:experimental:

[[schematic-to-pcb]]
== Transferring designs between schematic and PCB

=== Update PCB from Schematic
Use the Update PCB from Schematic tool to sync design information from the
Schematic Editor to the Board Editor. The tool can be accessed with **Tools** ->
**Update PCB from Schematic** (kbd:[F8]) in both the schematic and board
editors. You can also use the
image:images/icons/update_pcb_from_sch_24.png[Update PCB from Schematic icon] icon in the
top toolbar of the Board Editor.

NOTE: Update PCB from Schematic is the preferred way to transfer design
information from the schematic to the PCB. In older versions of KiCad, the
equivalent process was to export a netlist from the Schematic Editor and import
it into the Board Editor. It is no longer necessary to use a netlist file.

image::images/update_pcb_from_schematic.png[alt="Update PCB from schematic",scaledwidth="70%"]

The tool adds the footprint for each symbol to the board and transfers updated
schematic information to the board. In particular, the board's net connections
are updated to match the schematic.

The changes that will be made to the PCB are listed in the _Changes To Be
Applied_ pane. The PCB is not modified until you click the **Update PCB**
button.

You can show or hide different types of messages using the checkboxes at the
bottom of the window. A report of the changes can be saved to a file using the
**Save...** button.

==== Options

The tool has several options to control its behavior.

[cols="1,2"]
|===
| Option | Description

| Re-link footprints to schematic symbols based on their reference designators
| Footprints are normally linked to schematic symbols via a unique identifier
created when the symbol is added to the schematic. A symbol's unique identifier
cannot be changed.

If checked, each footprint in the PCB will be re-linked to the symbol that has
the same reference designator as the footprint.

If unchecked, footprints and symbols will be linked by unique identifier as
usual, rather than by reference designator. Each footprint's reference
designator will be updated to match the reference designator of its linked
symbol.

This option should generally be left unchecked. It is useful for specific
workflows that rely on changing the links between schematic symbols and
footprints, such as refactoring a schematic for easier layout or replicating
layout between identical channels of a design.

| Delete footprints with no symbols
| If checked, any footprint in the PCB without a corresponding symbol in the
schematic will be deleted from the PCB. Footprints with the "Not in schematic"
attribute will be unaffected.

If unchecked, footprints without a corresponding symbol will not be deleted.

| Replace footprints with those specified in the schematic
| If checked, footprints in the PCB will be replaced with the footprint that is
specified in the corresponding schematic symbol.

If unchecked, footprints that are already in the PCB will not be changed, even
if the schematic symbol is updated to specify a different footprint.
|===

=== Update Schematic from PCB

NOTE: TODO: write this section

==== Backannotation with CMP files

Select changes can also be synced from the PCB back to the schematic by
exporting a CMP file from the PCB editor (**File** -> **Export** -> **Footprint
Association (.cmp) File...**) and importing it in the Schematic Editor (**File**
-> **Import** -> **Footprint Assignments...**).

NOTE: This method can only sync changes made to footprint assignments and
footprint fields. It is recommended to use the Update Schematic from PCB tool
instead.