Relative Positioning

calc(...) expressions let you create layouts that stay correct even when part sizes or board dimensions change.

This guide focuses on PCB positioning with:

component bounds (R1.x, R1.maxX, R1.minY, etc.)
pin/pad bounds (U1.pin1.x, R1.pin2.maxX, etc.)
board bounds (board.minX, board.maxX, board.minY, board.maxY)
edge anchor props (pcbLeftEdgeX, pcbRightEdgeX, pcbTopEdgeY, pcbBottomEdgeY)

Position one component relative to another

A common pattern is: "place this part a fixed distance from another part's edge."

export default () => (
<board width="24mm" height="12mm">
  <resistor name="R1" footprint="0805" resistance="1k" pcbX="-5mm" pcbY="0mm" />
  <resistor
    name="R2"
    footprint="0805"
    resistance="1k"
    pcbX="calc(R1.maxX + 2mm)"
    pcbY="calc(R1.y)"
  />
</board>
)

Here R2 tracks R1: if R1 changes footprint or moves, R2 keeps a 2mm gap from R1's right edge.

Build a spacing chain

You can chain references to build predictable spacing across many components.

export default () => (
<board width="36mm" height="12mm">
  <resistor name="R1" footprint="0603" resistance="1k" pcbX="-11mm" pcbY="0mm" />
  <resistor
    name="R2"
    footprint="0603"
    resistance="1k"
    pcbX="calc(R1.maxX + 1.5mm)"
    pcbY="calc(R1.y)"
  />
  <resistor
    name="R3"
    footprint="0603"
    resistance="1k"
    pcbX="calc(R2.maxX + 1.5mm)"
    pcbY="calc(R2.y)"
  />
  <resistor
    name="R4"
    footprint="0603"
    resistance="1k"
    pcbX="calc(R3.maxX + 1.5mm)"
    pcbY="calc(R3.y)"
  />
</board>
)

This is useful for resistor ladders, LED banks, or connector rows where you want stable clearances.

Position from a specific pin/pad

You can anchor from a pin instead of from a component center/edge.

export default () => (
<board width="32mm" height="16mm">
  <resistor name="R1" footprint="0805" resistance="1k" pcbX="0mm" pcbY="0mm" />
  <resistor
    name="R2"
    footprint="0805"
    resistance="1k"
    pcbX="calc(R1.pin1.minX - 2mm)"
    pcbY="calc(R1.pin1.y)"
  />
  <resistor
    name="R3"
    footprint="0805"
    resistance="1k"
    pcbX="calc(R1.pin2.maxX + 2mm)"
    pcbY="calc(R1.pin2.y)"
  />
</board>
)

Pin-relative placement is great when the physical relation to a specific pad is what matters.

Anchor directly to board edges

Edge anchor properties are ideal for fixed margins from the PCB outline.

export default () => (
<board width="40mm" height="24mm">
  <resistor
    name="R_LEFT"
    footprint="0603"
    resistance="1k"
    pcbLeftEdgeX="calc(board.minX + 2mm)"
    pcbY="0mm"
  />
  <resistor
    name="R_RIGHT"
    footprint="0603"
    resistance="1k"
    pcbRightEdgeX="calc(board.maxX - 2mm)"
    pcbY="0mm"
  />
  <resistor
    name="R_TOP"
    footprint="0603"
    resistance="1k"
    pcbTopEdgeY="calc(board.maxY - 2mm)"
    pcbX="0mm"
  />
  <resistor
    name="R_BOTTOM"
    footprint="0603"
    resistance="1k"
    pcbBottomEdgeY="calc(board.minY + 2mm)"
    pcbX="0mm"
  />
</board>
)

These are especially useful for connectors, mounting holes, fiducials, and test points that need consistent edge offset.

Mix edge anchors and relative spacing

You can combine both styles: lock one component to the edge, then place others relative to it.

export default () => (
<board width="46mm" height="18mm">
  <resistor
    name="R1"
    footprint="0603"
    resistance="1k"
    pcbLeftEdgeX="calc(board.minX + 2mm)"
    pcbY="0mm"
  />
  <resistor
    name="R2"
    footprint="0603"
    resistance="1k"
    pcbX="calc(R1.maxX + 2mm)"
    pcbY="calc(R1.y)"
  />
  <resistor
    name="R3"
    footprint="0603"
    resistance="1k"
    pcbX="calc(R2.maxX + 2mm)"
    pcbY="calc(R2.y)"
  />
</board>
)