LTspice

Introduction

LTspice (by Analog Devices, formerly Linear Technology) is a SPICE simulation tool for analog circuit design. KiCad provides a schematic-only importer for LTspice files (LTspice has no layout capability).

Supported file types:

  • .asc — LTspice schematic (the import entry point)

  • .asy — LTspice symbol definition (consumed during import to reconstruct component graphics and pin definitions)

Both file types are plain text, line-oriented formats. Each line begins with an uppercase keyword followed by space-separated parameters. The parser splits lines on spaces and reconstructs multi-word values (such as SYMATTR values containing spaces) by concatenating all tokens from the value position onward. Files may use either LF or CR+LF line endings; trailing carriage returns are stripped during parsing.

Schematic Format (.asc)

An .asc file describes one schematic sheet. It contains a header declaring the version and sheet dimensions, followed by an unordered sequence of element lines.

Keywords

Keyword Description

VERSION

File format version number

SHEET

Sheet number and dimensions

SYMBOL

Component instance placement

WIRE

Electrical connection between two points

FLAG

Net label or power symbol

DATAFLAG

Data expression marker attached to a wire

LINE

Graphical line

CIRCLE

Graphical circle

ARC

Graphical arc

RECTANGLE

Graphical rectangle

TEXT

Text annotation or SPICE directive

WINDOW

Attribute display position override (follows a SYMBOL)

SYMATTR

Symbol attribute value override (follows a SYMBOL)

IOPIN

Hierarchical I/O pin marker

BUSTAP

Bus tap connection

VERSION

Declares the file format version.

VERSION <version>

The version may be an integer (4) or a dotted pair (4.1). When a dot is present, the major and minor parts are parsed separately.

SHEET

Declares the sheet number and drawing area size.

SHEET <sheet_number> <width> <height>

All three parameters are integers. The width and height define the drawing area in LTspice coordinate units.

SYMBOL

Places a component instance on the schematic.

SYMBOL <name> <x> <y> <orientation>
name

Symbol name or library-relative path. Backslashes in the name are converted to forward slashes for cross-platform path resolution (e.g., Opamps\UniversalOpamp2 becomes Opamps/UniversalOpamp2).
x, y

Placement position in LTspice coordinates.
orientation

One of the eight orientation values.

After a SYMBOL line, any number of WINDOW and SYMATTR lines may follow. These modify the most recently declared symbol.

WIRE

Defines an electrical connection between two points.

WIRE <x1> <y1> <x2> <y2>

All four parameters are integer coordinates.

FLAG

Places a net label at a point.

FLAG <x> <y> <name>

A FLAG with the name 0 is converted to a GND power symbol during import. All other names become global labels. The font size defaults to 2.

DATAFLAG

Places a data expression marker.

DATAFLAG <x> <y> <expression>

Data flags are imported as directive labels. The font size defaults to 2.

LINE

Draws a graphical line on the schematic.

LINE <line_width> <x1> <y1> <x2> <y2> [<line_style>]
line_width

Normal or Wide (case-insensitive).
x1, y1

Start point.
x2, y2

End point.
line_style

Optional integer, defaults to 0. See Line Style Values.

CIRCLE

Draws a graphical circle. The circle is defined by its bounding rectangle.

CIRCLE <line_width> <x1> <y1> <x2> <y2> [<line_style>]
line_width

Normal or Wide.
x1, y1

First corner of the bounding rectangle.
x2, y2

Opposite corner of the bounding rectangle.
line_style

Optional integer, defaults to 0. See Line Style Values.

The center is computed as ((x1+x2)/2, (y1+y2)/2) and the radius as (x1-x2)/2.

ARC

Draws a graphical arc. The arc is inscribed in a bounding rectangle, with explicit start and end points that lie on the arc. The arc is drawn counterclockwise from the start point to the end point.

ARC <line_width> <x1> <y1> <x2> <y2> <start_x> <start_y> <end_x> <end_y> [<line_style>]
line_width

Normal or Wide.
x1, y1

First corner of the bounding rectangle.
x2, y2

Opposite corner of the bounding rectangle.
start_x, start_y

Arc start point.
end_x, end_y

Arc end point.
line_style

Optional integer, defaults to 0. See Line Style Values.
In .asc files the parser swaps start and end points: the token labeled "start" in the file is stored as the arc end, and vice versa. This does not occur in .asy files.

RECTANGLE

Draws a graphical rectangle.

RECTANGLE <line_width> <x1> <y1> <x2> <y2> [<line_style>]
line_width

Normal or Wide.
x1, y1

First corner.
x2, y2

Opposite corner.
line_style

Optional integer, defaults to 0. See Line Style Values.

TEXT

Places a text annotation or SPICE directive.

TEXT <x> <y> <justification> <font_size> <value>
x, y

Text position.
justification

See Justification Encoding.
font_size

Integer font size (1—​7).
value

The text content. Multi-word values span to the end of the line.

Text values use prefix characters to indicate SPICE directives versus comments:

  • Values starting with ! are SPICE directives. The leading ! is stripped and subsequent `! ` sequences are converted to line breaks.

  • Values starting with ; are comments. The leading ; is stripped and subsequent `; ` sequences are converted to line breaks.

  • The escape sequence \n is converted to a line break in all cases.

WINDOW

Overrides the display position of a symbol attribute field. Must follow a SYMBOL line.

WINDOW <number> <x> <y> <justification> <font_size>
number

Window number identifying which attribute field to position. See Window Number Mappings.
x, y

Display position relative to the symbol origin.
justification

See Justification Encoding.
font_size

Integer font size. A font size of 0 hides the field.

If a WINDOW line in an .asc file specifies a window number that already exists in the symbol’s .asy definition, the .asc values override the .asy values.

SYMATTR

Sets a symbol attribute value. Must follow a SYMBOL line.

SYMATTR <key> <value>

The key is stored in uppercase. The value spans to the end of the line. A value of "" (two double-quote characters) is treated as an empty string. See SYMATTR Keys for known attribute keys.

IOPIN

Marks a hierarchical I/O pin location.

IOPIN <x> <y> <polarity>
polarity

One of In, Out, or BiDir (also accepted as I, O, B).

IOPINs are matched to FLAG elements at the same coordinates to determine the pin name. The matched FLAG is consumed and not imported as a separate net label.

BUSTAP

Defines a bus tap connection.

BUSTAP <x1> <y1> <x2> <y2>

Wires connected to the bus tap’s start point are promoted to the bus layer.

Orientation Encoding

Symbols can be placed in eight orientations, combining rotation and mirror operations. The orientation value appears as the last parameter of a SYMBOL line.

Value Rotation Mirror KiCad Transformation

R0

0deg

No

No transformation

R90

90deg CW

No

Rotate 180deg then rotate 90deg CCW

R180

180deg

No

Rotate 180deg

R270

270deg CW

No

Rotate 90deg CCW

M0

0deg

Yes

Mirror about Y axis

M90

90deg CW

Yes

Mirror about Y axis then rotate 90deg CCW

M180

180deg

Yes

Mirror about X axis

M270

270deg CW

Yes

Mirror about Y axis then rotate 90deg CW

Justification Encoding

Text and window positions use justification strings to control alignment and orientation. The "V" prefix indicates vertical (90deg) text.

Value Horizontal Align Vertical Align Text Angle

Left

Left

Center

Horizontal

Center

Center

Center

Horizontal

Right

Right

Center

Horizontal

Top

Center

Top

Horizontal

Bottom

Center

Bottom

Horizontal

VLeft

Left

Center

Vertical

VCenter

Center

Center

Vertical

VRight

Right

Center

Vertical

VTop

Center

Top

Vertical

VBottom

Center

Bottom

Vertical

Invisible

 — 

 — 

Hidden

For multiline text, horizontal justification modes (Left, Center, Right) force vertical alignment to Top with a half-line-height offset. Vertical text modes (VLeft, VCenter, VRight) apply the same adjustment on the horizontal axis.

Pin justification uses a subset of these values (Left, Right, Top, Bottom, None and their vertical variants). The pin justification determines pin orientation during import: Left maps to pin pointing right, Right to left, Bottom to up, Top to down. A justification of None hides the pin name.

Line Style Values

Graphical elements (LINE, CIRCLE, ARC, RECTANGLE) accept an optional line style integer.

Value Style

0

Solid (default)

1

Dash

2

Dot

3

Dash-dot

4

Dash-dot-dot

Line Width Values

Value Width

Normal

5 units (default)

Wide

10 units

KiCad maps Normal to 6 mils and Wide to 12 mils stroke width.

Symbol Format (.asy)

An .asy file defines the graphical appearance and pin layout of a single LTspice symbol. The file shares many keywords with the .asc format but adds pin and symbol type definitions.

Keywords

Keyword Description

LINE

Graphical line (same syntax as .asc)

RECTANGLE

Graphical rectangle (same syntax as .asc)

CIRCLE

Graphical circle (same syntax as .asc)

ARC

Graphical arc (same syntax as .asc, without the start/end swap)

WINDOW

Attribute display position

SYMATTR

Symbol attribute definition

PIN

Pin definition

PINATTR

Pin attribute (follows a PIN)

SYMBOLTYPE

Symbol type declaration

PIN

Defines a symbol pin.

PIN <x> <y> <justification> <name_offset>
x, y

Pin location in symbol coordinates.
justification

Pin orientation and name visibility. See Justification Encoding.
name_offset

Integer offset for the pin name text.

After a PIN line, any number of PINATTR lines may follow to set pin attributes.

PINATTR

Sets an attribute on the most recently declared pin.

PINATTR <name> <value>

The value spans to the end of the line. Common pin attributes:

Attribute Description

PinName

Display name for the pin

SpiceOrder

Pin order in SPICE netlist

SYMBOLTYPE

Declares the symbol category.

SYMBOLTYPE <type>
Value Description

Cell

Standard component symbol (default)

Block

Block diagram or subcircuit symbol

Window Number Mappings

Window numbers identify which attribute field a WINDOW line positions. The importer maps a subset of these to KiCad fields; unmapped numbers are recognized but ignored.

Number Attribute Name KiCad Field Mapping

-1

PartNum

 — 

0

InstName

Reference

1

Type

 — 

2

RefName

 — 

3

Value

Value

5

QArea

 — 

8

Width

 — 

9

Length

 — 

10

Multi

 — 

16

Nec

 — 

38

SpiceModel

Sim.Name

39

SpiceLine

Sim.Params

40

SpiceLine2

 — 

47

Def_Sub

 — 

50

Digital_Timing_Model

 — 

51

Digital_Extracts

 — 

52

Digital_IO_Model

 — 

53

Digital_Line

 — 

54

Digital_Primitive

 — 

55

Digital_MNTYMXDLY

 — 

56

Digital_IO_LEVEL

 — 

57

Digital_StdCell

 — 

58

Digital_File

 — 

105

Cell

 — 

106

W/L

 — 

107

PSIZE

 — 

108

NSIZE

 — 

109

sheets

 — 

110

sh#

 — 

111

Em_Scale

 — 

112

Epi

 — 

113

Sinker

 — 

114

Multi5

 — 

118

AQ

 — 

119

AQSUB

 — 

120

ZSIZE

 — 

121

ESR

 — 

123

Value2

 — 

124

COUPLE

 — 

125

Voltage

 — 

126—​129

Area1—​Area4

 — 

130—​133

Multi1—​Multi4

 — 

134

DArea

 — 

135

DPerim

 — 

136

CArea

 — 

137

CPerim

 — 

138

Shrink

 — 

139

Gate_Resize

 — 

142

BP

 — 

143

BN

 — 

144

Sim_Level

 — 

146

G_Voltage

 — 

150

SpiceLine3

 — 

153

D_VOLTAGES

 — 

156

Version

 — 

157

Comment

 — 

158

XDef_Sub

 — 

159

LVS_Area

 — 

162—​166

User1—​User5

 — 

167

Root

 — 

168

Class

 — 

169

Geometry

 — 

170

WL_Delimiter

 — 

175

T1

 — 

176

T2

 — 

184

DsgnName

 — 

185

Designer

 — 

190

RTN

 — 

191

PWR

 — 

192

BW

 — 

201

CAPROWS

 — 

202

CAPCOLS

 — 

203

NF

 — 

204

SLICES

 — 

205

CUR

 — 

206

TEMPRISE

 — 

207

STRIPS

 — 

208

WEM

 — 

209

LEM

 — 

210

BASES

 — 

211

COLS

 — 

212

XDef_Tub

 — 
Only window numbers 0, 3, 38, and 39 are actively mapped to KiCad fields. All other window numbers are parsed without error but have no effect on the imported schematic.

SYMATTR Keys

SYMATTR lines set key-value attributes on symbols. Keys are stored in uppercase internally. The following keys are used during import:

Key Description

InstName

Reference designator (mapped to KiCad Reference field)

Value

Component value (mapped to KiCad Value field)

Value2

Secondary value (used as fallback or appended to simulation model)

Prefix

SPICE netlist prefix character (R, C, L, X, etc.)

Type

Device type for semiconductor model lookup

Description

Component description text

SpiceLine

SPICE parameter string (mapped to Sim.Params)

SpiceLine2

Additional SPICE parameters

ModelFile

Path to external SPICE model file (mapped to Sim.Library)

The Prefix attribute has special significance for hierarchical design detection: a symbol whose .asy file lacks a Prefix attribute is treated as a sub-schematic rather than a component.

Coordinate System

LTspice uses an integer coordinate system with Y increasing downward. The coordinate scaling formula used during import is:

kicad_coord = MilsToIU( rescale( 50, ltspice_coord, 16 ) )

This maps 16 LTspice units to 50 mils (1.27 mm) in KiCad’s internal coordinate space. The inverse transform is:

ltspice_coord = IUToMils( rescale( 16, kicad_coord, 50 ) )

Page Centering

After converting all coordinates, the importer centers the design on the KiCad page. It computes a bounding box of all elements and offsets them to center on the page, clamping to a 10-grid margin if the design exceeds page dimensions. The offset snaps to a 50-mil grid.

Font Size Mapping

LTspice font sizes (1—​7) map to KiCad text sizes in mils:

LTspice Size KiCad Mils

1

36

2

42

3

50

4

60

5

72

6

88

7

108

A font size of 0 in a WINDOW definition within an .asy file is treated as size 2 (LTspice appears to ignore the hidden property from .asy files). A font size of 0 in an .asc WINDOW override hides the field.

SPICE Simulation Mapping

The importer translates LTspice component attributes into KiCad simulation fields (Sim.Device, Sim.Params, Sim.Library, Sim.Name, Sim.Type) based on the symbol’s Prefix attribute.

Prefix Sim.Device Behavior

R

R

Non-inferred passive; Sim.Params=R=${VALUE}

C

C

Non-inferred passive; Sim.Params=C=${VALUE}

L

L

Non-inferred passive; Sim.Params=L=${VALUE}

E, F, G, H

(prefix)

Controlled source; Sim.Params=gain=${VALUE}

B

V or I

Behavioral source; device is V for symbols starting with BV, I for BI

T

TLINE

Transmission line; value is passed directly as Sim.Params

V, I

SPICE

Voltage/current source with type and model parameters

X

SUBCKT

Subcircuit; SpiceLine becomes Sim.Params

(other)

SPICE

Generic SPICE device with model library lookup

For generic SPICE devices, the importer resolves model libraries from:

  • The ModelFile symbol attribute

  • The Type attribute matched against standard library files (standard.dio, standard.bjt, standard.jft, standard.mos)

  • Include paths discovered from .include, .inc, and .lib SPICE directives in TEXT elements

Hierarchical Design Detection

A symbol is treated as a hierarchical sub-schematic when its .asy file does not contain a SYMATTR Prefix line. The absence of a Prefix attribute signals that the symbol represents a sub-circuit sheet rather than a component.

When a sub-schematic is detected:

  • A corresponding .asc file is loaded as a child sheet.

  • The symbol graphics from the .asy file are drawn directly on the parent sheet (not as a KiCad symbol), and a KiCad sheet object is sized to match.

  • IOPIN elements in the .asc file become hierarchical labels.

  • Wires connecting to sub-schematic pin locations are adjusted to connect to the sheet boundary.

Imported Elements

  • Component instances with position, orientation (8-way rotation/mirror), and attribute overrides from WINDOW and SYMATTR lines

  • Symbol graphics (lines, rectangles, circles, arcs) from .asy files with line style and width mapping

  • Pins with name, position, and orientation from .asy definitions

  • Wires as electrical connections between two points

  • Net labels from FLAG elements (with 0 converted to GND power symbol)

  • Data expression markers from DATAFLAG elements as directive labels

  • Bus taps with wire-to-bus layer promotion

  • Text annotations and SPICE directives with font size mapping and multiline support

  • SPICE simulation fields (Sim.Device, Sim.Params, Sim.Library, Sim.Name, Sim.Type) derived from Prefix, Value, SpiceLine, ModelFile, and Type attributes

  • Hierarchical sub-schematics detected by the absence of a Prefix attribute, with IOPIN elements converted to hierarchical labels

  • Page centering with bounding box calculation and 50-mil grid snapping

Limitations

  • Custom LTspice symbol search paths are not supported.

  • Only global labels and directive labels are implemented; other label types are not handled.

  • Hierarchical sheet pin placement on sheet boundaries is not functional.

  • Many window number types are recognized but not mapped to KiCad fields (see the full window number table).

  • All pins are created as passive type regardless of actual pin function.

  • Window numbers outside the known set are silently ignored.

Undocumented Areas

  • The complete set of SYMBOLTYPE values beyond Cell and Block is unknown.

  • The purpose of dotted-pair version numbers (e.g., 4.1 vs 4) is unclear.