kicad/eeschema/dialogs/dialog_bom_help.md

144 lines
5.5 KiB
Markdown

# 1 - Full documentation
The Eeschema documentation (*eeschema.html*) describes this intermediate netlist and gives examples(chapter ***creating customized netlists and bom files***).
# 2 - The intermediate Netlist File
BOM files (and netlist files) can be created from an *Intermediate netlist file* created by Eeschema.
This file uses XML syntax and is called the intermediate netlist. The intermediate netlist includes a large amount of data about your board and because of this, it can be used with post-processing to create a BOM or other reports.
Depending on the output (BOM or netlist), different subsets of the complete Intermediate Netlist file will be used in the post-processing.
# 3 - Conversion to a new format
By applying a post-processing filter to the Intermediate netlist file you can generate foreign netlist files as well as BOM files. Because this conversion is a text to text transformation, this post-processing filter can be written using *Python*, *XSLT*, or any other tool capable of taking XML as input.
XSLT itself is a XML language suitable for XML transformations. There is a free program called `xsltproc` that you can download and install. The `xsltproc` program can be used to read the Intermediate XML netlist input file, apply a style-sheet to transform the input, and save the results in an output file. Use of `xsltproc` requires a style-sheet file using XSLT conventions. The full conversion process is handled by Eeschema, after it is configured once to run `xsltproc` in a specific way.
A Python script is somewhat more easy to create.
# 4 - Initialization of the dialog window
You should add a new plugin (a script) in the plugin list by clicking on the Add Plugin button.
## 4.1 - Plugin Configuration Parameters
The Eeschema plug-in configuration dialog requires the following information:
* The title: for instance, the name of the netlist format.
* The command line to launch the converter (usually a script).
***Note (Windows only):***
*By default, the command line runs with hidden console window and output is redirected to "Plugin info" field. To show the window of the running command, set the checkbox "Show console window".*
Once you click on the generate button the following will happen:
1. Eeschema creates an intermediate netlist file \*.xml, for instance `test.xml`.
2. Eeschema runs the script from the command line to create the final output file.
## 4.2 - Generate netlist files with the command line
Assuming we are using the program `xsltproc.exe` to apply the sheet style to the intermediate file, `xsltproc.exe` is executed with the following command.
```
xsltproc.exe -o <output filename> <style-sheet filename> <input XML file to convert>
```
On Windows the command line is the following.
```
f:/kicad/bin/xsltproc.exe -o "%O" f:/kicad/bin/plugins/myconverter.xsl "%I"
```
On Linux the command becomes as following.
```
xsltproc -o "%O" /usr/local/kicad/bin/plugins/myconverter .xsl "%I"
```
where `myconverter.xsl` is the style-sheet that you are applying.
Do not forget the double quotes around the file names, this allows them to have spaces after the substitution by Eeschema.
If a Python script is used, the command line is something like (depending on the Python script):
```
python f:/kicad/bin/plugins/bom-in-python/myconverter.py "%I" "%O"
```
or
```
python /usr/local/kicad/bin/plugins/bom-in-python/myconverter .xsl "%I" "%O"
```
The command line format accepts parameters for filenames. The supported formatting parameters are:
* `%B`: base filename of selected output file, minus path and extension.
* `%P`: project directory, without name and without trailing '/'.
* `%I`: complete filename and path of the temporary input file
(the intermediate net file).
* `%O`: complete filename and path (but without extension) of the user
chosen output file.
`%I` will be replaced by the actual intermediate file name (usually the full root sheet filename with extension ".xml").
`%O` will be replaced by the actual output file name (the full root sheet filename minus extension).
`%B` will be replaced by the actual output short file name (the short root sheet filename minus extension).
`%P` will be replaced by the actual current project path.
## 4.3 - Command line format:
### 4.3.1 - Remark:
Most of time, the created file must have an extension, depending on its type.
Therefore you have to add to the option ***%O*** the right file extension.
For instance:
* **%O.csv** to create a .csv file (comma separated value file).
* **%O.htm** to create a .html file.
* **%O.bom** to create a .bom file.
### 4.3.2 Example for xsltproc:
The command line format for xsltproc is the following:
```
<path of xsltproc> xsltproc <xsltproc parameters>
```
On Windows:
```
f:/kicad/bin/xsltproc.exe -o "%O.bom" f:/kicad/bin/plugins/netlist_form_pads-pcb.xsl "%I"
```
On Linux:
```
xsltproc -o "%O.bom" /usr/local/kicad/bin/plugins/netlist_form_pads-pcb.xsl "%I"
```
The above examples assume `xsltproc` is installed on your PC under Windows and xsl files located in `<path_to_kicad>/kicad/bin/plugins/`.
### 4.3.3 Example for Python scripts:
Assuming python is installed on your PC, and python scripts are located in
`<path_to_kicad>/kicad/bin/plugins/bom-in-python/`,
the command line format for python is something like:
```
python <script file name> <input filename> <output filename>
```
On Windows:
```
python.exe f:/kicad/bin/plugins/bom-in-python/my_python_script.py "%I" "%O.html"
```
On Linux:
```
python /usr/local/kicad/bin/plugins/bom-in-python/my_python_script.py "%I" "%O.csv"
```