Things you should know about LTSpice

[gerrydevis]

Hello Friends.
Might be easier if I explain what I'm doing. I have an opamp constant current source that is varied by the voltage on its non-inverting input. I want to model the current through the load output by varying a potentiometer on the non-inverting input. I started out varying the value of the resistive elements of the pot and plotting on a paper graph the load current but was thinking there must be an easier way to do this with such a basic circuit / simulation.

The step does work as it gives me various curves, except its difficult to work out what curves (flat DC current lines actually) relate to what values.

 

[gaetan8888]

Hello

I've done many sim with LTspice. But wen, in some amps circuits, I ad a boost filter it's change totally the distortion FFT spectrums, boosting much more the distortion than it could possibly normally happen.

I have done a small 50 w amp sim, as an example, to show the problem, in the second amps I've add a 5 db treble boost in the gnfb. Even if we count the 5 db boost, it should not do so much more distortions.

Which setting I have to change to get it right ?

I include a zip file of the .asc files of the two amps.

Thank you

Bye

Gaetan

 

[mightydub]

Hello Friends.
Might be easier if I explain what I'm doing. I have an opamp constant current source that is varied by the voltage on its non-inverting input. I want to model the current through the load output by varying a potentiometer on the non-inverting input. I started out varying the value of the resistive elements of the pot and plotting on a paper graph the load current but was thinking there must be an easier way to do this with such a basic circuit / simulation.

The step does work as it gives me various curves, except its difficult to work out what curves (flat DC current lines actually) relate to what values.

see the wiki description of the .step command (Useful Commands - diyAudio) it has a description of how to understand which trace is which value.

 

[mightydub]

Gaetan -

you need to name the net you want to run the FFT on (for example amp_out) and change your .four command:

.four {freq} 9 8 V(amp_out)

That will run the FFT over 8 cycles of the node named amp_out and display results for 9 harmonics.

Try running the basic simulation for different time periods and seeing if the .four results stay constant. If not then it is probably caused by voltage drift on C14. Try replacing C14 with a voltage source (set it to 0) and see if you get consistent .four results.

Discussion of all of the above is on the wiki Common Issues Encountered By New Users - diyAudio

see THD measurement and Slanted FFT topics

 

[gaetan8888]

Hello

Here is my the parameter that I use.


;ac oct 10 10Hz 10000000Hz
;op
.param num_fft_pts 65532
.param freq 20k
.param timestep {1/((num_fft_pts-1)*freq)}
.options plotwinsize=0
.tran 5m


Thank

Bye

Gaetan

 

[Rafael L]

Try this:

SINE(0 1 {freq}) (source)

.four {freq} V(OUT)
.options plotwinsize=0
;tran 0 2m 0 {timestep}
.param timestep {1/((num_fft_pts-1)*freq)}
.param freq 20k
.param num_fft_pts 6550

 

[gaetan8888]

Hello

Reading the Common_Issues_Encountered_By_New_Users wiki, it seem that my problem is a Slanted FFT.

I did replace c14 with a voltage sources but nothing changed.

The image are the circuit before replacing c14 with a voltage sources, the fft are same with and without replacing c14 with a voltage sources.

Bye

Gaetan

 

[jcx]

may be slow transient settling - give a start time in the .tran that allows it to settle out

windowing also reduces the settling time effect - try Blackman window

.four and assoc params only applies to the legacy numerical output in the error log - not the graphic plot fft - you have to setup the graphic fft length, windowing, ect in the pop up window

you can experiment with the fft start, end time in the pop-up window

 

[mightydub]

Run the .tran for a long time (maybe 100m) and find where in the circuit there is DC drift. Since it is a bootstrapped design C9 is another likely suspect.

 

[gaetan8888]

Hello

I did run the .tran at 200ms

At the node C14 and R6 it seem to be the dc drift, I've include an image of the sinewave.

Than

Bye

Gaetan

 

[jcx]

sometimes you can get a better starting bias point by using the .savebias, loadbias pair - initialize by saving the bias after a really long run - say several seconds in your example

then use .loadbias to start shorter analysis sims

it doesn't work as well as I'd like when HF dynamic signals are upsetting the bias since dynamic state - I thru C and V across L isn't saved

you could Hi Pass fliter the signal you want to look at - buffer with an E vcvs to avoid loading effects

 

[polsol]

Which Spice Models to use with LTSpice?

Hi,
I've just downloaded LTSpice and started to try it out. Most of the BJTs I need are not in the download package.
Looking at Fairchild they have both PSpice and HSpice models. Are either compatable with LTSpice?
Looking at the first post in the thread it was mentioned that a .TXT file might be available for BJT's presumably used in audio. Is there are link/reference for this?

Cheers

 

[unclejed613]

i think hspice models are compatible, but pspice models are easier to import to LTSpice. i seem to remember Hspice models needing a bit of modification to work right.

 

[mightydub]

You want the PSpice format models. I have dropped in PSpice models from Fairchild, OnSemi, TI, etc. with no problems.

 

[gaetan8888]

Hello jcx, mightydub and Rafael L

I've done experimenting with the fft start, end time in the pop-up window.

I did get better results now.

Thank guy's

Bye

Gaetan

 

[gaetan8888]

Hello

I have another question about LT Spice.

With some amps circuits, wen I do modifications and I check the distortions FFT, I get an inverted harmonic peak, like in the image I include.

What does it mean ?

Thank

Bye

Gaetan

 

[keantoken]

I have been trying to figure that out too.

My best guess is that that's the actual value of the harmonic. Not sure.

And I see the words "Rush Cascode" hiding in plain sight.

- keantoken

 

[gaetan8888]

Hello

That thd harmonics inverse peak was bugging few times me since I can not figure out what it is and if it is a good or bad thing.

Bye

Gaetan

 

[keantoken]

Just to be clear, I just think it's cool to see someone else looking at the Rush Cascode. If it's okay, I would like to hear your thoughts on it when you get the amp running.

I'm afraid I don't know why the negative peak is there; I always assumed it was harmless because it seemed to be a reasonable value of the harmonic at that point.

If it is an error, it is likely just an error in the FFT process.

Maybe I shouldn't have answered without a good response. :/

- keantoken

 

[unclejed613]

the "nverted" peak seems to be (and i have been using LTSpice for several years) an actual value. this seems to happen if you have a DC component to the signal being measured. LTSpice sees an actual value for (in many cases) a second or third harmonic, and it's lower than the present portion of the trace, so LTSpice draws a line down to it, then back up. if you eliminate the DC component, then you will see the tace at the noise floor going up to the harmonic that was shown as a dip.