuit
representation must be used!
Note: Parasitics for the passive elements were maintained for
both simulation cases.
1.000
14.69
0
12.69
VOUT in Volts
-1.000
-2.000
VPOWER in Volts
10.69
8.690
1
2
-3.000
6.690
5.000N 15.00N 25.00N 35.00N 45.00N
WFM.2 VPOWER vs. TIME in Secs
With Bead and Parasitics
11.81
1.000
1
9.811
0
VPOWER in Volts
7.811
5.811
VOUT in Volts
-1.000
-2.000
3.811
-3.000
2
5.000N 15.00N 25.00N 35.00N 45.00N
WFM.1 VOUT vs. TIME in Secs
No Beads with Parasitics
Figure 4, Comparison of the start-up and power supply waveforms with (Top) and
without (Bottom) the new RF bead model.
Page 4

Results
In order to isolate VCC and not contaminate the power supply with
the 500 MHz oscillating waveform, adequate bypassing is required.
A voltage generator represents a perfect bypass because
it is zero ohms at all frequencies. This is quite different from the
real world.
As shown in Figure 4, use of an inductor causes a droop in the
VCC voltage. The reason for the droop is that the 170nH represents
a large impedance. As the oscillator starts up, the transistor
wants more current. Because of the large inductance it can't draw
adequate current so it starts to discharge the bypass capacitors.
This appears as a drooping in the VCC power (lower graph). The
bead, on the other hand, has a very low DC impedance and a high
AC impedance. By choosing the proper bead, a frequency response
can be selected that will block all the AC around the
oscillation frequency. With the bead (upper graph), the VCC line
doesn't droop and shows that the size of the ripple stays the same
revealing the imperfections in the bypassing. Also note that the
oscillation starts slower and does not have quite as much power
out with the bead inserted (to be expected) as it does when the
inductors are used.
The oscillator with no BJT parasitics or beads still oscillates
because it was made to be tolerant of package parasitics, but the
results predicted were inaccurate in several important areas. As
shown in Figure 5, the FFT and transient response of the circuit
with beads and new RF BJT subcircuit model reveals that the
frequency of oscillation is lower and the distortion higher.
Conclusions
From the simulations performed, it is clear that modeling the
proper circuit parasitics is of vital importance, especially at RF
frequencies. It is recommended that initial simulations run for
many cycles in order to verify that stable oscillation is actually
taking place. As for performing an FFT, the ISSPICE .TRAN tstart
parameter can be used to delay the start of data taking until steady
state oscillation has been reached.
With the new bead and BJT models in the RF library, ISSPICE is
able to show the peak component stresses when power is
applied, the transient start-up performance, and the variations in
the power supply. In contrast to the linear analysis programs
commonly used by RF designers, ISSPICE simulations can reveal
many important circuit properties such as efficiency, power dissipation,
start up characteristics, and harmonic distortion. Characteristics
that would be either difficult or impossible to measure.
Page 5

FFT of VOUT (NBNP) in Volts
1.600
1.200
800.0M
400.0M
FFT of VOUT (WBWP) in Volts
800.0M
600.0M
400.0M
200.0M
With
Beads and
BJT
Parasitics
x
<
519.5MEG
733.3M
>
With
Inductors
and No
Parasitics
x
<
1.052G
135.4M
>
0
0
1
2
200.0MEG 600.0MEG 1.000G 1.400G 1.800G
WFM.2 VOUT vs. TIME in Secs
FFT Responses
dx = 532.8MEG dy = -597.9M
3.000
1.000
With Beads and BJT
Parasitics
1
VOUT (WBWP) in Volts
2.000
1.000
0
-1.000
VOUT (NBNP) in Volts
0
-1.000
-2.000
-3.000
With Inductors and
No Parasitics
2
91.00N 93.00N 95.00N 97.00N 99.00N
TIME in Secs
Output Waveforms at Steady State
Figure 5, Comparison of the frequency spectrum and time waveforms using the new
Intusoft BJT and bead models vs. the Gummel-Poon model and inductor chokes. The
new models give a more accurate prediction of distortion and oscillation frequency.
Table 1, ISSPICE Subcircuit for an RF Transistor & Bead
1
.SUBCKT QN5109 1 2 3
LC 1 4 0.875E-9
LC
4
LB 2 6 1.590E-9
CB CC
LE 5 3 2.650E-9
2 LB 6
CC 4 3 1.410E-12
Q1
CB 4 6 0.561E-12
LE
5 3
Q1 4 6 5 QR33
.MODEL QR33 NPN ( BF=44 VAF=160 VAR=16.0 RC=0.69
+RB=1.57 RE=2.75 IKF=0.28E+00 ISE=0.36E-13 TF=0.111E-09
+TR=0.80E-08 ITF=0.82E-01 VTF=0.66E+01 CJC=2.758E-12
+CJE=1.822E-12 XTI=3.0 NE=1.5 ISC=0.12E-13 EG=1.11
+XTB=1.5 BR=1.14 VJC=0.75 VJE=0.75 IS=0.40E-14
+MJC=0.33 MJE=0.33 XTF=4.0 IKR=0.28E+00 KF=0.1E-14
+NC=1.7 FC=0.50 RBM=1.1 IRB=0.40E-01 XCJC=0.5 )
.ENDS
.SUBCKT BEAD 1 2
R4 1 2 220 TC=-.00333
C2 1 2 .9PF
RX 3 2 1E12
CB 3 2 7.432N
F1 1 2 VM1 1
G2 2 3 1 2 1
.MODEL DCLAMP D
E1 4 2 3 2 1
+CJO=8.2286P VJ=25
VM1 4 5
.ENDS
RB 5 2 341.5
RS 5 6 3.7904
VP 7 2 300
D1 6 7 DCLAMP
VN 2 8 300
D2 8 6 DCLAMP
Page 6

References
[1] Analog & RF Models, Bill Sands (602) 575-5323, FAX (602)
297-5160
[2] RF Device Library, Intusoft, 1990
[3] “SIMULATING WITH SPICE”, L.G. Meares, C.E. Hymowtiz, Intusoft,
1988
Page 7