exportJson

JSON export for Allegro PCB designs

Skill script for Allegro PCB Designer to generate a JSON file representing the design.

The generated json file complies to the schema, that is needed to generate the InteractiveHtmlBom.

A demo is worth a thousand words.

Prerequisites

To make the skill script available for use, you need to copy the exportJson.il file to your local skill directory ( usually your installation path + \share\pcb\etc ) or the skill directory in the $CDS_SITE path. Append it to the allegro.ilinit file ( add load( "path/exportJson.il" ) ) or load it manually via the skill load command ( type set telskill into the command line and then type load("exportJson.il" ).

Usage

Once the script is loaded successfully, you can start exporting the json file by typing exportJson + enter in the command line. A directory named json is created in your project folder containing the .json.

The script uses the “project name” ( optional: + “_” + “variant” ) as the file name and asks for the optional arguments revision and company. By passing ?rev "xyz" and ?company "name" as arguments to the exportJson function, the input prompt is suppressed and these values are used for file generation. This is can be useful to customize the function to your needs.

The output can be configured by passing the optional arguments directly (as listed below) or by using a JSON file that contains the output configuration. The JSON file can be used passing ?config "filePath" to the exportJson function.

If a JSON file is used, but the linewidths are not to be changed, the value "design" must be used instead of a number ( e.g. 0.1).

Optional arguments

argument	description	type
?exportInnerLayers	default: nil, exports the inner layers	bool
?renderViaHoles	default: nil, render via holes	bool
?textAsSvgPaths	default: t, uses font-data otherwise	bool
?excludeDNP	default: nil, all fabrication and silkscreen data of an unplaced component are ignored	bool
?pcbLinewidth	override value	float
?fabricationLayerLinewidth	override value	float
?silkscreenLayerLinewidth	override value	float
?margin	extra spacing for displaying	list / float
?rev	revision	string
?company	company name	string

Linewidths

Without appending any additional arguments to the exportJson function, the linewidth of every segment is assigned to its original value. However, in some cases you may want to use a different and consistent linewidth as used in the pcb design. In this case three optional arguments can be passed to override the linewidth of pcb outline (?pcbLinewidth), the fabrication layer (?fabricationLayerLinewidth) and the silkscreen layer (silkscreenLayerLinewidth). For example:

    exportJson( ?pcbLinewidth 0.1 ?fabricationLayerLinewidth 0.2 ?silkscreenLayerLinewidth 0.2 )

uses a 0.1 unit linewidth for the pcb outline and a linewidth of 0.2 unit for the fabrication and the silkscreen layer.

Margin

Because the extents are defined by the pcb’s minimum and maximum x/y values you may want to add some extra spacing. The function call below, adds a spacing of 20.0 unit to all four directions ( list( '( spacingLeft spacingBottom ) '( spacingRight spacingTop ) ) ).

    exportJson( ?margin list( '( 20.0 20.0 ) '( 20.0 20.0 ) ) )

Texts

Texts are represented as svgpaths by default. If you want to use custom font_data or the newstroke font you can pass the optional argument ?textsAsSvgPaths nil to the export function( exportJson( ?textsAsSvgPaths nil ) ) and the texts are described as defined in DATAFORMAT.md.

Variants and alternate parts

If no variants.lst is present in the allegro directory, a warning is displayed in the command prompt and all components are considered in the json file; otherwise a json file for each variant is created and the DNP field in the extra_fields is set to mark unplaced components. When an alternate part are used, the value of the part is changed to the value of the alternate part.

By passing the optional argument ?excludeDNP t to the export function ( exportJson( ?excludeDNP t ) ) all fabrication and silkscreen data of an unplaced component are ignored.

Parts with no reference designator assigned are not included in the interactive BOM.

Custom properties

Any custom properties assigned to a component are added to the extra_fields.

Default Layer Mapping

If no JSON file for output configuration is used, only the following layers are considered for file creation:

ibom	allegro
edges	BOARD GEOMETRY/DESIGN_OUTLINE BOARD GEOMETRY/CUTOUT
fabrication	PACKAGE GEOMETRY/ASSEMBLY_TOP PACKAGE GEOMETRY/ASSEMBLY_BOTTOM REF DES/ASSEMBLY_TOP REF DES/ASSEMBLY_BOTTOM COMPONENT_VALUE/ASSEMBLY_TOP COMPONENT_VALUE/ASSEMBLY_BOTTOM
silkscreen	PACKAGE GEOMETRY/SILKSCREEN_TOP PACKAGE GEOMETRY/SILKSCREEN_BOTTOM REF DES/SILKSCREEN_TOP REF DES/SILKSCREEN_BOTTOM COMPONENT_VALUE/SILKSCREEN_TOP COMPONENT_VALUE/SILKSCREEN_BOTTOM

Call interactive HTML BOM from allegro

If you want to export the json file and convert it to the ibom in one step, you can use the code snippet below to write your own script. For ibomArgs see command line options.

ibomSourcePath = ...

when( ibomSourcePath
    ibomPythonFile = strcat( ibomSourcePath "generate_interactive_bom.py" )		
)

ibomArgs = "--name %f --dnp-field DNP --show-fabrication --hide-silkscreen --dest-dir ../ibom --layer-view F --dark-mode --no-browser"

workingDir = getWorkingDir()

; list create files in json directory
files = getDirFiles( "json" ) 

foreach( file files 
    subStrings = parseString( file "." )

    ; if file is json file
    when( car( last( subStrings ) ) == "json" 
        fullFilePath = strcat( "\"" buildString( list( workingDir "json" file ) "/" ) "\"" )
        command = buildString( list( "python" ibomPythonFile fullFilePath ibomArgs ) )
        result = shell( command )	

        unless( result				
            axlUIConfirm( "Error during ibom generation ..." 'error )
        )
    )						
)				
axlUIConfirm( "Process finished!" 'info )

Example

As an example I have done the json export and the ibom creation for the AD-FMCOMMS3-EBZ design, which .brd file is freely accessible.