Hello,
I have a project, which is to make audio amplifier, and for now, I have everything except distortion analysis. I have simulated the circuit, plotted the FFT in both decibel and linear representation. I also used .four directive to get distortion percentage. You can see everything from pictures. It doesn't look very good, and I don't know if it is because of the settings or my circuit?
I have a project, which is to make audio amplifier, and for now, I have everything except distortion analysis. I have simulated the circuit, plotted the FFT in both decibel and linear representation. I also used .four directive to get distortion percentage. You can see everything from pictures. It doesn't look very good, and I don't know if it is because of the settings or my circuit?
Attachments
Hello,
Here are the options that I use,
they adapt the tran sim parameters depending on the frequency.
input voltage:
SINE(0 1 {freq} 0 0)
.tran 0 {simtime} {dlytime} {timestep}
.options plotwinsize=0
.options method=gear
.options numdgt=7
.param Freq=1k
.param numcyc=50
.param dlycyc=5
.param FFT=2**16
.param simtime=numcyc/Freq+dlytime
.param dlytime=dlycyc/Freq
.param timestep=(simtime-dlytime)/FFT
.four {freq}15 8 V(Vout)
.four {freq}15 8 V(Vvas)
.four {freq} 4 8 V(Vout)
Regards,
Danny
Here are the options that I use,
they adapt the tran sim parameters depending on the frequency.
input voltage:
SINE(0 1 {freq} 0 0)
.tran 0 {simtime} {dlytime} {timestep}
.options plotwinsize=0
.options method=gear
.options numdgt=7
.param Freq=1k
.param numcyc=50
.param dlycyc=5
.param FFT=2**16
.param simtime=numcyc/Freq+dlytime
.param dlytime=dlycyc/Freq
.param timestep=(simtime-dlytime)/FFT
.four {freq}15 8 V(Vout)
.four {freq}15 8 V(Vvas)
.four {freq} 4 8 V(Vout)
Regards,
Danny
I don't know if it is because of the settings or my circuit?
In the end it's the circuit. Working .asc file attached. The only change to your circuit is that I added a miller capacitor to the VAS - your circuit was unstable and oscillating.
View attachment Uros11.asc
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
- Home
- Design & Build
- Software Tools
- Distortion simulation LTSpice