I am trying to import a new model, an AD633 multiplier, and have created a new symbol for it. However, I am getting a 'time step too small' type of error. I've tried increasing the Trtol value (as SgtWookie suggested in an older thread) bringing it up to over 20, but still have the same flavor of error.

Any suggestions? I've attached the model, symbol (had to zip these to get them to attach) and circuit files.

Thank you for your help!

 

i had a problem like this yesterday, it was simply that the circuit stopped working.. crashed if you like.. very odd

 

I've got it! I followed the advice in this thread:
http://forum.allaboutcircuits.com/showthread.php?t=60825

and I was able to get it to work, now I just need to adjust my variable input voltage and current readings (slower time is needed I'm guessing?) to see how the IC reacts.

 

I'm attaching the files for the 'working' version. However, the simulation is very sensitive to the input values I enter. I'd appreciate if anyone could advise on what Spice settings I could change to help stabilize it (so that I can vary the input in 1 us time frames and test the slew rate / bandwidth of the IC in the model).

Thanks!

 

I tried grounding all the inputs (X1, X2, Y1, Y2 and Z), leaving only W connected to ground via a 1k resistor; timestep error.

The only way I could get it to complete running was to leave X1 and Y1 open.

There's something strange going on with that model.

I looked in the Yahoo! LTSpice user group, and found this exchange:

> Hi,
>
> I can't get LTSpice to simulate AD633 correctly.
> My output Vout is railed when I used as in the
> schematic posted in the temp folder with the filename
> ad633test.rar
>
> Can someone please help me explain why the model is
> not working correctly? I expect the output Vout to
> be at -9.998V but I am getting it railed to the supply.
>
> Thanks in advance,
>


Hello,

All these multiplier models make a lot of trouble.

Solution for your circuit:
Either only use positive voltages on X1 or exchange the
connection on Y1 and Y2 when you use negative voltages.
You also need the Alternate solver for this circuit.
Control Panel -> SPICE -> Solver:Alternate

Files > Temp > ad633test_GLCc_pos.asc

Best regards,
Helmut

I tried the Alternate solver, and only positive inputs - then only negative inputs. Didn't help.

Another:

> Hi
>
> I'm trying to use the AD633 symbols previously discussed
> that are located in Files > Lib > AD633 but i'm having
> the problem that the simulation is extremely slow, a few
> nanoseconds per second. I have uploaded a file where i'm
> trying to use the ad633 for division (per the AD datasheet)
> to the "temp" folder called "ad633extract.asc". Any help
> greatly appreciated! Also i would be very happy to learn
> if there are other ways to perform division within LTSpice?
>
> Thanks
>
> Karl

Hello Karl,

This circuit requires the following settings to run your
circuit with the latest version of LTspiceIV, V4.06?.

1. Use the Alternate solver
Control Panel -> SPICE -> Solver:Alternate

2. You can gain simulation speed.
.options gmin=1e-10 abstol=1e-10 reltol=0.003

Remove or make this SPICE-directive to comment.
.options itl1=500 itl2=500

Files > Temp > ad633extract1.zip

Best regards,
Helmut

I'd tried the different solvers, tried the statements, nothing seems to work except to leave the inputs floating.

Instead of a transient analysis, try a DC analysis.

 

I'm attaching the files for the 'working' version. However, the simulation is very sensitive to the input values I enter. I'd appreciate if anyone could advise on what Spice settings I could change to help stabilize it (so that I can vary the input in 1 us time frames and test the slew rate / bandwidth of the IC in the model).

Thanks!

I didn't see your reply before I posted mine.

Don't bother trying to test the slew rate for this, as it's a macromodel, not a component model. You'll have to go by the specifications in the datasheet.

 

Hey Sgt, I tried the alternate solver (along with my latest sim settings, and slower input values in posts #2 & 3) and it did help to stabilize the simulation more. It's not perfect, but no model is, and I think it is good enough. Thanks for your help!