Control Panel    

From LTwiki-Wiki for LTspice
Jump to: navigation, search

The Control Panel is accessed in LTspice via the Control Panel hammer Icon Hammer.png Icon or the drop down menu items: Tools => Control Panel and sometimes Simulate => Control Panel.  This access is generally available in all LTspice window types (Schematic, Netlist Editor, Waveform Viewer, FFT Waveform Viewer).

The Control Panel is a dialog box organized like three rows of tabbed index cards:

Operation  Hacks  Internet
Netlist Options  Waveforms 
Compression Save Defaults  SPICE  Drafting Options
User options for the selected tab


LTspice compresses the raw data files as they are generated.  A compressed file can be 50 times smaller than the uncompressed one.  This is a lossy compression.  This pane of the control panel allows you to control how lossy the compression runs.

  • Window Size (No. of Points): Maximum number of points that can be compressed into two end points.
  • Relative Tolerance: The relative error allowed between the compressed data and the uncompressed data.
  • Absolute Voltage tolerance [V]: The voltage error allowed by the compression algorithm.
  • Absolute Current tolerance [A]: The current error allowed be the compression algorithm.

These compression settings are not remembered between program invocations to encourage use of the defaults.  They are available on the control panel for diagnostic purposes.  The tolerances and window size can be specified with option parameters plotreltol, plotvntol, plotabstol and plotwinsize in .option statements placed as SPICE Directives on the schematic.

Save Defaults

These settings are used when you don't explicitly state which nodes should be saved in a simulation.  Useful setting are "Save Device Currents", "Save Subcircuit Node Voltages", and "Save Subcircuit Device Currents".  Device voltages and internal device voltages are only of internal program development use.

  • Save Device Currents: Check this so that you can plot device and terminal currents.  You will also need it to be able to plot dissipation.
  • Save Subcircuit Node Voltages: You will need to check this to plot voltages in hierarchical designs.
  • Save Subcircuit Device Currents: You will need to check this to plot currents in hierarchical designs.
  • Don’t save Ib(), Ie(), Is(), Ig(): This saves only the collector(drain) currents of transistors in the interest of reducing the size of the output .data file.  This is useful for IC design, but it using it means that there isn't enough data available to compute transistor dissipation.
  • Save Device Currents: Check this so that you can plot device and terminal currents.  You will also need it to be able to plot dissipation.


This pane allows you to define the various defaults for LTspice.  These defaults can be overridden in any simulation by specifying the options in that simulation.  Usually you can leave these options as they are.  If you have frequently updated the program over the web, you might want to press Reset to Default Values to reset to the current recommended settings.

One default you may want to change is Trtol.  Most commercial SPICE programs default this to 7.  In LTspice this defaults to 1 so that simulations using the SMPS macromodels are less likely to show any simulation artifacts in their waveforms.  Trtol more affects the timestep strategy than directly affects the accuracy of the simulation.  For transistor-level simulations, a value larger than 1 is usually a better overall solution.  You might find that you get a speed of 2x if you increase trtol with out adversely affecting simulation accuracy.  Your trtol is remembered between program invocations.  However, most of the traditional SPICE tolerance parameters, gmin, abstol, reltol, chgtol, vntol are not remembered between program invocations.  If you want to use something other than the default values, you will have to write a .option statement specifying the values you want to use and place it on the schematic or keep the settings in a file and .inc that file.

Also interesting is which solver is used. LTspice contains two complete versions of SPICE.  One is called the normal solver and the other is called the alternate solver.  The alternate solver uses a different sparse matrix package with reduced roundoff error.  Typically the alternate solver will simulate at half the speed of the normal solver but with one thousand times more internal accuracy.  This can be a useful diagnostic to have available.  There is no .option to specify which solver is used, the choice must be made before the netlist is parsed because the two solvers use different parsers.

Check the box next to "Accept 3K4 as 3.4K" to force LTspice to understand a number written as 4K99 to be equal to 4.99K.  Normal SPICE practice does not allow this, but it is available in LTspice by popular request.

Drafting Options

  • Allow direct component pin shorts: Normally you can draw a wire directly through a component and the wire segment shorting pins is deleted. If you check it, the shorting wire will not be automatically deleted.
  • Automatically scroll the view: Checking this box makes the view of the schematic scroll as you move the mouse close the edge while
  • Mark text Justification anchor points: Draw a small circle to indicate the reference point of text blocks.
  • Mark unconnected pins: Draw a small square at each unconnected pin to flag it as unconnected.
  • Show schematic grid points: Start with visible grid enabled.
  • Orthogonal snap wires: Force wires to be drawn in vertical and horizontal segments while drawing.  If not checked, a wire can drawn at any angle and will snap to any grid.  Holding down the control key will momentarily toggle the current setting while drawing wires.
  • Cut angled wires during drags: During the Drag command, a non-orthogonal wire will be broken into two connected wires if you click along the middle of the wire.
  • Undo history size: Set the size of the undo/redo buffer.
  • Draft with thick lines: Increases the all line widths.  Useful for generating images for publication.
  • Show Title Block: For internal use.

Netlist Options

  • Convert 'µ' to 'u': Replace all instances of 'µ' to 'u'.  Useful if your MS Windows installation can't display a Greek Mu(as, e.g., some Chinese editions of Windows don't with default fonts) and (ii) generating netlists for SPICE simulators that don't understand the 'µ' character as the metric multiplier of 1e-6.
  • Reverse comp. order: Circuit elements are normally netlisted in the order in which they were added to the schematic.  Checking this box causes this order to be reversed.
  • Default Devices: Whenever a diode is used in an LTspice schematic, the default model statement .model D D is added to the netlist to suppress messages about using the default model.  Unchecking this option suppresses inclusion of this line as well as the analogous model statements for bipolar, MOSFET, and JFET transistors.
  • Default Libraries: Whenever a diode is used in an LTspice schematic, the default library, standard.dio, is included in the simulation by a .lib statement.  Unchecking this option suppresses inclusion of this library as well as the analogous library statements for bipolar, MOSFET, and JFET transistors.
  • Convergence Aids: For Internal program development use only.


"Sticky" settings are remembered between LTspice sessions.

  • Plot data with thick lines: "Sticky" selectable check box.
  • Use radian measure in waveform expression: "Sticky" selectable check box.
  • Replace "Ohm" with capital Greek omega: "Sticky" selectable check box.
  • Font: "Sticky."  System (fixed to size and style of System font) or Arial (sans serif proportional font with user selectable size).
  • Color Scheme: "Sticky."
  • Open Plot Defs: 
  • Hot Keys: "Sticky." LTspice allows Hot Keys to be (re)assigned to many of its functions.


Settings marked with an asterisk [*] are remembered between program invocations.

  • Marching Waveforms: Check to enable simulation results to be incrementally plotted during the simulation.
  • Generate Expanded Listing: Dump the flat netlist after expanding subcircuits to the in the SPICE Error Log file.
  • Open Demo circuits as regular schematics: Use [File] [Open] to open demo circuits in .\LTspiceIV\lib\app\*.app. All SPICE commands will be visible.  The schematic can be edited and saved to a new file.  The double dots '..' is for demo circuit display control use.  Only one dot is required for editing.
  • Don't warn when using preliminary models: Turn off the warning message for all preliminary models.  Note: All SMPS models are flagged as preliminary as a disclaimer.
  • Automatically delete .raw files: This allows waveform data files to be deleted automatically after closing a simulation.  This dramatically reduces the amount of disk space used by LTspice but requires the simulation to be rerun when you reopen the simulation.
  • Automatically delete .net files: This allows the schematic's netlist to be automatically deleted whenever the schematic is closed.  These files can be thought of as small temporary files and deleting them makes exploring the directory tidier.  They define the electrical connectivity of the schematic to the LTspice simulator.  Some people prefer not to delete them because they have further use for them.
  • Automatically delete .log files: This allows the simulation log to be automatically deleted whenever the simulation is closed. These files contain various simulation statistics such as elapsed time during the simulation, warning and error messages, and step parameters used for .step/.temp/.dc analyses.
  • Directory for Temporary Files: Directory for temporary storage of waveform and update files.


This pane was used for internal program development, but is currently almost obsolete.

Usually you can leave these options as they are.  If you have frequently updated the program over the web, you might want to press "Reset to Default Values" to reset to the current recommended settings.


This pane of the Control Panel is used for the incremental updates obtained from the web.  LTspice is often updated with new features and models.  Use the menu command Tools => Sync Release to update to the current version.  If you don’t update for a couple months, LTspice will begin to ask if you would like to check for updates.  LTspice never accesses the web without asking for your permission to do so.  LTspice contains no spyware or transmits any type of data while obtaining the files it need for update.

  • Don't cache files: Neither cache nor use files cached on our machine for the update.
  • Don't verify checksums: For security reasons, LTspice uses a proprietary and confidential 128 bit checksum algorithm to authenticate the files it receives off the web for updating.  This authentication can be disabled in case there's a error in that algorithm.  However, no problem with this has ever been reported, so it is not recommended that you ever defeat this security feature.

LTspice uses only high-level operating system calls for its Internet access.  It should not be required to make any adjustments to these settings except in rare cases when you need to specify the Proxy server and password since LTspice is not managing the Internet access, but your computer and operating system.  Settings on this pane are not remembered between program invocations.

blog comments powered by Disqus