Schematic

Placing Components

2 min read Updated Markdown
On this page

Place schematic symbols from approved local libraries and assign the exact value and PCB footprint required by the selected physical part.

Prepare the library#

  1. Open View → Local Library Manager.
  2. Add the KiCad symbol file or containing library folder.
  3. Confirm the source and symbol in the active inventory.
  4. Activate the target schematic and search its Component Library.

If the exact part is missing, import an approved library, create it in Symbol Library Editor, or use the Fix or Create a Component with full datasheet review.

Place a symbol#

  1. In the Library panel (Local Library tab), type the part family or symbol name in Filter.... Tick Hide Power/Logo to hide power symbols and logos from the list.
  2. Click a symbol to preview it in Properties (Symbol, Footprint, and 3D Model tabs) before placing it. A warning icon means No footprint linked.
  3. Drag the symbol from the list onto a clear spot of the sheet and release.
  4. Rotate with Space (or R while it is selected).
  5. Press Esc to return to selection.
Filter the project library for 24LC, drag a third 24LC1025 EEPROM onto the sheet, press Esc — it becomes U5

On the KLP4e datalogger the Library panel lists the symbols that came with the project — the 16 symbols imported from its KiCad project into the project's own library. A placed part takes the next free designator: after U1–U4 the new EEPROM becomes U5. Its pins are unconnected until you wire them, and ERC reports each one.

Complete component properties#

Select the component and verify:

Properties → Component Properties has three tabs:

Tab Fields
General Info: Designator, Value, Comment, Exclude from PCB. Location: Position, Rotation. Linked Footprint with Link Footprint & Save to File
3D Model Preview of the linked footprint's 3D model
Pins Each pin's No, Name, position, and Show Num / Show Name

Review each one:

Field Review
Designator Unique and appropriate prefix
Value Electrical value or exact orderable part number
Footprint Exact package variant and pad count
Comment Useful design or sourcing note, when required
Exclude from PCB Only for parts that are not on this board (test points on a fixture, off-board items)

The eye button beside a field shows or hides that text on the sheet.

Changing a designator can affect connected references. Review the updated item and run ERC before PCB update.

Move, rotate, copy, or delete#

Drag to move (or nudge with the arrow keys), Space to rotate, Ctrl+C / Ctrl+V to duplicate, and Del to remove — the wires attached to a deleted component are removed with it. Right-click a component for Move ▸ (10 px steps), Rotate (90), Reload from Library, and Sync Attributes to Similar Components. After moving or rotating a connected component, inspect each wire endpoint at the pin tip.

Pasted components receive new identities to avoid duplicates, but you must still review their values, footprint assignments, and connections.

Pre-ERC checklist#

  • Exact device and package variant are known.
  • Designator is unique.
  • Value and rating are correct.
  • Footprint pad numbering matches symbol pins.
  • Polarity and orientation are clear.
  • Every used pin is connected intentionally; unused pins are handled explicitly.