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 
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。 |
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 | 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. |
Delete/replace footprints even if locked |
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. |
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"。
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 |
Description |
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。 |