Generate Outputs
The Generate outputs command opens the Generate output files dialog, which provides controls to configure and generate manufacturing outputs from the current board design in a batch-style release process. The command is accessed from the PCB editor, schematic editor, and the Layer Stack Editor by choosing Project | Project Actions | Generate outputs from the main menus.
The Generate output files dialog provides controls to configure and generate manufacturing outputs from the current board design in a batch-style release process. To fabricate a printed circuit board, there are a variety of files needed in specific formats, such as Gerber, NC drill, or ODB++. You also need to be able to generate documentation outputs, such as print-type outputs to Windows printers, and tabular output suitable for the Bill of Materials.
CircuitMaker has built-in support for all of the needed output types, including Microsoft Excel format output with support for Excel templates.
Generating Output Files
The Generate Output Files dialog is used for three distinct output processes, which are performed individually. These are: Generating output files for the enabled outputs, Viewing the enabled outputs, or Releasing the enabled outputs. All output types are generated as files, which can then be opened for viewing, or released.
To use the dialog:
- Configure the Required Output – click the Configure... link to open a dialog and define the requirements of that output type, such as included layers, format of the BOM, and so on.
- Set Up the Output Page – click the Page setup... link to define how that output type should appear on the output page.
-
Enable the Required Output – click the Enabled checkbox to include that output type.
-
Generate – click to run the release process. The Electrical Rules Check validation report will be run first (if enabled), checking the electrical/drafting validity of the captured source design. All other defined (and enabled) outputs are then run. These are the manufacturing outputs from which the physical Item will be produced to exist as a tangible product that can be bought and sold. Information regarding the Electrical Rules Check validation report will also be listed in the Messages panel, which will appear after the Generate button is clicked.
The generated output is stored under the \Default Configuration folder - a child folder of the directory containing the project file. Separate sub-folders will be generated to contain specific output as applicable for BOM, ERC, Gerber, NC Drill, and ODB. In addition, certain outputs will be available from the Projects panel (including BOM and HTML-based ERC report).
A PDF document will be generated, named [<ProjectName>.PrjPcb] <ProjectName>.pdf. This will contain entries for the following generated output (where enabled): Electrical Rules Check, BOM, Schematic Prints, PCB Prints, PCB 3D Print, and Assembly Drawings.
Each time a release is performed, the previously generated output(s) will be deleted and replaced with the enabled and newly generated output(s).
- View – after output generation, and with a specific output type selected in the list, click this button to open that output for viewing. An output can only be Viewed or Released if it is Up to date.
-
Release – this button becomes available after successful output generation. Click to release the generated output; the Confirm Release dialog opens. The dialog displays the data to be released. If the data is correct, you can add notes about the release then click OK to perform the release. Upon successful release, the Project Release dialog opens stating that the project has been released, and includes a link that opens the project in your Web Browser.
Outputers List
The main region of the dialog presents a listing of all supported output types that can be generated from the design. Output types are grouped into the following categories:
- BOM - this category offers the following output types: Bill of Materials.
- Documentation - this category offers the following output types: Schematic Prints, PCB Prints, PCB 3D Print, and PDF3D.
- Fabrication - this category offers the following output types: Gerber Files, NC Drill Files, ODB++ Files, and Report Board Stack.
- Assembly - this category offers the following output types: Generates pick and place files and Assembly Drawings.
- Validation - this category offers the following output types: Design Rules Check and Electrical Rules Check.
- Export - this category offers the following output types: Export STEP.
Each specific output type is presented with the following fields:
- Output Generator - the type of output generator, the name of which indicates the type of output that will be generated.
- Configure - click this button to access an associated dialog with which to configure the currently selected output generator. The dialogs involved are:
- BOM_PartType for Project <project name> dialog - for configuring Bill of Materials outputs.
- Schematic Print Properties dialog - for configuring Schematic Prints.
- PCB Printout Properties dialog - for configuring PCB Prints and Assembly Drawings.
- PCB 3D Print Settings dialog - for configuring PCB 3D Prints.
- PDF3D dialog - for configuring PDF3D output.
- Gerber Setup dialog - for configuring Gerber output.
- NC Drill Setup dialog - for configuring NC Drill output.
- ODB++ Setup dialog - for configuring ODB++ output.
- Layer Stack Report Setup dialog - for configuring Report Board Stack outputs.
- Pick and Place Setup dialog - for configuring Pick and Place outputs.
- Electrical Rules Check Setup dialog - for configuring an Electrical Rules Check validation report.
- Export Options dialog - for configuring STEP outputs.
- Page Setup - click to open the associated properties dialog to configure the printout.
- Status - the current state of the output. The following possible states exist:
- The output is currently in the process of being generated.
-
The output has been generated successfully. For an ERC report, there are either no errors or the level of those errors falls within the specified maximum tolerated error level for that report.
If the output cannot be generated successfully, an error dialog will appear alerting you to the fact that validation has failed. For the validation-based ERC output, this means there are errors within the source design documents that are causing certain check(s) to fail. For a standard output, the output could not be generated successfully. Perhaps Fatal Errors exist when performing a pre-generation compile, or something is amiss in the configuration of the associated output generator.
- Enabled - indicates whether this output type is to be included in the batch generation of outputs (enabled), or not (disabled).
BOM_PartType for Project Dialog
The Bill of Materials dialog provides a listing of all components required to build the product and the ability to export the Bill of Materials report.
The Bill of Materials, or BOM, is a key ingredient of the data set generated from a board design project. This report-type document provides a listing of all components required to build the product, including the bare board, which is essentially the base 'component' upon which all other parts are assembled. The BOM acts as a guide for what needs to be procured to build the product as designed. It also provides a means to calculate cost based on the required number of assembled boards in a requested spin.
The Bill of Materials dialog presents the various properties/parameters for all components on the source document(s). Each property/parameter has its own column. You can simply choose which data to include in the generated BOM report. Data can be grouped, sorted and filtered as required, with the ability to include additional parametric data from a nominated PCB for the project, as required.
The following sections take a closer look at the manipulation of the data to arrive at the desired BOM content prior to exporting the report.
View Mode
There are three view modes available to display the list of BOM Items. Select the required mode using the buttons located above the list:
-
Flat view - click to displays a row for every component. -
Base view - click to display a row for each unique component in the project. The Designator column lists the designators of all components of this type. -
Consolidated view - click to use when the project includes variants to display a Consolidated BOM for all variants.
Variant
If there are variants defined in the project, they will be listed in the drop-down next to the view mode selectors. Choose the required variant from the drop-down. If Consolidated view is enabled, this control is not available.
Preview
Click 
to generate a preview of the BOM based on the current settings of the File Format and Template options.
The BOM Items list supports the following features:
- Use the Columns tab in the Properties region of the dialog to display/hide a column.
- Drag and drop to change the order of columns.
- Click a column heading to sort by that column; hold Shift to sub-sort on the subsequent column(s).
- Click the Filter icon that is available when hovering over a column name (
) to filter by column values using the Select Columns dialog. - Use the standard Windows shortcuts to scroll through the list of BOM Items:
- To scroll vertically, use the MouseWheelRoll.
- To scroll horizontally, use the Shift+MouseWheel Roll.
Properties
The main region of the dialog lists all of the components.
BOM Items
-
Show Not Fitted - enable this option to display the Not Fitted Items in the BOM Item grid.
- Include DB Parameters in Variations - if there are database components that have been placed and those components are varied in a design Variant, enable this option to update the database parameters when the selected variant is changed.
Supply Chain
Supplier data is available only when generating a report for the project. It is not available when generating a report for a PCB document.
- Production Quantity - enter the quantity or use the arrows to select the quantity that needs to be ordered to produce the given product quantity.
- Currency - use the drop-down to select the desired currency.
- Cached - click this to display the last cached pricing data if working offline.
- Real-time - click this to display pricing-based data for components with links to Supply Chain Data that are updated in real-time.
Export Options
- File Format - select a format from the drop-down list. The following file formats are supported:
- CSV (Comma Delimited) (*.csv)
- Tab Delimited Text (*.txt)
- MS-Excel (*.xls, *.xlsx) (uses Microsoft Excel)
- Generic XLS (*.xls, *.xlsx) (uses a built-in XLS-format file generator, so that this format can be generated without having Microsoft Excel installed)
- Portable Document Format (*.pdf)
- Web Page (*.htm, *.html)
- XML Spreadsheet (*.xml)
- Template - enter the desired Excel template file by either typing the file name into the text box, using the drop-down and selecting a template file (*.xlt), or browsing for the template file by clicking:
- Add to Project - enable to have the generated report added to the project after it is created.
- Open Exported - enable to open the relevant software application, e.g., Microsoft Excel, once the exported file has been saved.
Columns Tab Options
This region of the dialog is used to configure which parameters are displayed for each BOM Item and the data sources that are available for those parameters.
- Search - use to quickly locate parameters of interest. The software will search for the typed text anywhere within the Name or Alias strings.
- Sources - the BOM can also include information taken from the following additional data sources:
-
- enable to include Workspace items. -
- enable to include PCB location/rotation/side of board data in the available Columns for each of the components. -
- enable to load additional component parameters from an external database. -
- enable to include all detected schematic document parameters across all schematics in the PCB project in the available Columns.
-
- Drag a column to group - like-components will be grouped in the BOM when the contents of all grouped columns match. Click, hold, and drag a column from the Columns section of the dialog, then drop it in the Drag a column to group section to include it as a grouping parameter.
- Columns - lists all available sources of part information. The region can be sorted by clicking on any of the heading fields, including the Visibility and Source columns.
- Visibility - click on the eye icon in the left column to control the visibility of that column in the main BOM Items grid.
- Source - displays an icon to show from where that parameter is sourced:
-
- sourced from the schematic. -
- sourced from the BOM. -
- sourced from a Workspace.
-
- Name - displays the name of the property/parameter as defined in the source document.
- Alias - if required, an alias can be defined to rename a column.
Additional Controls
- Export - click to generate the report. A standard Windows dialog in which you can name the report will be presented.
PDF3D Dialog
The PDF3D dialog provides controls to configure how the exported PDF will look and behave. It allows you to define the rendering, behavior and the included design content for the PDF.
The key options are described below.
-
Selected Only - enable to include specific object types that are selected in the design space.
- Merge meshes - enable to combine common groups of objects for navigation purposes, such as grouping together all pads that belong to a component.
- Exclude outside - enable to exclude all copper outside of the regular PCB boundary.
- Auto activate - when enabled, the 3D image will be automatically rendered when the PDF is opened in Acrobat Reader. If disabled, a Click to activate button icon will first appear in the PDF.
- Toolbar - enables the 3D Toolbar in the PDF Reader.
- Navigation - enables the Model Tree Navigation pane in the PDF Reader.
- Use 3D Movie views - enable to include Key Frames defined in the PCB document as part of the export. The Key Frames exported to the PDF 3D document will then be available as selectable views in Acrobat Reader. When the PDF 3D document is opened in Adobe Reader, the additional Key Frame views appear in the View selection area of the Model Tree navigation pane, along with the standard Default/Top/Bottom/Left views.
- View - defines the initial view angle in the PDF Reader.
- Light - defines the initial 3D light source type in the PDF Reader.
- Color - defines the initial image background color.
- Color scheme - Use the drop-down to choose the PDF render style from a list of predefined options, which includes the system's current 3D View settings and the board layer colors.
Gerber Setup Dialog
The Gerber Setup dialog allows you to specify the layers to be plotted and configure related additional options when generating output from the active PCB in Gerber format.
General Tab
The General tab of the Gerber Setup dialog
- Units
- 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.
- Format
- 2:3 - provides a resolution of 1 mil (1/1000 inch).
- 2:4 - provides a resolution of 0.1 mil.
- 2:5 - provides a resolution of 0.01 mil.
Layers Tab
The Layers tab of the Gerber Setup dialog
Layers To Plot
This region is a list of layers that can be plotted as part of Gerber generation.
- Plot - check the Plot box next to each specific layer(s) you want to plot as part of the generated output.
- Mirror - check the Mirror box to the right of each layer if you want a mirrored Gerber file to be created.
Mechanical Layer(s) to Add to All Plots
Check the box next to each mechanical layer(s) you want added to all plots.
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.
Mirror Layers
Use the drop-down to access a menu of commands that allow the Mirror field for all layers in the Layers to Plot region to be enabled or disabled:
- All On - select to check all boxes in the Mirror column (mirrored Gerber data will be created for all checked layers).
- All Off - select to clear all checked boxes in the Mirror column (no mirrored Gerber data will be created).
- Used On - select to check all boxes in the Mirror column of the layers that are used in the design.
Right-click Menu
The Plot Layers and Mirror Layers commands also can be accessed by right-clicking the layer name in the list region. The following are additional commands included on the right-click menu:
- Add Layer Class - click to open the Layer Class Name dialog then enter a name for the new layer.
- Edit Layer Class - click to edit the name of a Layer Class.
Include unconnected mid-layer pads
Check this box to allow unconnected pads in the mid-layer on Gerber plots.
Drill Drawing Tab
The Drill Drawing tab of the Gerber Setup dialog
Use this tab to specify that a drill drawing is required. Mirrored plots can also be specified.
Drill Drawing Plots
- Plot all used drill pairs - check this option to plot all used drill pairs in drill drawing plots.
- Mirror plots - check this option to mirror layer pairs in drill drawing plots.
- Configure Drill Symbols - click to open the Drill Symbols dialog in which you can configure the drill symbols.
- Layer Pairs Region - this area shows all defined layer pairs in the design. Check the box in front of each desired layer pair to draw that layer pair in drill drawing plots. The check box is accessible only when Plot all used drill pairs is unchecked.
Drill Guide Plots
- Plot all used drill pairs - check this option to plot all used drill pairs in drill guide plots.
- Mirror plots - check this option to mirror drill guide plots.
- Layer Pairs Region - this area shows all defined layer pairs in the design. Check the box in front of each desired layer pair to draw that layer pair in drill guide plots. The check box is accessible only when Plot all used drill pairs is unchecked.
Apertures Tab
The Apertures tab of the Gerber Setup dialog
Use this tab to set up the required aperture information for the design.
- Embedded apertures (RS274X) - when this option is enabled, the apertures are embedded in the Gerber files according to the RS274X standard and all information for each layer is contained in a single file. Enabling this option ensures that the current apertures list includes all the required apertures. If this option is disabled, the Options region and additional controls become available.
- Apertures List - lists all the current aperture data.
- Options - use this region to select the following:
- Maximum aperture size - input the maximum size of the apertures for the design.
- Generate relief shapes - check this option to create relief style apertures.
- Flash pad shapes- check this option to flash the pad shapes.
- Flash all fills - check this option to flash all fills.
- Additional Controls
- New - click to open the DCode dialog. Enter the DCode then click OK to open the Aperture dialog in which you can specify the properties of the new aperture. The DCode is a code assigned to that size aperture.
- Edit - click to edit the properties of the selected aperture.
- Rename - click to open the DCode dialog. Enter the new DCode name of the selected aperture.
- Clear - click to clear all apertures from the Apertures List. A confirmation box appears before clearing.
- Delete - click to delete the selected aperture.
- Create List From PCB - click to create the Apertures List from the current PCB design.
- Load - click to open a dialog with which you can select the location of the aperture file to load.
- Save - click to save the current apertures in the Apertures List.
Notes on Apertures
Unless your PCB manufacturer does not support embedded apertures, it is highly recommended that you use the Embedded apertures (RS274X) option. Most modern photoplotters are raster plotters that can accept any size aperture. Generally, they also accept Gerber files with embedded apertures.
If your manufacturer does not use embedded apertures, a separate aperture file (*.apt) must be included with the Gerber files. If you use an existing aperture file rather than a generated one, the PCB Editor scans the primitives (tracks, pads, etc.,) in the PCB document and matches these with aperture descriptions in the loaded *.apt file. If there is no exact match of aperture to primitive, the PCB Editor will automatically paint the primitive with a suitable smaller aperture. If there is no aperture suitable with which to paint, a *.MAT (match) file will be generated listing the missing apertures and Gerber file generation will be aborted.
Advanced Tab
The Advanced tab of the Gerber Setup dialog
Use this tab to specify options such as film size, position on film, and plotter type to be used during Gerber generation.
Film Size
- X (horizontal) - enter a value for the film length.
- Y (vertical) - enter a value for the film width.
- Border size - enter a value for the border size of the film.
Aperture Matching Tolerances
- Plus - use this box to define the positive tolerance for aperture matching.
- Minus - use this box to define the negative tolerance for aperture matching.
Batch Mode
- Separate file per layer - select this option if you want each layer to generate a separate Gerber file.
- Panelize layers - select this option if you want only one Gerber file to be generated in the format of panelization.
Leading/Trailing Zeroes
- Keep leading and trailing zeroes - if this option is enabled, all leading and trailing zeroes will appear in the generated Gerber file.
- Suppress leading zeroes - if this option is enabled, no leading zeroes will appear in the generated Gerber file.
- Suppress trailing zeroes - if this option is enabled, no trailing zeroes will appear in the generated Gerber file.
Position on Film
Use the following options to choose the position on the film:
- Reference to absolute origin
- Reference to relative origin
- Center on film
Plotter Type
- Unsorted (raster) - select to use raster machine (default).
- Sorted (vector) - select to use vector machine.
Other
- G54 on aperture change - check this option to rotate the aperture wheel of the plotter after each aperture change.
- Use software arcs - check this option to use software arcs.
- Use polygons for octagonal pads - check this option to use polygons for any octagonal pads.
- 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) - check this option to generate a DRC Rules Export file (.RUL). This file report details the design rules for the source PCB document from which the Gerber data is being generated.
NC Drill Setup Dialog
The NC Drill Setup dialog is used to configure NC Drill file output options.
Options
- NC Drill Format - use this region to specify the units and format to be used in the NC Drill output files.
- Units
- 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.
- Format
- 2:3 - provides a resolution of 1 mil (1/1000 inch).
- 2:4 - provides a resolution of 0.1 mil.
- 2:5 - provides a resolution of 0.01 mil.
- Leading/Trailing Zeroes - zero suppression is a technique that reduces the size of the generated data files by removing all zeroes from the start (leading) or end (trailing) of numbers.
- Keep leading and trailing zeroes - if this option is enabled, all leading and trailing zeroes will appear in the generated NC Drill file.
- Suppress leading zeroes - if this option is enabled, no leading zeroes will appear in the generated NC Drill file.
- Suppress trailing zeroes - if this option is enabled, no trailing zeroes will appear in the generated NC Drill file.
- Coordinate Positions
- Reference to absolute origin - use the absolute origin as the reference point.
- Reference to relative origin - use the relative origin as the reference point.
- Other
- Optimize change location commands - check this option to optimize any change location commands.
- Generate separate NC Drill files for plated & non-plated holes - check this option to create separate drill files for plated and unplated holes.
- Use drilled slot command (G85) - check this option to use multiple drilled holes to create slots.
- Generate Board Edge Rout Paths - check this option to create a separate NC Rout file to define the board shape, including board cutouts.
- Rout Tool Dia - specify the tool size used to rout the board outline. This option is only available when Generate Board Edge Rout Paths is enabled.
- Generate EIA Binary Drill File (.DRL) - use this option to generate a .DRL file. DRL is a binary format drill file. For a multi-layer PCB that incorporates blind and/or buried vias, a separate drill file for each layer pair is created with a unique file extension.
ODB++ Setup Dialog
The ODB++ Setup dialog provides controls to configure the ODB++ file output options. ODB++ is a CAD-to-CAM data exchange format used in the design and manufacture of printed circuit boards. The format was originally developed by Valor Computerized Systems, Ltd., as an open database that could provide an information-rich data exchange between PCB design software and Valor CAD-CAM software used by PCB fabricators.
The key options of the dialog are described below.
- Generate DRC Rules export file (.RUL) - select to generate a .RUL file that contains all design rules defined for the source document from which the ODB++ data is being generated.
- Layers to Plot - enable the specific layer(s) you want to plot as part of the generated output.
- Plot Layers - use the drop-down to select a group of layers to plot. These commands are also available on the right-click menu.
Layer Stack Report Setup Dialog
The Layer Stack Report Setup dialog allows you to specify the unit of measure in the fabrication output that is generated after clicking OK.
Pick and Place Setup Dialog
The Pick and Place Setup allows you to configure pick and place options.
The key options are described below.
- Grid region - this region is a preview of the information that will be included in the output file.
- Exclude Filter Parameters - enable to exclude parameters being used for filtering (refer to the Notes section below for more information).
Notes
To exclude specific parts from the report, the dialog provides the ability to apply custom filtering. To apply filtering, click the filter icon in a column header. The subsequent drop-down lists all individual row entries for quick selective filtering. Click the (Custom…) entry to open the Custom Filter dialog in which you can specify which rows of data to show in the report based on the filtering criteria defined for that column. Once applied, the filter icon turns blue to indicate custom filtering is in force for that column. The full filter currently applied is reflected at the bottom-left of the grid region. Columns being used for filtering can also be excluded from the generated pick and place files by enabling the Exclude Filter Parameters option.
Export Options Dialog
The Export Options dialog is used to configure options of PCB export to the STEP file.
Board Options
- Skip Free 3D Bodies - enable to export without free 3D models.
- Skip Hidden 3D Bodies - enable to export without hidden 3D models.
- Export As Single Part - check to export the STEP file as a single part or as one model per component. When this option is enabled, the STEP file will be saved as a part and not as an assembly.
3D Bodies Export Options
These options apply to components that have both extruded (simple) 3D bodies and Generic 3D bodies assigned to them:
- Prefer simple bodies - export the extruded (simple) 3D body version of the component.
- Prefer generic 3D models - export the generic 3D body version.
- Export both - export both extruded and generic 3D body versions.
If only extruded 3D bodies are available for components, they will always be exported.
Pad Holes
Use the following options to select which holes to include in the exported file. The options are designed to offer a choice between full and limited detail in order to speed up the export process and reduce file size.
- Export Mechanical Component Pad Holes - check this box to export any mechanical component pad holes.
- Export Electrical Component Pad Holes - check this box to export any electrical component pad holes.
- Export Free Pad Holes - check this box to export any free pad holes.
Component Suffix
Use the following options to specify the suffix of the exported components.
- None - no suffix will be applied to components.
- Board file name - use generic 3D filename as the component suffix.
- Custom - select to customize the component suffix. Enter the custom suffix in the text box.
Right-Click Menu
To access the right-click menu, ensure the cursor is over the area occupied by the output type entries and not in the blank space beneath.
The following commands are available from the right-click context menu for the dialog:
- Configure - use this command to access an associated dialog in which you can configure the currently selected output generator.
- Disable - use this command to disable the currently selected output generator, excluding it from the batch release process.
- Enable all - use this command to quickly enable all output generators, including all in the batch release process.
- Disable all - use this command to quickly disable all output generators, excluding all from the batch release process.
- Open Document - use this command to open the generated output for the currently selected output generator. This command will only be available provided output has been successfully generated for that particular output type.