This dialog allows you to specify the layers to be plotted and configure related additional options when generating output from the active PCB in Gerber X2 format. Gerber X2 is a direct and advanced evolution of the existing Gerber RS-274X standard and adds a large range of additional data for PCB fabrication and assembly.
A prime advantage of the Gerber X2 format is backward compatibility with the older Gerber RS-274X standard. Being a multi-file standard, a target fab/assembly house that has not moved to the new standard can extract the traditional Gerber file elements as needed. This may be a significant advantage for those unwilling to tackle a major shift in fabrication file formats or for fabrication houses with inflexible equipment and software.
The Gerber X2 Setup dialog is accessed from the PCB Editor by clicking File » Fabrication Outputs » Gerber X2 Files.
Use this region to choose the units used in the generated file:
Inches - enable this option to use imperial units where all work is done in mils (1/1000 inch).
Millimeters - enable this option to use metric units where all work is done in millimeters.
Use this region to specify the numerical precision of the plot coordinates in the Gerber file:
2:3 - providing a resolution of 1 mil (1/1000 inch).
2:4 - providing a resolution of 0.1 mil.
2:5 - providing a resolution of 0.01 mil.
2:6 - providing a resolution of 0.001 mil.
The first number represents the number of digits before the decimal point; the second is the number of digits after the decimal point. With the 2:3 format for example, the largest number in the Gerber file could be 99.999 inches and the smallest number could be 0.001 inches (1 mil).
The format is selected to suit the placement precision of the objects in the PCB workspace and/or fabricator preferences (normally set to the highest resolution: 2:6).
Use the options in this region to set the tolerance range used when matching apertures for each item in the plots.
Plus - use to define the positive tolerance for aperture matching.
Minus - use to define the negative tolerance for aperture matching.
If no exact match for an item is available in the current aperture list, the software checks to see if a slightly smaller or larger aperture exists within this tolerance range and uses it instead. If no suitable aperture exists within the tolerance range, the software will attempt to ‘paint’ with a smaller aperture to create the required shape. This requires that a suitable smaller aperture is available and that this aperture can be used for ‘painting’.
Aperture match tolerances are normally used only when targeting a vector photoplotter, which requires a fixed or supplied aperture file. They will not be required if the apertures have been created from the PCB and ‘flashed’. If match tolerances are not required, they should be left at the default of 0.005 mil.
Use this region to specify the target photoplotter type:
Unsorted (raster) - select to use raster machine (default).
Sorted (vector) - select to use vector machine.
Gerber files can be created with the data sorted by its position on the ‘film’ or unsorted. Sorting is required only by vector photoplotters and does not apply to modern raster-style plotters that create an initial image internally. If sorting is enabled, Gerber generation may take an extended time.
Optimize change location commands – when this option is enabled, X or Y location data is not included if it does not change from one object to the next.
Generate DRC Rules export file (.RUL) - enable this option to generate a DRC Rules Export file. The report details the design rules defined for the source PCB document from which the Gerber data is being generated.
Gerber X2 Specific
File Subject – use this field to select the file type, which is included as a Part attribute in the Gerber X2 outputs. The drop-down list provides the following choices:
Autodetect – automatically assigns an attribute from the below list based on the type of board file. For example, a PCB document containing a single board design will be assigned the Single part attribute.
Single – a single PCB.
CustomerPanel – a board array or shipping panel.
ProductionPanel – a working panel or fabrication panel.
Coupon – a coupon (performance test board associated with a main board design).
Other – none of the above. In the file, a string appended to the attribute informally indicates the part.
File Comment – enter a comment that will be included as an attribute in the generated outputs.
Layers To Plot Tab
This tab allows you to configure which layers to plot in the Gerber X2 output for the current PCB document.
Layers List - a listing of layers in the current PCB. Each layer is presented in terms of the following:
File name – the individual Gerber output file name. This uses a naming convention that is indicative of the file’s function and uses a .gbr extension. Naming is based on the project name, layer, and function, and uses an underscore character as a descriptive separator.
Layer Name – the layer name that applies to the output file as defined by the board’s layer stack.
Plot – enable this option to include a Gerber plot for that layer in the generated output. Disable to exclude the plot from being generated for that layer.
Plot Layers - use the drop-down to access a menu of commands that allow the Plot field for all layers in the Layers to Plot region to be enabled or disabled:
All On - select to check all boxes in the Plot column (Gerber data will be created for all checked layers).
All Off - select to clear all checked boxes in the Plot column (no Gerber data will be created).
Used On - select to check all boxes in the Plot column of the listed layers that are used in the design.
The above Plot Layers selections can also be accessed from the right-click menu.
Any invalid layers (violating layers) in the layer stack are displayed in red.
All relevant drill files for the current board design are listed on the Drills tab.
This tab includes the relevant drill files that will be generated for the current board design that can be selected for generation on an individual or group basis.
Drills List - this is a listing of drill files for the current PCB and includes drill drawing and guide outputs. A drill drawing is a plot of the location of each drill site on the PCB, with each drill size plotted with a different symbol. A drill guide marks each site with a small cross. Separate files are also available for plated and non-plated through-holes and blind/buried vias if included in the design. Each drill file is presented in terms of the following:
File Name – the individual Drill output file name constructed to comply with the Gerber X2 standard.
Layer Drill Pair – the Layer Drill Pair that is associated with the drill holes file. Layer Drill Pairs are configured in the Drill Pair Manager and accessed from the Layer Stack Manager.
Plot – check this box to include a Gerber plot for that drill file in the generated output. Uncheck to exclude the plot from being generated for that drill file.
Note that the Plot checkbox associated with each file type heading (Drill drawing, Drill guide, etc.) toggles the selection of all files in that section.
Plot Drills - use the drop-down to access a menu of commands that allow the Plot field for all layers in the Layers to Plot region to be enabled or disabled:
All On - select to check all boxes in the Plot column (create Gerber plots for all listed drill files).
All Off - select to uncheck all boxes in the Plot column (create no Gerber plots).
Used On - select to check all boxes in the Plot column for all used drill files (create Gerber plots for all listed drill files that are used in the design).
The above Plot Drills selections can also be accessed from the right-click menu.