# Placing Components

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](../ai/component-generator.md) 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.

### Short video — Find and place a symbol

<video controls muted playsinline preload="metadata" src="../assets/wf/docs/schematic/placing-components/find-and-place-a-symbol.mp4" title="Filter the project library for 24LC, drag a third 24LC1025 EEPROM onto the sheet, press Esc — it becomes U5"></video>
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](erc.md) 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 ++delete++ 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.

## Related guidelines

- [Symbol Libraries](../libraries/symbols-library.md)
- [Wiring and Nets](wiring-and-nets.md)
- [Properties and Attributes](properties-and-attributes.md)
- [ERC](erc.md)
