Hello

Has somebody expereince with exact simulation of transmission chain with inductive coupling.
Under transmission chain I understand transmitter circuit, transmitter antenna, receiver antenna, receiver circuit.
I envisage following approach:
1. Design couple of 2 antanna coils (transmitter, receiver) in some EM-tools (HFSS, Sonnet, Momentum,...) with given geometries and mutual distance/orientation
2. Simulate this couple of coils and obtain its matrix of S-parameters for given frequency.
3. Create in Cadence a cell, that symbolize this couple of coils and attach Spice/Spectre view, that contains S-matrix.
4. Put this cell in schema that includes transmitter and receiver parts.

If my comrehesion is just (I didn't do it yet), this approch works only for linear circuits, because EM simulators (at least HFSS) require to specify resistance at ports before simulation.

But if at transmitter side amplifier is E-class (non-linear), how to proceed?

Regards

Pavel.

Hello Didac,

First of all, thank you for response.
Quote:

I'm trying to simulate propagation of signal between HF (13.56 MHz) Reader and Transponder. There are 2 boards - reader and transponder. Each board contains its proper antenna. Two boards are placed at some distance one from other.
First I want to specify reader antenna amplifier performance for given geometries of antennas (reader and transponder) and given distance between them. For this I want to estimate the induced voltage on transponder LC-tank for different configurations of reader antenna amplifier.

Second, I would like to simulate data link, of course.

Quote:

Obtain mutual copling... How? Using simplifying formulas?
Lumped model... Sorry, I don't understand what you mean under this term.
In any way if EM-simulator can give extract precise S-matrix (for different geometries, different distances and different orientations), why not use it?
Find the directivity of antenna... How to do it without EM-simulator?

Regards.

Pavel.

Hi to all,
Usually when I deal with antennas I use different approaches depending on what I'm doing with it:
1)If I'm designing it I use formulas,books and EM to modelate it.
2)If I want to test the effect over a circuit I usually consider them as a complex load(obtained by hand or using EM software-better EM software we are engineers after all-), in your case for your frequency the frontier between induced fields and radiated fields is around 3'5m  so for antennas separated around 30-40m I don't expect that the mutual inductance affect the input impedance of the antenna, I expect more disturbance coming from the PCB itself. So I think that you can model the antenna just as a load for the receiver and other load for the transmiter,avoiding potential problems mixing time domain simulation with frequency domain data.
3)When I want to test a datalink I just find the directivity of the transmitter and the receiver antenna(if they are in far field their directivity is independent of each other), add a block that models the channel(at this frequency I think that a AWGN channel it's just right) and connect the transmitter and the receiver using this equivalent blocks.

But as pancho says spectre Nport allows you to use the results of the EM, so in fact I think that the metodology you proposed in your first post is valid-

At first I was confused because I thought you have something like a FDD transceiver in which you sent and transmit simultaneusly and you wanted to check the effects of mutual coupling on the performance.
Hope it helps,

Hi Pavel,
Nport accepts the TOUCHSTONE standard, a link to a more detailed description:http://www.vhdl.org/pub/ibis/connector/touchstone_spec11.pdf(it's not the last version but I've been using it recently and I didn't notice any change-. Basically you define the iinput data with a first line like:
# GHz S RI R 100
Where the first term is the units of frequency,second term the type of data, third term indicate how you provide the data(in this case Real and Imaginary) and finally the R of normalization. I don't have many experience with it(I used only to substitute inductors in the extracted with the silicon measured to see if the drift matched the measurements) but I think two important factors come into play:
1)Provide enough low frequency points because spectre needs them for calculate dc operating point.
2)Take care with phase "jumps", it can cause trouble.

Regarding your operational distance then I think you are right, you should take into account both coils for the EM simulation.


Hope it helps,

Hi Pavel,
Sorry for the delay in answering but I was searching an application note from Cadence about nport that I used.http://www.cadence.com/whitepapers/spramapn.pdf. From what I understand spectre takes the s-parameters inserted in the file using nport, an transforms them to an equivalent time-domain model that it can handle before the simulation,after this calculation s-params dissappear for spectre. So I think that if you use a 2-port (port 1 transmitter,port 2 receiver) the simulator will take into account the effect of switching.
As you say S-params in EM are calculated for specific impedance, but I think that they are necessary for spectre only to make the "transformation" from frequency domain to time domain,nothin else.
Hope it helps,

Hi Pavel,
I'm not sure about this one but I think it really doesn't matter. In S-parameters we specify a reference impedance cause we are working with normalized power waves, as you said different reference impedances result in different S-parameters matrix. But the equivalent circuit will always be the same, so I think that when spectre does the time domain model from the s-parameters file he would use the reference impedance to obtain the equivalent model because spectre doesn't deal with power waves, only with voltages and currents. Probably for this question it's better to contact with a product engineer.
Hope it helps,

Hi.

Characteristic impedance(Port Impedance) for S-parameter is not concerned with load impedance.
They can be different.
S-parameter is defined by characteristic impedance(Port Impedance).
You seem to be misunderstanding them.

In EM-simulation such as Agilent ADS Momentum, you need to specify port impedance.
Basically you can specify any value as port impedance since target block that EM-simulator treat is linear.
But some numerical accuracy loss will occur if you specify extraordinally value as port impedance.
[Note] Common EM-simulator can't treat nonlinear device at same time.

In circuit simulator. S-parameter is converted to unnormalized Y-parameter internally where characteristic impedance value is needed to
convert s-parameter to y-parameter.
In convolution, IFFT of this Y-parameter is used.

Resulting Y-parameter has no relation with port impedance.

It's better to use HFSS to design the attena things.