Blameless THD

[nicholas1113]

Hey
I really need some help with my high THD ... i really dunno what happen to my High THD can anyone help me giving me some advise with 10hz THD is 0.0006% .. but i simulated a 73% for the Blameless power Amplifier.

I really need some help since I have stucked.

Below is the Blameless.asc and also the Diagram of the THD result .
Mind everyone for the help!

View attachment ClassB(THD8ohm).txt

 

[jaycee]

add .options plotwinsize = 0 to your spice diagram. also you will have to simulate at a small timestep like 0.05u.

Post your LTSPICE .ASC file and we can help more

 

[megajocke]

The models used were not included so I couldn't test your simulation but with a simulation length of only 15ms you are not going to get any information on the 10Hz distortion.

 

[godfrey]

This gives sensible results:

.four 0.01kHz V(OUTPUT)
.tran 0 500m 100m 0.1m

 

[h_a]

Well, the output clearly shows he's simulating 10kHz, not 10Hz. That's a much more reasonable number.

Likely you're DC-operating points are completely banana.

Always distrust the computer.

Have fun, Hannes

 

[megajocke]

Oh, that's right too. There is a mismatch between the signal source which was set to 10 Hz and the .four command set to 10 kHz.

 

[nicholas1113]

Well, the output clearly shows he's simulating 10kHz, not 10Hz. That's a much more reasonable number.

Likely you're DC-operating points are completely banana.

Always distrust the computer.

Have fun, Hannes

What does it mean by DC-operating points are completely banana?
How does it know ?

 

[nicholas1113]

add .options plotwinsize = 0 to your spice diagram. also you will have to simulate at a small timestep like 0.05u.

Post your LTSPICE .ASC file and we can help more

I have post the .txt file and you can change to .asc .
thank you

 

[nicholas1113]

This gives sensible results:

.four 0.01kHz V(OUTPUT)
.tran 0 500m 100m 0.1m

Ya man ... the THD is lower but it should be 0.0006% in the BLameless ..
IS the input voltage frequency should be same as 0.01K for the command of
.four 0.01kHz V(OUTPUT)?
Are they the same?

 

[h_a]

How does it know ?

Any amp you want to simulate you need to know very well first. You need to understand how it works and what the DC-working points (currents, voltages) are. Otherwise you cannot be sure that the results are worth the time you needed to generate them. A simulator does not replace basic understanding of the circuit.

However, first you should read the wikipedia-article on distortion

I'm sure then it's more clear what signal to put in (1kHz) and what to analyze for (1kHz).

Have fun, Hannes

 

[nicholas1113]

Hey.

If the longer Time Stop the make the Distortion to be more accurate?

Another question, What is the optimal Frequency if the stop time is 2000m?
Cause I use .trans 2000m 1m 0.01m as the command to operate a 10Hz of Input voltage. But i dunno does the Frequency is suitable or not?

Also what is the Suitable Step time for a suitable Frequency?

 

[wahab]

there must be enough cycles...10 is enough generaly,at least in my
simulator whch is not ltspice..so set up the stop time accordingly..
a 20ns step time is enough at 10khz..
if you decrease the frequency, don t decrease the step time
colinearly, stay at 50ns for 1khz, and so on..

 

[krachkiste]

Interesting - why is that (with the time step)

I usually simulate 10 cycles with timestep 101n7 for 1kHz
and 10n1 for 10kHz. (no real reason for these values - they are easy to type, and they don't divide the cycletime I suppose)

You must take a look at the actual waveform that you fft. this way you can make sure it isn't heavily distorted (clipped).
Also check the bias conditions in the output devices.

In real life the BC5?7 and BC8?7 devices are rated at max 45Vce. So if you actually built that amp with these devices in the VAS it is likely to go up in smokes.