Problem simulating poweramp in LTSPICE

[akkar]

Hello everyone,

I'm trying to simulate my poweramp (already builded and working) in ltspice

No matter what I do but I can't get any current through the two mosfets (it should be regulated via P2 - P2a and P2b in my file)

Here you can find the files
Amp - Google Drive

 

[abraxalito]

You havn't filled in 'Ncycles' in your two AC voltage sources - put in a reasonable number there like 5000. Then you'll see the amp comes to life but I suspect you're not able to get enough bias for those MOSFETs because either your current source is too low or the bias spreader resistance is too small.

 

[indra1]

P2b is shorted, any value there makes no difference, give P2a some value.

 

[abraxalito]

You'd get it going quicker if you dispensed with the AC voltage sources and used DC voltage sources for your rails until you've got the bias conditions set up correctly. Then you can use AC analysis which will calculate your operating point more quickly than waiting to see what happens with transient analysis.

 

[akkar]

Even by setting 5000 Ncycles and setting the P2 pot half way (P2a = 250, P2b = 500)
I get no current through the mosfets

I've updated the file in Google Drive

 

[indra1]

P2a too small, try > 1k5.

 

[akkar]

Yes it works but I still don't get why in the real amp I'm using a 500ohm trimpot and still get 120mA in both mosfets.

Also, using P2a = 530ohm and V+,V- = 42V I get 120mA in mosfet M2 but only 90mA in M1.
Can it be a problem with models?

 

[abraxalito]

If you're using IRF MOSFETs (which are verticals) you're very unlikely to get a stable bias current without some temperature compensation. Are you using lateral FETs in the real amp?

 

[akkar]

No, I'm using the exact same models you see in the LTSPICE file

Should I set a temperature in the simulator?

 

[abraxalito]

Here's an idea - measure the voltage between the gates of the two output FETs on your real amp.

 

[akkar]

Between the two gates I've 7,5V

 

[abraxalito]

I'm getting 5.4mA in your CCS (Q4,Q5) which indicates you'd need 1k4 for your bias spreader to get 7.5V between your gates. So your 500R trimpot is in series with what resistor value?

Incidentally your 120mA/90mA bias split is most likely caused by a DC offset at the output.

Snipping the short across P2b I'm now getting 60/80mA which is fairly close agreement with your real world amp. Remember vertical MOSFETs have a strong negative gate threshold voltage coefficient, meaning the bias increases as they warm up. The model doesn't simulate that.

 

[akkar]

Trimpot is in series with 1k as in the file.

Is there a way to simulate that warm up?

 

[indra1]

... Can it be a problem with models?

It is not a problem, it is a model, not the real parts you use. Not every characteristic of a part is modeled. I do not think it is worth the effort to accurately measure and make a model for the real parts you use.