Import Matrix File

The FAB 3000 Import Matrix File permits external tools (like PCB Design software) to predefine layers and jobs for intelligent loading into FAB 3000 for instant Gerber Viewing & Verification. This prevents the monotonous steps of loading Gerber & Drill files, assigning layer colors, assigning layer types, defining layer stack ups, defining blind/buried drill layers (if required), etc.; allowing pcb designers to easily use Gerber/CAM software for its primary purpose... to quickly verify their gerbers & drills are correct and ready for manufacturing.

The FAB 3000 Import Matrix file also supports PANEL arrays which allow the merging of several PCB jobs together so they can be manufactured simultaneously - saving $$$ on fabrication costs. In addition, FAB 3000 will automatically performs all necessary object transformations, dcode & drill tool transcoding.

Note: Simply call FAB 3000 and pass the matrix file as the first argument.

Note: All FAB 3000 Import Matrix Files must end with *.fm6.

RULE #1: LAYER arrays are Always defined first.

RULE #2: JOB arrays are defined after LAYER arrays

RULE #3: PANEL arrays are defined Last

LAYER {

TYPE=MASK_TOP

NAME=smt

START_DRILL=

END_DRILL=

DRAW_COLOR=223,100,100

FLASH_COLOR=223,100,100

}

LAYER {

TYPE=TOP

NAME=layer_1

START_DRILL=

END_DRILL=

DRAW_COLOR=100,223,0

FLASH_COLOR=100,223,0

}

...

JOB {

NAME=test-odb++-gerber

LAYER=layer_1,C:\temp\examples\274X\Art0121.pho

LAYER=layer_2,C:\temp\examples\274X\Art02.pho

LAYER=layer_4,C:\temp\examples\274X\Pgp2529.pho

LAYER=layer_3,C:\temp\examples\274X\gnd2530.pho

LAYER=sst,C:\temp\examples\274X\Sst0126.pho

LAYER=spt,C:\temp\examples\274X\Sp0128.pho

LAYER=smb,C:\temp\examples\274X\Sm0227.pho

LAYER=smt,C:\temp\examples\274X\Sm0128.pho

LAYER=d_1_2,C:\temp\examples\274X\Drill.drl

}

JOB {

NAME=board1

LAYER=smb,C:\temp\examples\Board1\Bottom Mask.gbr

LAYER=layer_4,C:\temp\examples\Board1\Bottom.gbr

LAYER=smt,C:\temp\examples\Board1\Top Mask.gbr

LAYER=layer_1,C:\temp\examples\Board1\Top.gbr

LAYER=sst,C:\temp\examples\Board1\Top Silk.gbr

LAYER=d_1_2,C:\temp\examples\Board1\drill.drl

}

...

PANEL {

NAME=mypanel

UNITS=INCH

WIDTH=18

HEIGHT=18.5

STEPREPEAT=board1,17.0,4,3.8,3.4,2,5,90,No

STEPREPEAT=test-odb++-gerber,17.85,11.5,7,6,1,3,90,No

}

...

Fields in the LAYER array

TYPE	Describes the purpose of the layer and must be one of these defined Layer Types
NAME	The name of the layer. This will be directly referenced in the JOB array.
START_DRILL END_DRILL	These fields are only used for drill layers. They specify the span of the drill, in case it is a blind or buried via layers. Each field must be a valid layer name. When the fields are empty, the drill is assumed to be thru hole (i.e START_DRILL is assumed to be the first board layer and END_DRILL is assumed to be the last board layer).
DRAW_COLOR	The RGB representation of the draw color for display of the layer. Note: RGB values are separated by commas.
FLASH_COLOR	The RGB representation of the flash color for display of the layer. Note: RGB values are separated by commas.

Fields in the JOB array

NAME

The name of the job. This will be directly referenced in the PANEL array.

LAYER

This field contains the layer name and Gerber file location, separated by a comma.

Note: The Gerber file location must be an actual location on your system and not localized path (i.e .../gerbers/top.gbr)

Note: For DRILL and ROUT layer types, the file location must point to a NC file (not Gerber). The NC file must contain tool number, sizes in the header. If not, we recommend that you define a NCTOOLS array in the FAB 3000 Import Matrix before the JOB array.

Fields in the PANEL array

NAME	The name of the panel. This will be the name FAB 3000 uses when it creates the panel.
UNITS	Units to use for this panel array. Must be either: INCH or MM
WIDTH	Panel Width. Note: The value is defined in the panel units.
HEIGHT	Panel Height. Note: The value is defined in the panel units.
STEPREPEAT	This field contains the Job Name, X and Y Origin, X and Y Spacing, X and Y Count, Job Angle (must be 0, 90, 180, 270), and Mirror (must be either: YES or NO) all separated by a commas. Note: Origin and Spacing values are defined in the panel units. Note: If you only require a 1 up (no array) assign X and Y Spacing to 0; X and Y Count to 1.

Note: Jobs must be referenced before Panel

Fields in the NCTOOLS array

UNITS	Units to use for this nctools array. Must be either: INCH or MM
INTEGER DECIMAL	Integer digits for drill or rout file between (0-6). Decimal digits for drill or rout file between (0-6).
TYPE	Drill or rout file type. ABSOLUTE -- Use Absolute coordinates during NC Import INCREMENTAL -- Use Incremental coordinates during NC Import
SUPPRESSION	Drill or rout file zero suppression. LEADING -- Suppress Leading Zeros during NC Import TRAILING -- Suppress Trailing Zeros during NC Import NONE -- No Zero Suppression during NC Import
TOOL	This field contains the Tool # (between 1 to 1000), Diameter (in Tool Units), and Plated (either: YES or NO); all separated by a commas.

Note: NCTOOLS array is optional. It is only intended for NC files that don't include tool definitions in the header. Must be called before Job

# - Comment Line (Ignored by FAB 3000). Any line that begins with the pound character (#) will be ignored by FAB 3000.