Most frequently asked questions for beginners

From LTwiki-Wiki for LTspice
Revision as of 19:55, 19 August 2009 by Analogspiceman (talk | contribs)

What are the different LTspice file types?

Schematic:     name.asc   the drawing with your circuit (a text file)
Symbol:        name.asy   symbols for the schematic (a text file)
Netlist:   unprocessed netlist (text file viewable from within LTspice 
                          & usable by other SPICE engines) 
Logfile:       name.log   info and results from .four, .measure, .op (text file viewable 
                          from within LTspice); may also contain the fully processed
                          and expanded netlist (a Control Panel setting)
Result:        name.raw   binary output data file (text format may be optionally specified)
Result:        name.fft   binary result of an FFT
Plot settings: name.plt   text file used to save and restore Waveform Viewer plot settings
Model file:   text file containing model(s) - may be any valid file name
Circuit file:  name.cir   frequently used extension for an external netlist input file (text)

How do you copy and paste between schematics?

Click the Copy Icon in the tool bar or select Copy from the Edit drop down menu (or type ctrl-C).  Select (with the mouse) what you want to copy.  Make the target schematic active (click on it or its tab or type ctrl-Tab) and then click the Paste Icon in the tool bar or select Paste from the Edit drop down menu (or type ctrl-V).

How do I copy and paste between symbols in the symbol editor?

It is not possible to use copy and paste in the symbol editor.  Symbol files are ascii text.  Merge the text as described in message 7201 in the LTspice Yahoo Group.

How can I add intrinsic device models (BJTs, FETs, etc.) to LTspice?

Please take a look to the many examples in the files section of the LTspice Yahoo Group (Files => Lib).

How can I add subcircuits to LTspice?

You will find many answers when you search the LTspice Yahoo Group messages for words like "library", "symbol" or "FAQ".

Please read first the programs help:
Help -> Schematic Capture -> Editing Components -> Creating New Symbols
Help -> Help Topics ->FAQs -> Third party models
Help -> Help Topics ->FAQs -> Mosfet

You will find also help in the linked documents from our LTspice Yahoo Group.

Links -> Spice Courseware And Tutorials

There is another document about symbols and models in our Files section.

Files -> Tut -> Symbol Types For Subcircuits

I have a pulse source in my schematic with zero transition times.  LTspice only shows slow transition times of 2ns.  What's going on here?

PULSE(0 5 0 0 0 20n 100n)

LTspice automatically will use a default value for <trise> and <tfall> if these parameters are set to zero.  Default value: 10% of Ton or 10% of Tperiod-Ton whatever is smaller.  You must specify Trise and Tfall if you want a certain value.

PULSE(0 5 0 100p 100p 20n 100n)

Don't use steeper transitions than required by your application.

I have used a pure sine source in my schematic, but the output signal of my circuit looks slightly different from cycle to cycle.

LTspice has waveform compression enabled as the default setting.  This compression reduces the amount of saved data during the simulation.  It's a lossy compression and thus it can distort the saved signals.  You can switch it off with the following command line in your schematic.

.options plotwinsize=0

It could be switched off in the "Control Panel -> Compression" pane as well, but this setting will be lost upon closing the current session of LTspice.

How does one set the threshold and high/low voltages for LTspice's digital devices?

The default threshold is always (Vhigh+Vlow)/2 . Flipflops require either a Td or a Trise for correct operation under every condition.

Right-mouse-click on the device (instance) in the schematic.

  • SpiceLine: Vhigh=3V Ref=1.5
  • SpiceLine2: Td=5n Trise=3n

Schmitt devices have the threshold and hysteresis parameters Vt and Vh instead of Ref. Vup=Vt+Vh Vdn=Vt-Vh.