LTspice simulator stops with "time step too small" message
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
5. 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
http://www.electronicspoint.com/ltspice-issues-t217902.html
沒有留言:
張貼留言
注意：只有此網誌的成員可以留言。