simulation of a hybrid amp : so long

[UltimateX86]

hello,

i'm trying to simulate a hybrid amp with LTspice, but it's really long, do you have any advice?

thanks

best regards
Sébastien

 

[Ray Waters]

You can sometimes work around convergence issues by changing the simulation parameters in LTspice. In this case, using the "alternate" solver will allow the simulation to run normally.

This option is available on the SPICE tab under the Control Panel menu item. Note that this is a persistent setting; LTspice will remain in this mode until you explicitly change back to the "normal" solver.

 

[gearheadgene]

Your LT spice deck simulated fine for me, and quickly. What exactly is not working for you?

By the way...the filament portion of the schematic appears to be incorrect. The diodes are facing the wrong way, yes? I think 48V +/- should be reversed.

 

[gearheadgene]

BTW, the LTSpice schematic shows floating input signal. Maybe you meant to have a differential input, ground referenced? Use 2 voltage sources in series, for example, and ground the common point.

 

[Ray Waters]

Your LT spice deck simulated fine for me, and quickly. What exactly is not working for you?

The OP might have been using LTspice IV instead of LTspice XVII. I have both versions installed on my PC and there were indeed convergence issues with IV that I didn't see with XVII. I also found that the simulation ran normally as drawn under LTspice XVII.

 

[gearheadgene]

10-4....I get the same result in LTSpice IV.

It doesn't like the model for the MOSFET very much. Look at the Error Log for details.

More importantly, change the solver to use "alternate" instead of "normal" and the simulation runs. It stutters for a second then completes in just a couple of seconds.

 

[Ray Waters]

Yep, see my post #2. 🙂

 

[Koonw]

Change C1, C2 to 0.22u instead of 0.22, the sim speed should be normal as expected.

 

[Ray Waters]

Good catch!!

 

[UltimateX86]

You can sometimes work around convergence issues by changing the simulation parameters in LTspice. In this case, using the "alternate" solver will allow the simulation to run normally.

This option is available on the SPICE tab under the Control Panel menu item. Note that this is a persistent setting; LTspice will remain in this mode until you explicitly change back to the "normal" solver.

Thanks, with alternate it's instantaneous !

I have never used alternate, I will do some research on the subject

BTW, the LTSpice schematic shows floating input signal. Maybe you meant to have a differential input, ground referenced? Use 2 voltage sources in series, for example, and ground the common point.

yes I have an XLR input, do you really have to use two sources? is it annoying for the simulation?

Change C1, C2 to 0.22u instead of 0.22, the sim speed should be normal as expected.

yes it comes from there !! thanks