Time Step too small in EWB

[Sharptop]

In Electronic Workbench I am getting the error

Output from instrument analysis

TRAN: Timestep too small; time = 0.029452, timestep = 1.25e-015:
trouble with node $20:xu1

doAnalyses: timestep too small

I set the time step manually but still get the error and I do not see a
node $20.

 

[Kevin Aylward]

In Electronic Workbench I am getting the error

Output from instrument analysis

TRAN: Timestep too small; time = 0.029452, timestep = 1.25e-015:
trouble with node $20:xu1

This is a node internally in the .subckt model, of probable, u1.

doAnalyses: timestep too small

I set the time step manually but still get the error and I do not see
a node $20.

It doesn't matter what you set the minimum time step, this message means
that internally the circuit isn't converging.

There are many reasons for non convergence. Check for floating nodes,
and unrealistic circuit design.

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

 

[Winfield Hill]

Kevin Aylward wrote...

It doesn't matter what you set the minimum time step, this
message means that internally the circuit isn't converging.
There are many reasons for non convergence. Check for
floating nodes, and unrealistic circuit design.

Right... e.g., add a bit of G-ohm leakage resistance to ground
on high-Z nodes, add some series resistance for inductors, ditto
for caps (esr) if in a series loop, etc. Mostly it's just stuff
that always exists with real components in real circuits.

 

[Jim Thompson]

In Electronic Workbench I am getting the error

Output from instrument analysis

TRAN: Timestep too small; time = 0.029452, timestep = 1.25e-015:
trouble with node $20:xu1

doAnalyses: timestep too small

I set the time step manually but still get the error and I do not see a
node $20.

node $20 should be in subcircuit xu1

Make sure you have a ground node, 0 (zero).

Make sure your circuit has realistic impedances... ideal inductors can
ruin your day ;-)

...Jim Thompson

 

[Winfield Hill]

Jim Thompson wrote...

Make sure your circuit has realistic impedances... ideal inductors
can ruin your day ;-)

Right. Standard spice inductors have zero resistance, which means
they have infinite Q. Standard spice capacitors also have zero
resistance, which means they have infinite Q. These two components
often occur together (all real inductors have self capacitance, and
real nodes have capacitance to ground, etc.), potentially creating
resonances with infinite Q. How is spice supposed to be able to deal
with that? It's up to the user to create real components, by adding
appropriate lossy resistances.