开云体育

Hello everyone,

I have a problem with ac analysis of my circuit (can be found in Files > Temp > AC Analysis > TEC-Model.asc). The overall circuit consists of two separate circuits which are connected with each other by behaviourale sources. Transient analysis seems to work flawlessly as expected, however ac analysis doesn't unfortunately. My goal is to get the transfer function of this particular circuit with input being voltage (net name = V_input) and output being temperature (net name = T_h_TC).
To begin with I had tried the laborious way of manually determining the bode diagram by performing transient analysis at several frequencies (0.001 0.01 0.1 1)Hz with sinusoidal excitation. I then compared amplitudes and phases of input and output at each frequency to get the bode plots of my system. It works but the process takes up too much time...
All I want is to apply a ac sweep from 0.001 to 1 Hz on my system to see how the output responds, however, the output is steady with absolut no changes when doing so (as a matter of fact, there are no changes anywhere within the circuit). It seems as the output is not dependent on the input anymore when performing ac analysis and I was wondering for quite a while now why that is the case? I suspect that the behaviourale sources are the cause for this phenomenon as they connect input and output.
I was hoping an LTspice expert could help me with this issue?

Many thanks in advance already.

--- In LTspice@..., "legendary_earl_e_bird" <m-marcus@...> wrote:

Hello everyone,

I have a problem with ac analysis of my circuit (can be found in Files > Temp > AC Analysis > TEC-Model.asc). The overall circuit consists of two separate circuits which are connected with each other by behaviourale sources. Transient analysis seems to work flawlessly as expected, however ac analysis doesn't unfortunately. My goal is to get the transfer function of this particular circuit with input being voltage (net name = V_input) and output being temperature (net name = T_h_TC).
To begin with I had tried the laborious way of manually determining the bode diagram by performing transient analysis at several frequencies (0.001 0.01 0.1 1)Hz with sinusoidal excitation. I then compared amplitudes and phases of input and output at each frequency to get the bode plots of my system. It works but the process takes up too much time...
All I want is to apply a ac sweep from 0.001 to 1 Hz on my system to see how the output responds, however, the output is steady with absolut no changes when doing so (as a matter of fact, there are no changes anywhere within the circuit). It seems as the output is not dependent on the input anymore when performing ac analysis and I was wondering for quite a while now why that is the case? I suspect that the behaviourale sources are the cause for this phenomenon as they connect input and output.
I was hoping an LTspice expert could help me with this issue?

Many thanks in advance already.

Hello,

.AC analysis is a small signal AC analysis. This means that the model is linearized at the DC operating point before the AC sweep is done. If you model contains BV sources of the form V=V(a)*V(b) and the DC value of either V(a) or V(b) is zero, the output of the small signal model will be zero. This is not a problem with SPICE; it is the way the math works. Your i(R_m1) terms are probably causing the result you are getting.

Rick

--- In LTspice@..., "sawreyrw" <sawreyrw@...> wrote:

--- In LTspice@..., "legendary_earl_e_bird" <m-marcus@> wrote:

Hello everyone,

I have a problem with ac analysis of my circuit (can be found in Files > Temp > AC Analysis > TEC-Model.asc). The overall circuit consists of two separate circuits which are connected with each other by behaviourale sources. Transient analysis seems to work flawlessly as expected, however ac analysis doesn't unfortunately. My goal is to get the transfer function of this particular circuit with input being voltage (net name = V_input) and output being temperature (net name = T_h_TC).
To begin with I had tried the laborious way of manually determining the bode diagram by performing transient analysis at several frequencies (0.001 0.01 0.1 1)Hz with sinusoidal excitation. I then compared amplitudes and phases of input and output at each frequency to get the bode plots of my system. It works but the process takes up too much time...
All I want is to apply a ac sweep from 0.001 to 1 Hz on my system to see how the output responds, however, the output is steady with absolut no changes when doing so (as a matter of fact, there are no changes anywhere within the circuit). It seems as the output is not dependent on the input anymore when performing ac analysis and I was wondering for quite a while now why that is the case? I suspect that the behaviourale sources are the cause for this phenomenon as they connect input and output.
I was hoping an LTspice expert could help me with this issue?

Many thanks in advance already.

Hello,

.AC analysis is a small signal AC analysis. This means that the model is linearized at the DC operating point before the AC sweep is done. If you model contains BV sources of the form V=V(a)*V(b) and the DC value of either V(a) or V(b) is zero, the output of the small signal model will be zero. This is not a problem with SPICE; it is the way the math works. Your i(R_m1) terms are probably causing the result you are getting.

Rick

Hello Rick,
Thanks for pointing to the mistake.
I have uploaded the same circuit using an additional V-source
to solve the problem. It's common in SPICE to use a V-source
with 0V for current measurement.

Files > Temp > TEC-Model1.asc

Best regards,
Helmut