Footprinter Strings

Overview

You can quickly specify the footprint and 3d model for any element by setting the footprint property to a string. Footprinter strings use a compact underscore-separated syntax (<package><pins>_<param><value>) to customize pitch, pad dimensions, body width, drill sizes, and thermal pads.

export default () => (
  <chip
    name="U1"
    footprint="0402"
  />
)

Common Parameter Modifiers

Modifier	Example	Meaning
p<length>	soic8_p1.27mm	Center-to-center pin pitch
w<length>	soic8_w3.9mm	Package body width
h<length>	qfn16_w3mm_h3mm	Package body height
pw<length>	0603_pw0.8mm	Individual SMD pad width
pl<length>	0603_pl0.9mm	Individual SMD pad length
id<length>	dip8_id0.8mm	Plated hole inner (drill) diameter
od<length>	dip8_od1.6mm	Plated hole outer (annular ring) diameter
thermalpad	qfn32_thermalpad3.1x3.1mm	Centered exposed thermal pad (default or WxH)

dip

Dual in-line package.

export default () => (
  <board>
    <chip footprint="dip" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="dip16_p1.27_id0.6mm_od0.9mm" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="dip8_wide" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
p	"2.54mm"	Pitch. Space between pins
id	"1mm"	Inner diameter (hole diameter) of plated holes
od	"1.5mm"	Outer diameter (copper diameter) of plated holes
w	"300mil"	Distance between columns
wide	false	Wide DIP style (600mil between columns)
narrow	true	Narrow DIP style (300mil between columns)

axial

Basic through-hole “axial” resistor or diode footprint.

Examples:

• axial
• axial_p0.1in

export default () => (
  <chip
    name="U1"
    footprint="axial"
  />
)

axial parameters:

Parameter	Default	Description
p	"2.54mm"	Pitch. Space between pins
id	"0.7mm"	Inner diameter (hole diameter) of plated holes
od	"1mm"	Outer diameter (copper diameter) of plated holes

01005

Ultra-miniature imperial 01005 (metric 0402) two-pad SMD package. 0.4mm × 0.2mm

export default () => (
  <chip
    name="U1"
    footprint="01005"
  />
)

0201

Sub-miniature imperial 0201 (metric 0603) two-pad SMD package. 0.6mm × 0.3mm

export default () => (
  <chip
    name="U1"
    footprint="0201"
  />
)

0402

Standard imperial 0402 package. 1.0mm × 0.5mm

export default () => (
  <chip
    name="U1"
    footprint="0402"
  />
)

0603

Standard imperial 0603 package. 1.6mm × 0.8mm

export default () => (
  <chip
    name="U1"
    footprint="0603"
  />
)

0805

Standard imperial 0805 package. 2.0mm × 1.2mm

export default () => (
  <chip
    name="U1"
    footprint="0805"
  />
)

1206

Standard imperial 1206 package. 3.2mm × 1.6mm

export default () => (
  <chip
    name="U1"
    footprint="1206"
  />
)

1210

Standard imperial 1210 package. 3.2mm × 2.5mm

export default () => (
  <chip
    name="U1"
    footprint="1210"
  />
)

soic

Small Outline Integrated Circuit (SOIC) footprint.

export default () => (
  <board>
    <chip footprint="soic" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="soic16_w7mm_p0.8mm" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	8	Number of pins in the package.
w	"5.3mm"	Overall package width.
p	"1.27mm"	Pin pitch (center-to-center distance between adjacent pins).
pl	"1.0mm"	Pin length.
pw	"0.6mm"	Pin width.
legsoutside	false	If true, positions pins outside the package body; otherwise, pins are inset.

---

bga

Ball Grid Array (BGA) footprint.

export default () => (
  <board>
    <chip footprint="bga9" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="bga16_p2mm" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="bga14_p1.5mm_missing(1,2)" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	64	Total number of solder balls.
grid	calculated	Grid dimensions as an object (e.g. { x: N, y: N }). If unspecified, a square grid is assumed.
p	"0.8mm"	Ball pitch: center-to-center distance between adjacent balls.
w	none	Package width (optional).
h	none	Package height (optional).
ball	none	Ball diameter (optional).
pad	none	Pad size for each ball (optional).
tlorigin	false	Use top-left numbering for balls.
blorigin	false	Use bottom-left numbering for balls.
trorigin	false	Use top-right numbering for balls.
brorigin	false	Use bottom-right numbering for balls.
missing	[]	List of balls to omit (by number or position) to accommodate design needs.

tssop

Thin-Shrink Small Outline Package (TSSOP) footprint. Default configuration is 6.1mm width with 0.65mm pitch.

export default () => (
  <board>
    <chip footprint="tssop20" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="tssop20_w6.5mm_p0.65mm" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	8	Number of pins in the package
w	"6.1mm"	Overall package width
p	"0.65mm"	Pin pitch (center-to-center distance between adjacent pins)
pw	calculated	Pin width (calculated from pitch if not specified)
pl	calculated	Pin length (calculated from pin width if not specified)

msop

Mini Small Outline Package (MSOP) footprint for compact dual-row surface-mount ICs.

export default () => (
  <board>
    <chip footprint="msop8" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="msop10" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	8	Number of pins in the package (commonly 8 or 10)
w	"3.0mm"	Overall package body width
p	"0.65mm"	Pin pitch (0.65mm for MSOP-8, 0.5mm for MSOP-10)
pw	calculated	Pad width
pl	calculated	Pad length

dfn

Dual Flat No-Lead (DFN) surface-mount package with flush side pads.

export default () => (
  <board>
    <chip footprint="dfn8" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="dfn8_w3mm_p0.5mm" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	8	Number of pins (even number split across left and right sides)
w	"3.0mm"	Package body width
p	"0.5mm"	Pin pitch
pw	"0.3mm"	Pad width
pl	"0.8mm"	Pad length

tqfp

Thin Quad Flat Package (TQFP) footprint with intelligent defaults based on pin count. Commonly used for microcontrollers and FPGAs.

export default () => (
  <board>
    <chip footprint="tqfp32" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="tqfp44" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="tqfp64" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	32	Total number of pins (must be divisible by 4). Common values: 32, 44, 48, 64, 80, 100, 144
p	varies	Pin pitch. Defaults: 0.8mm for 32-pin, 0.5mm for 44+ pins
pl	varies	Pin length. Defaults based on pin count: 1.475mm for 32-100 pins, 1.6mm for 144 pins
pw	varies	Pin width. Defaults based on pin count: 0.55mm (32-pin), 0.3mm (44-100 pins), 0.25mm (144-pin)
w	inherited	Package width (inherited from quad base)
h	inherited	Package height (inherited from quad base)

stampboard

A breakout board with configurable pins on all sides. Can include inner holes for mounting.

export default () => (
  <board>
    <chip footprint="stampboard_left10_right10_bottom4_top0_w21mm_p2.54mm" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="stampboard_left20_right20_bottom3_top2_w21mm_p2.54mm_innerhole" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
w	"22.58mm"	Board width
h	calculated	Board height (calculated from number of pins if not specified)
left	20	Number of pins on left side
right	20	Number of pins on right side
top	2	Number of pins on top side
bottom	2	Number of pins on bottom side
p	"2.54mm"	Pin pitch
pw	"1.6mm"	Pin width
pl	"2.4mm"	Pin length
innerhole	false	Whether to include inner mounting holes
innerholeedgedistance	"1.61mm"	Distance of inner holes from edge

stampreceiver

Similar to stampboard but with modified pad dimensions for receiving a stampboard component.

export default () => (
  <board>
    <chip footprint="stampreceiver_left20_right20_bottom3_top2_w21mm_p2.54mm" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="stampreceiver_left20_right20_bottom3_top2_w21mm_p2.54mm_innerhole" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
w	"22.58mm"	Board width
h	calculated	Board height (calculated from number of pins if not specified)
left	20	Number of pins on left side
right	20	Number of pins on right side
top	2	Number of pins on top side
bottom	2	Number of pins on bottom side
p	"2.54mm"	Pin pitch
pw	"1.6mm"	Pin width
pl	"3.2mm"	Pin length
innerhole	false	Whether to include inner mounting holes
innerholeedgedistance	"1.61mm"	Distance of inner holes from edge

hc49

Standard HC49 crystal footprint.

export default () => (
  <chip
    name="U1"
    footprint="hc49"
  />
)

Parameters:

Parameter	Default	Description
p	"4.88mm"	Pin pitch
id	"0.6mm"	Inner diameter of plated holes
od	"1.2mm"	Outer diameter of plated holes
w	"5.6mm"	Package width
h	"3.5mm"	Package height

to92

TO-92 transistor package footprint, available in triangular or inline arrangements.

export default () => (
  <board>
    <chip footprint="to92" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="to92_inline" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
p	"1.27mm"	Pin pitch
id	"0.72mm"	Inner diameter of plated holes
od	"0.95mm"	Outer diameter of plated holes
w	"4.5mm"	Package width
h	"4.5mm"	Package height
arrangement	"triangular"	Pin arrangement, either "triangular" or "inline"

to220

TO-220 package footprint with configurable number of pins.

export default () => (
  <board>
    <chip footprint="to220_2" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="to220_3" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="to220_4" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	3	Number of pins (specify using format "to220_N")
p	"5.0mm"	Pin pitch
id	"1.0mm"	Inner diameter of plated holes
od	"1.9mm"	Outer diameter of plated holes
w	"13mm"	Package width
h	"7mm"	Package height

ssop

Shrink Small Outline Package (SSOP) footprint.

export default () => (
  <board>
    <chip footprint="ssop8" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="ssop16" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	8	Number of pins in the package
w	"3.9mm"	Overall package width
p	"1.27mm"	Pin pitch (center-to-center distance between adjacent pins)
pw	calculated	Pin width (calculated from pitch if not specified)
pl	calculated	Pin length (calculated from pin width if not specified)

sop8

8-pin Small Outline Package (SOP) footprint.

export default () => (
  <chip
    name="U1"
    footprint="sop8"
  />
)

Parameters:

Parameter	Default	Description
num_pins	8	Fixed at 8 pins
w	inherited	Overall package width
p	inherited	Pin pitch
pl	"1.5mm"	Pin length
pw	"0.6mm"	Pin width

qfp

Quad Flat Package (QFP) footprint with configurable number of pins. Add thermalpad for a centered exposed pad, or pass dimensions such as thermalpad3x3mm to size it.

export default () => (
  <board>
    <chip footprint="qfp32" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="qfp32_thermalpad" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="qfp32_thermalpad3x3mm" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	32	Total number of pins (must be divisible by 4)
w	calculated	Package body width
h	same as w	Package body height
p	"0.8mm"	Pin pitch (center-to-center distance between adjacent pins)
pw	"0.25mm"	Pin width
pl	"0.6mm"	Pin length (exposed pad length)
thermalpad	none	Center exposed thermal pad. Use thermalpad for the default size or thermalpad3x3mm for a custom width and height.

qfn

Quad Flat No-Lead (QFN) package footprint with configurable number of pins. Add thermalpad for a centered exposed pad, or pass dimensions such as thermalpad3.1x3.1mm to size it.

export default () => (
  <board>
    <chip footprint="qfn20" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="qfn32_thermalpad" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="qfn32_thermalpad3.1x3.1mm" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	20	Total number of pins (must be divisible by 4)
w	calculated	Package body width
h	same as w	Package body height
p	"0.5mm"	Pin pitch (center-to-center distance between adjacent pins)
pw	"0.25mm"	Pin width
pl	"0.875mm"	Pin length (exposed pad length)
thermalpad	none	Center exposed thermal pad. Use thermalpad for the default size or thermalpad3.1x3.1mm for a custom width and height.

sot23

Small Outline Transistor (SOT-23) footprint with 3 pins.

export default () => (
  <chip
    name="U1"
    footprint="sot23"
  />
)

Parameters:

Parameter	Default	Description
num_pins	3	Fixed at 3 pins
body_size	"2.9mm"	Size of the package body
p	"0.95mm"	Pin pitch
pw	"0.4mm"	Pin width
pl	"0.6mm"	Pin length

sot23_5

Small Outline Transistor (SOT-23-5) footprint with 5 pins.

export default () => (
  <chip
    name="U1"
    footprint="sot23_5"
  />
)

Parameters:

Parameter	Default	Description
num_pins	5	Fixed at 5 pins
body_size	"2.9mm"	Size of the package body
p	"0.95mm"	Pin pitch
pw	"0.4mm"	Pin width
pl	"0.6mm"	Pin length

sot223

Small Outline Transistor (SOT-223) footprint with 4 pins.

export default () => (
  <chip
    name="U1"
    footprint="sot223"
  />
)

Parameters:

Parameter	Default	Description
num_pins	4	Fixed at 4 pins
body_size	"6.5mm"	Size of the package body
p	"2.3mm"	Pin pitch
pw	"0.7mm"	Pin width
pl	"0.8mm"	Pin length

sot363

6-pin Small Outline Transistor (SOT-363 / SC-88) footprint.

export default () => (
  <chip
    name="U1"
    footprint="sot363"
  />
)

Parameters:

Parameter	Default	Description
num_pins	6	Fixed at 6 pins
w	"2.1mm"	Overall width across pads
p	"0.65mm"	Pin pitch
pw	"0.3mm"	Pad width
pl	"0.7mm"	Pad length

sot563

Ultra-compact 6-pin Small Outline Transistor (SOT-563) footprint.

export default () => (
  <chip
    name="U1"
    footprint="sot563"
  />
)

Parameters:

Parameter	Default	Description
num_pins	6	Fixed at 6 pins
w	"1.6mm"	Package width
p	"0.5mm"	Pin pitch
pw	"0.3mm"	Pad width
pl	"0.55mm"	Pad length

sot723

Ultra-small 3-pin Small Outline Transistor (SOT-723) footprint.

export default () => (
  <chip
    name="U1"
    footprint="sot723"
  />
)

Parameters:

Parameter	Default	Description
num_pins	3	Fixed at 3 pins
w	"1.2mm"	Package body width
h	"1.2mm"	Package body height
pl	"0.4mm"	Pad length
pw	"0.32mm"	Pad width

sot89

Medium-power Small Outline Transistor (SOT-89) footprint with 3 or 5 pins.

export default () => (
  <board>
    <chip footprint="sot89" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="sot89_5" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
num_pins	3	Number of pins (3 or 5)
w	"4.5mm"	Package body width
p	"1.5mm"	Pin pitch

sod123 & sod323

Small Outline Diode (SOD-123 and SOD-323) two-pad SMD diode footprints.

export default () => (
  <board>
    <chip footprint="sod123" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="sod323" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default (sod123 / sod323)	Description
w	"3.65mm" / "2.5mm"	Overall width across pads
h	"1.6mm" / "1.25mm"	Package body height
pw	"1.22mm" / "0.6mm"	Pad width
pl	"0.91mm" / "0.6mm"	Pad length

sma, smb, & smc

DO-214 surface-mount power diode packages (sma / DO-214AC, smb / DO-214AA, and smc / DO-214AB).

export default () => (
  <board>
    <chip footprint="sma" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="smb" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="smc" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters:

Package	Default Pitch (p)	Default Pad Width (pw)	Default Pad Length (pl)
sma	"4.0mm"	"1.5mm"	"1.7mm"
smb	"4.3mm"	"2.2mm"	"2.5mm"
smc	"6.85mm"	"3.2mm"	"2.2mm"

pushbutton

4-pin tactile pushbutton switch footprint with configurable width, height, and internally shorted pin pairs.

export default () => (
  <board>
    <chip footprint="pushbutton" name="U1" pcbX={-7.5} pcbY={0} />  
    <chip footprint="pushbutton_id1.2mm_od2mm" name="U2" pcbX={7.5} pcbY={0} />
  </board>
)

Parameters:

Parameter	Default	Description
w	"6.5mm"	Horizontal spacing between switch pins
h	"4.5mm"	Vertical spacing between switch pins
id	"1.0mm"	Inner drill diameter of plated holes
od	"1.8mm"	Outer copper diameter of plated holes
tllabel / trlabel / bllabel / brlabel	optional	Silkscreen labels for top-left, top-right, bottom-left, and bottom-right pins

pinrow

Row of pins suitable for male or female pin headers. If _male or _female is specified the 3d model will update accordingly.

export default () => (
  <chip
    name="U1"
    footprint="pinrow4"
  />
)

Parameters:

Parameter	Default	Description
num_pins	6	Number of pins
p	"0.1in"	Pin pitch
id	"1.0mm"	Inner diameter
od	"1.5mm"	Outer diameter
rows	1	Number of rows (single- or double-row headers)
male	true	Male header
female	false	Female header
smd	false	Surface mount device
rightangle	false	Right angle configuration
pw	"1.0mm"	Pad width for SMD
pl	"2.0mm"	Pad length for SMD
pinlabeltextalignleft	false	Align pin labels to the left
pinlabeltextaligncenter	false	Align pin labels to the center
pinlabeltextalignright	false	Align pin labels to the right
pinlabelverticallyinverted	false	Vertically invert pin labels
pinlabelorthogonal	false	Make pin labels orthogonal
nosquareplating	false	Do not use rectangular pad for pin 1
nopinlabels	false	Omit silkscreen pin labels
doublesidedpinlabel	false	Add silkscreen pins in top and bottom layers
bottomsidepinlabel	false	Place silkscreen reference text on bottom layer

melf, micromelf, & minimelf

MELF (Metal Electrode Leadless Face) cylindrical surface-mount packages (melf, micromelf, and minimelf).

export default () => (
  <board>
    <chip footprint="melf" name="U1" pcbX={-15} pcbY={0} />  
    <chip footprint="micromelf" name="U2" pcbX={0} pcbY={0} />  
    <chip footprint="minimelf" name="U3" pcbX={15} pcbY={0} />
  </board>
)

Parameters (micromelf / minimelf):

Parameter	micromelf Default	minimelf Default	Description
num_pins	2	2	Number of pins (fixed at 2)
w	"3.0mm"	"5.40mm"	Package width
h	"1.80mm"	"2.30mm"	Package height
pl	"0.80mm"	"1.30mm"	Pad length
pw	"1.20mm"	"1.70mm"	Pad width
p	"1.6mm"	"3.5mm"	Pin pitch