[Ngspice-users] Antenna spice modelisation

[Dominique M. <dom...@ho...>]

It was an old message for help with an antenna model.

An antenna is basiquely an RLC circuit, and like all the RLC, you have only 
the resistive composant att the resonance.
If your concern is to simulate the antenna's emission or reception diagram, 
spice is definitly not the right software for that.
If you want to simulate how a tuner or a high frequency amplifier look at 
the antenna, you must make a model for your antenna.
It will include a RLC circuit in all the cases, and a voltage source if your 
antenna is working in reception mode.

Now, the mathematics that must be used to determine the RLC componants of 
the antenna are really complicated. The best book i know on the subject is 
"Antenna Theory, Analysis and Design" by Constantine A. Balanis. This book 
is great because it is both academic and useful. You wiil find all the 
mathematics and when they are complicated, the autor have computed the 
values and included some kind of diagram for easy and precise designing.
Books on radioelectricity can be useful to find informations on how an 
antenna is interacting with an electronic circuit, but they are not so 
useful to find antenna characteristics.

As exempel, a standard outdoor receiving antenna for the AM band (longwire 
150kHz-20MHz) can be modeled as follow (as in électronique et 
radioelectricité, tome 2 haute fréquence, G. Thalmann):

V1 1 0 SIN(0 0.001 1meg)
C1 1 2 200pF
R1 2 3 400
C2 3 4 400pF
L1 2 4 20uH

The output is between 4 and 0. A such circuit is very usefull too to align a 
tuner, just insert it between the HF generator (V1 for spice) and the radio 
you want to align. It is equivalent to the following antenna: 15 meters 
horizontal wire at 7.5 meter high, followed by 10 meters wire going in 
straight line directly to the tuner (on the ground).
As you can see, the RLC is open. The only way between the node 1 and the 
ground is trough V1, that mean trough the ether in the real world.

I have not test the circuit in spice. The only way to the ground at node 1 
is V1, and maybe you must have an extra resistor (R2 1 0 1G). The circuit 
assume at the way to the ground for node 4 is where you are connecting the 
antenna, usually a coil. It can be necessary to put an extra resistor for 
spice to work.

Another problem is if you have a transmission line between the antenna and 
the electronic. A coaxial cable like the RG58 (or a connector) don't have at 
all a constant transfer impedance with the frequency. The Swedish National 
Testing and Research Institute ( www.sp.se ) have done some work on this, 
and they have developped a windows program (FD2D) that can be used to 
determine PSpice models for EMC analysis. They are using some kind of 
multiports with associated S parameters for the models.

Regards
Dominique Michel

_________________________________________________________________
MSN Hotmail : antivirus et antispam intégrés 
http://www.msn.fr/newhotmail/Default.asp?Ath=f