正向和反向批注

从原理图更新 PCB（正向批注）

使用 "从原理图更新 PCB" 工具将设计信息从原理图编辑器同步到电路板编辑器。在原理图编辑器和电路板编辑器中都可以用 工具 → 从原理图更新 PCB（F8）来访问该工具。你也可以使用电路板编辑器顶部工具栏上的 从原理图更新 PCB图标。这个过程通常被称为正向批注。

从原理图更新 PCB 是将设计信息从原理图转移到 PCB 的首选方法。在旧版本的 KiCad 中，相应的过程是将网表从原理图编辑器中导出并导入到电路板编辑器中。现在已经没有必要使用网表文件了。
从原理图更新 PCB

该工具将每个符号的封装添加到电路板上，并将更新的原理图信息传输到电路板上。同时，电路板的网络连接会被更新以匹配原理图。带有排除在电路板属性之外 的符号不会被更新到 PCB 上。

将对 PCB 进行的修改列在 待应用修改 窗格中。点击 更新 PCB 按钮之前，PCB 不会被修改。

你可以使用窗口底部的复选框来显示或隐藏不同类型的信息。可以使用 保存…​ 按钮将更改的报告保存到文件中。

选项

该工具有几个选项可以控制其行为。

Option 描述

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, but will be lost when the symbol is deleted, even if a symbol with the same reference designator replaces it.

If checked, each footprint in the PCB will be re-linked such that each footprint has its unique identifier updated to match the symbol that has the same reference designator as the footprint.

This option should generally be left unchecked. See below for more details on when to use this option.

Replace footprints with those specified by symbols

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.

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.

Override locks

If checked, locking a footprint will not affect whether a footprint is deleted or replaced based on changes in the schematic.

If unchecked, locked footprints will never be deleted or replaced even if they otherwise would be.

Update footprint fields from symbols

If checked, new and updated fields in symbols will be transferred to the corresponding footprints, keeping symbol and footprint fields in sync.

If unchecked, footprint fields will not be updated when fields change in the corresponding symbols.

Remove footprint fields not found in symbols

If checked, footprint fields will be removed if they do not exist in the corresponding symbol.

If unchecked, footprint fields that do not exist in the corresponding symbol will not be removed, allowing footprints to have additional fields compared to the corresponding symbols.

Re-linking symbols and footprints

Symbols and footprints are linked together using unique identifiers (also called UUIDs). These are handled automatically within KiCad and are not usually visible to users. They allow a symbol and its partner footprint to keep their connection between schematic and PCB, even if the reference designator is changed. New objects get assigned their identifiers upon creation.

Re-linking by unique identifier (default)

In normal use, the Re-link footprints to schematic symbols based on their reference designators option should be unchecked. In this mode, symbols with the same identifier as a footprint will update that footprint, regardless of the reference designator. Symbols which have an identifier that doesn’t match any footprint will add a new footprint linked to that identifier.

For example, in the below schematic, both R1 and R2 are linked via their unique IDs to footprints on the PCB:

Forward annotation linking by unique identifier, before a change in reference designator

If symbol reference designators are changed in the schematic (e.g. by re-annotation), running the Update PCB from Schematic process will update the reference designators on the PCB.

Forward annotation linking by unique identifier, after a change in reference designator
Re-linking by reference designator

If the checkbox is checked, the linking process is done using the reference designators. This can be useful for workflows that result in a symbol being deleted and replaced by another one, rather than being updated in-place. For example, cut-and-pasting a block of schematic or a sheet and copy-pasting and re-annotating will usually break the identifier-based links.

For example in the below case, the resistors R1 and R2 have been deleted and replaced, then re-annotated. While the reference designators are the same, the internal identifiers have changed. Updating the PCB by identifier would cause the existing footprints to be deleted and new ones added - to KiCad, the existing footprints have no matching symbol. This would cause the footprints to lose their positions and need placing again.

Forward annotation linking by reference designator, after deleting and replacing symbols, but before updating the PCB

Re-linking the footprints by reference designator causes KiCad to re-create the links, using the matching reference designators as a guide.

Forward annotation linking by reference designator, after updating the PCB

Because the links have been re-established, the next forward annotation should use the normal identifier-based linking (i.e. the checkbox should be unchecked).

从 PCB 上更新原理图（反向批注）

KiCad 的典型工作流程是在原理图中进行修改，然后使用 "从原理图更新 PCB" 工具将修改内容同步到电路板上。然而，相反的过程也是可行的：可以在电路板上进行设计修改，然后在原理图或电路板编辑器中使用 工具 → 从 PCB 更新原理图 同步回原理图。这个过程也被称为 "反向批注"。

从 PCB 上更新原理图

The tool syncs changes in reference designators, values, attributes (like DNP or Exclude From BOM), footprint assignments, other fields, and net names from the board to the schematic. Each type of change can be individually enabled or disabled.

将对原理图进行的修改列在 待应用的修改 窗格中。在您点击 更新原理图 按钮之前，原理图不会被修改。

你可以使用窗口底部的复选框来显示或隐藏不同类型的信息。可以使用 保存…​ 按钮将更改的报告保存到文件中。

选项

该工具有几个选项可以控制其行为。

Option

描述

Re-link footprints to schematic symbols based on their reference designators

If checked, each footprint in the PCB will be re-linked to the symbol that has the same reference designator as the footprint. This option is incompatible with updating symbol reference designators.

If unchecked, footprints and symbols will be linked by unique identifier as usual, rather than by reference designator.

Reference designators

If checked, symbol reference designators will be updated to match the reference designators of the linked footprints.

If unchecked, symbol reference designators will not be updated.

Values

If checked, symbol values will be updated to match the values of the linked footprints.

Values

If checked, symbol attributes (like exclude from BOM and DNP) will be updated to match the corresponding attributes of the linked footprints.

If unchecked, symbol values will not be updated.

Footprint assignments

If checked, footprint assignments will be updated for symbols which have had their footprints changed or replaced in the board.

If unchecked, symbol footprint assignments will not be updated.

Net names

If checked, the schematic will be updated with any net name changes that have been made in the board. Net labels will be updated or added to the schematic as necessary to match the board.

Other fields

If checked, other symbol fields will be updated to match the corresponding fields of the linked footprints. Reference designator, value, and footprint are each controlled by their own separate option.

If unchecked, net names will not be updated in the schematic.
The 按位置重新批注 该功能可以与反向批注位号结合使用 根据设计中的元件的位置重新批注所有元件。

用 CMP 文件进行反向批注

通过从 PCB 编辑器中导出 CMP 文件（文件 → 导出 → 封装关联（.cmp）文件…​）并在原理图编辑器中导入（文件 → 导入 → 封装分配…​），也可以将变化从 PCB 同步到原理图。

这种方法只能同步对封装分配和封装字段的修改。建议使用 "从 PCB 更新原理图" 工具来代替。