Maker Pro
Maker Pro

LTspice issues.

J

Jamie

Jan 1, 1970
0
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?
 
P

pimpom

Jan 1, 1970
0
Jamie said:
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.
 
H

Helmut Sennewald

Jan 1, 1970
0
Jamie said:
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
 
J

Jamie

Jan 1, 1970
0
pimpom said:
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.
I have come to the conclusion there is a bug in it. Because when I
receive this error, changing a value enough to make it happy allows a
SIM operation. Then after a SIM run, I can go back and change that same
component to the value I had that generated the error to which it will
then exec the SIM with no problems.

Since I do a lot of coding my self, I see this as an initiation problem
of variables or something of that sort on start up!.

I don't recall seeing this problem before the last update that was
done. But then again, I'm getting old and memory loss maybe an issue :)
 
H

Helmut Sennewald

Jan 1, 1970
0
Jamie said:
As I indicated in another message, I found that after I make the SIM
happy, I run a SIM and if I change the values back to where they were that
caused the problem, I can rerun SIM with no issues ;/

Something is wrong with the software. A initiation problem perhaps?

BTW.
I do use the options in the control panel to make it nearest to
real world operation as possible. Nice features btw and still learning
what most of them do, good thing there are docs :)

I tried a combination of things and no matter what I did, once the error
was there, it just wasn't going to start. This error takes place
at the very beginning. It does not happen once the annalistic data starts
collecting.

Who knows, maybe one day I'll track it down..


Hello Jamie,

Can you send me one example for trying?

Best regards,
Helmut
 
H

Helmut Sennewald

Jan 1, 1970
0
Jamie said:
As I indicated in another message, I found that after I make the SIM
happy, I run a SIM and if I change the values back to where they were that
caused the problem, I can rerun SIM with no issues ;/

Something is wrong with the software. A initiation problem perhaps?

BTW.
I do use the options in the control panel to make it nearest to
real world operation as possible. Nice features btw and still learning
what most of them do, good thing there are docs :)

I tried a combination of things and no matter what I did, once the error
was there, it just wasn't going to start. This error takes place
at the very beginning. It does not happen once the annalistic data starts
collecting.

Who knows, maybe one day I'll track it down..

Hello Jamie,

Maybe you feel it's different, because LTspice nowadays tries with
"pseudo transient analysis" to find the operating point when the classic
methods failed.
Older versions simply started with the transient simulation even without
having found an operating point.
You could suppress this method with this SPICE-directive.
..options ptrantau=0

Best regards,
Helmut
 
J

Jamie

Jan 1, 1970
0
Helmut said:
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
As I indicated in another message, I found that after I make the SIM
happy, I run a SIM and if I change the values back to where they were
that caused the problem, I can rerun SIM with no issues ;/

Something is wrong with the software. A initiation problem perhaps?

BTW.
I do use the options in the control panel to make it nearest to
real world operation as possible. Nice features btw and still learning
what most of them do, good thing there are docs :)

I tried a combination of things and no matter what I did, once the
error was there, it just wasn't going to start. This error takes place
at the very beginning. It does not happen once the annalistic data
starts collecting.

Who knows, maybe one day I'll track it down..
 
J

Jamie

Jan 1, 1970
0
Wimpie said:
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.
Thanks.

But toggling the values between SIMS does not explain why I can get it
to SIM with the values that originally generated the problem.

Oh well. One day I may find out the issue.
 
J

Jamie

Jan 1, 1970
0
Helmut said:
Hello Jamie,

Maybe you feel it's different, because LTspice nowadays tries with
"pseudo transient analysis" to find the operating point when the classic
methods failed.
Older versions simply started with the transient simulation even without
having found an operating point.
You could suppress this method with this SPICE-directive.
.options ptrantau=0

Best regards,
Helmut
I'll keep that noted, I don't remember seeing this in older versions, It
may have something to do with it.

Thanks.
 
F

Fred Abse

Jan 1, 1970
0
If change an inductor to 150uf, it didn't like that.

Changing inductors to capacitors can have lots of consequences :)

Assuming that you didn't actually mean what you wrote, try using the
"alternative" solver for a start.

Maybe post the .asc file and people might take a look at it.
 
Top