Prev: Speaking of high frequency transformer stuff...
Next: Repair water damaged Solar Garden Lamp
From: Jamie on 20 Feb 2010 21:02

I don't use LTspice a lot how ever, recently I have been poking around
with a simple buck circuit that just does not seem to do in spice as it
does in real life. I can put those little things aside how ever, I do
have a problem when changing values and then exec the sim. It pops up
with an error stating something on the line of
"Step size to small x.xxxxxx xxxxxx, error at NC_01"

that may not be the exact message but it's close..

This can happen just about any where on any component I change the
value on. To fix the problem, I decreas/increase the value by 1.

For example:
If change an inductor to 150uf, it didn't like that. I could
go larger or smaller, but I found that all I needed to do was to
add 1 or subtract 1 to make the sim happy.

This does not happen in just inductors, it happens with R's caps
etc..

Any one have something on that?


From: pimpom on 21 Feb 2010 04:53
Jamie wrote:
> I don't use LTspice a lot how ever, recently I have been
> poking
> around with a simple buck circuit that just does not seem to do
> in
> spice as it does in real life. I can put those little things
> aside
> how ever, I do have a problem when changing values and then
> exec the
> sim. It pops up with an error stating something on the line of
> "Step size to small x.xxxxxx xxxxxx, error at NC_01"
>
> that may not be the exact message but it's close..
>
> This can happen just about any where on any component I change
> the
> value on. To fix the problem, I decreas/increase the value by
> 1.
>
> For example:
> If change an inductor to 150uf, it didn't like that. I
> could
> go larger or smaller, but I found that all I needed to do was
> to
> add 1 or subtract 1 to make the sim happy.
>
> This does not happen in just inductors, it happens with R's
> caps
> etc..
>
> Any one have something on that?

I don't have an answer but I get similar errors from time to
time. I haven't been using LTSpice for very long either. When the
"error at...." message comes up, it's usually when I forget to
complete a connection and leave a node open. It may also happen
when one makes a connection that LTSpice doesn't understand.

I have even less clue about the "Step size too small" thing.
Until someone with more insight comes along to enlighten us, I
surmise that it happens when certain combinations of circuit
arrangement, component values and signal and measurement
parameters require more complex calculations than LTSpice wants
to attempt. Maybe multiple parasitic oscillations. I don't know.
Just guessing.


From: Helmut Sennewald on 21 Feb 2010 06:49
"Jamie" <jamie_ka1lpa_not_valid_after_ka1lpa_(a)charter.net> schrieb im
Newsbeitrag news:Yb0gn.1532$mn6.304(a)newsfe07.iad...
>
> I don't use LTspice a lot how ever, recently I have been poking around
> with a simple buck circuit that just does not seem to do in spice as it
> does in real life. I can put those little things aside how ever, I do
> have a problem when changing values and then exec the sim. It pops up with
> an error stating something on the line of
> "Step size to small x.xxxxxx xxxxxx, error at NC_01"
>
> that may not be the exact message but it's close..
>
> This can happen just about any where on any component I change the
> value on. To fix the problem, I decreas/increase the value by 1.
>
> For example:
> If change an inductor to 150uf, it didn't like that. I could
> go larger or smaller, but I found that all I needed to do was to
> add 1 or subtract 1 to make the sim happy.
>
> This does not happen in just inductors, it happens with R's caps
> etc..
>
> Any one have something on that?


Hello Jamie,

If the simulator stops with "time step too small", you should try some
options to help the solver.

1.

..tran 20m

Set a small time step in .TRAN , e.g 100n if you have a 100kHz switching
frequency.

..tran 0 20ms 0 100n

If it alreay fails at the beginning, you should try with the
option "startup" in the .TRAN command.
Sometimes additional ".nodeset" will help to get the simulation
started.

..tran 0 40ms 0 100n startup



I prefer to continue as shown below.

2..

Control Panel -> SPICE -> Reset to default
Control Panel -> Hacks -> Reset to default

There are some options which can be helpful. Try either one,
some or all in combination.
These are SPICE directives which you place in your schematic.

..options gmin=1e-10
..options abstol=1e-10
..options reltol=0.003

3.

If that fails, you could try with the Alternate solver.
Therefore don't use any option from above orr set them to their default
values.


Control Panel -> SPICE -> Reset to default
Control Panel -> SPICE -> Solver: Alternate

The default values:
..options gmin=1e-12
..options abstol=1e-12
..options reltol=0.001




4.

If it still fails, go back to the normal solver.

Control Panel -> SPICE -> Solver: Normal

Use the following only as the last option, because it can have a
lot of side effects, especially if you have used a larger value
for cshunt.

..options cshunt=1e-15

This adds a capacitor with 1fF from every node to GND.
I wouldn't go higher than 1e-14.

You should also use a combination of these options as in 2) in this case.
..options gmin=1e-10
..options abstol=1e-10
..options reltol=0.003


Best regards,
Helmut



From: Wimpie on 21 Feb 2010 09:57
On 21 feb, 03:02, Jamie
<jamie_ka1lpa_not_valid_after_ka1l...(a)charter.net> wrote:
>   I don't use LTspice a lot how ever, recently I have been poking around
> with a simple buck circuit that just does not seem to do in spice as it
> does in real life. I can put those little things aside how ever, I do
> have a problem when changing values and then exec the sim. It pops up
> with an error stating something on the line of
>   "Step size to small  x.xxxxxx xxxxxx, error at NC_01"
>
>   that may not be the exact message but it's close..
>
>   This can happen just about any where on any component I change the
> value on. To fix the problem, I decreas/increase the value by 1.
>
>   For example:
>      If change an inductor to 150uf, it didn't like that. I could
> go larger or smaller, but I found that all I needed to do was to
> add 1 or subtract 1 to make the sim happy.
>
>    This does not happen in just inductors, it happens with R's caps
> etc..
>
>    Any one have something on that?

Hello Jamie,

In addition to the good tips of Helmut, you may check your circuit for
unrealistic components. A real inductor has loss that you can model
with resistors and capacitors.

To increase the simulation speed and/or solve convergence problems,
you can add a resistor in parallel with problematic inductors. You may
add a capacitor in series with the parallel resistor when the effect
on circuit behavior is too large.

Good luck with getting your simulation to run!

Wim
PA3DJS
www.tetech.nl
without abc, PM will reach me.
From: MooseFET on 21 Feb 2010 10:32
On Feb 21, 6:57 am, Wimpie <wimabc...(a)tetech.nl> wrote:
> On 21 feb, 03:02, Jamie
>
>
>
> <jamie_ka1lpa_not_valid_after_ka1l...(a)charter.net> wrote:
> >   I don't use LTspice a lot how ever, recently I have been poking around
> > with a simple buck circuit that just does not seem to do in spice as it
> > does in real life. I can put those little things aside how ever, I do
> > have a problem when changing values and then exec the sim. It pops up
> > with an error stating something on the line of
> >   "Step size to small  x.xxxxxx xxxxxx, error at NC_01"
>
> >   that may not be the exact message but it's close..
>
> >   This can happen just about any where on any component I change the
> > value on. To fix the problem, I decreas/increase the value by 1.
>
> >   For example:
> >      If change an inductor to 150uf, it didn't like that. I could
> > go larger or smaller, but I found that all I needed to do was to
> > add 1 or subtract 1 to make the sim happy.
>
> >    This does not happen in just inductors, it happens with R's caps
> > etc..
>
> >    Any one have something on that?
>
> Hello Jamie,
>
> In addition to the good tips of Helmut, you may check your circuit for
> unrealistic components. A real inductor has loss that you can model
> with resistors and capacitors.
>
> To increase the simulation speed and/or solve convergence problems,
> you can add a resistor in parallel with problematic inductors. You may
> add a capacitor in series with the parallel resistor when the effect
> on circuit behavior is too large.
>
> Good luck with getting your simulation to run!

It is better to use the values that are part of the inductor rather
than adding ones. Right click on the inductor and fill in the stray
values. The solver runs faster with them built into the part because
it has an extra optimization for that.

>
> Wim
> PA3DJSwww.tetech.nl
> without abc, PM will reach me.

 |  Next  |  Last
Pages: 1 2 3
Prev: Speaking of high frequency transformer stuff...
Next: Repair water damaged Solar Garden Lamp