Manufacturing Outputs (Gerber/ODB++/IDF)

Overview

These dialogue forms provide configuration options for exporting the layout for manufacture. The same layer selection and output generation controls appear on three dialogues: CADCAM (Gerber and Excellon) Output, opened by Output menu > Generate Gerber/Excellon Files; the ODB++ database dialogue, opened by Output menu > Generate ODB++ Database; and the IDF database dialogue, opened by Output menu > Generate IDF Database. Sections marked Gerber/Excellon Only appear on the first of these only. The 3D M-CAD export has its own dialogue and its own topic.

This topic is also the reference for the three layer states, which are used by every output dialogue that presents a layer selector.

Options

Output Generation

These options allow you to configure the destination and format of the CADCAM output files and also to automatically perform actions immediately after generation of the files.

  • Filestem, specify the filestem for your output files. This is useful if you want to prefix all your CADCAM files with a filestem different from the name of the project file, to indicate revisions for example.
  • Folder, specify the output folder for your CADCAM files. By default all files will be written to the project directory, the same directory as the layout file. You can specify a new default location via the Set Paths command on the System menu.
  • Output to Individual TXT files?, check this box if you want all files to be exported individually. The files will be placed in the folder specified above. You may want to use the Automatically open output folder option in tandem with this selection.
  • Output to ODB++ database folder?, check this box to write the output as an ODB++ database, a structured folder tree rather than a set of flat artwork files. The database folder is created inside the folder specified above.
  • Output to single ZIP file?, check this box if you want all the CADCAM files to be exported into a single zip archive. The zip archive will be placed in the folder specified above. You may want to use the Automatically open zip file option in tandem with this selection.
  • Automatically open output folder?, check this box if you want to automatically open the folder containing the CADCAM files in Windows Explorer following the CADCAM operation. Typically this option is useful if you have specified the Output to individual text files option on the left.
  • Automatically open ZIP file?, check this box if you want to automatically open the zip file containing the CADCAM files following the CADCAM operation. This option is only useful if you have specified the Output to a single zip file option on the left.

Layers/Artworks

The layer selector panel determines which layers of the board are included in the output. Each layer checkbox has a tri-state selection that allows you to override the automatic layer detection.

Icon State Description
✱ Auto The layer is included or excluded automatically based on whether the design has content on that layer. This is the default for all layers.
✎ (bold) Manual On The layer is forced on. It will be included in the output even if the design has no content on that layer.
✎ (bold) Manual Off The layer is forced off. It will be excluded from the output even if the design has content on that layer.

Clicking a layer checkbox moves it through the three states. The first click always takes the layer away from whatever its automatic state was, so a layer that is automatically on becomes Manual Off and a layer that is automatically off becomes Manual On. The second click forces it to the same setting the automatic state would have given, and the third click returns it to Auto. The icon and font weight update at each step to show which state the layer is now in.

The Turn On, Turn Off and To Auto buttons in the Quick Select group provide quick ways to configure multiple layers at once. Turn On and Turn Off set layers to Manual On or Manual Off respectively, whilst To Auto returns layers to the Auto state. The combo box beside them chooses the scope, either For Current Tab or For All Layers.

When this dialogue is launched as a standalone operation, all layer selections reset to Auto each time the dialogue opens. To persist manual layer overrides across sessions, configure the layers within an Output Job profile. The Output Job Manager stores your overrides within the profile so that they are applied automatically each time the job runs.

Note that you can include top assembly and bottom assembly with both ODB++ and Gerber X2 output formats.

Apply Global Gap Guard?

When checked this option will allow you to specify a global value for the guard gap on the resist layers. This should be used only where a global value for resist (pads and vias) is required, as a local change is applied to all the styles in the layout.

Rotation (Gerber/Excellon Only)

Specify the desired x-rotation for output.

Our Virtual Graphics subsystem can produce output with the x-dimension either vertical or horizontal on your peripheral. This lets you orient your work most naturally within the Layout Editor and still be able to make the best use of the size of your peripheral when producing artwork.

The terms x-horizontal and x-vertical will depend also on whether you have selected portrait or landscape mode for the print device itself. On a portrait page we define horizontal to mean parallel to the short edge.

Reflection (Gerber/Excellon Only)

Specify whether you wish normal (i.e. as seen on screen) or mirrored output.

File Units (Gerber/Excellon Only)

Specify which type of file units you wish to use for the aperture information. Metric is the default as it will have the highest precision.

Gerber Format (Gerber/Excellon Only)

Specify whether the newer Gerber X2 or the older RS274X format. Gerber X2 has the major advantages of including the IPC-D-356 netlist, having separated drill files and including automatic attribute data.

Slotting/Routing Layer

Unfortunately, there is no widely accepted mechanism within the industry for specifying the location of slots and cut-outs within the CADCAM data. Therefore, the best we can do is to output the co-ordinates of each routing stroke in Gerber format, and then leave it to individual board manufacturers to convert the data for their own particular routing machines.

To do this, we make use of one of the MECH layers. Use this option to specify which MECH layer is to be used. 2D graphics placed on that layer will then also be interpreted as defining routing strokes.

Please refer to the topic on slotting and mechanical data for more information as the location of the routing data may vary between output formats.

It is important to ensure that your board manufacturer understands that the specified MECH layer contains routing co-ordinates in Gerber format. You will need to tell them this explicitly.

Bitmap/Font Rasterizer

Use this combo box to specify the output resolution of any bitmaps and fonts on the layout. The rasterization process converts these objects into bitmaps. Bitmap images are formed from lines (rows) of adjacent pixels, such rows being referred to as rasters. It follows then that the higher the resolution setting the better the tonality of the resulting bitmaps but the larger the files. In general this option can be left at the default setting.

Run Gerber view when done? (Gerber/Excellon Only)

When checked this option will automatically launch the Gerber Viewer and load in the CADCAM files after completing the CADCAM generation.

Via Filling

When checked, the via filling option instructs the CADCAM generator to mark CNC-drilled through-hole vias for non-conductive via fill (NCVF) in the output data. This is relevant to designs where via-in-pad or similar techniques require resin-filled and capped vias (IPC-4761 Type VII).

Micro-vias (laser-drilled blind vias spanning a single dielectric layer) are always filled with copper during the sequential lamination electroplating process. They do not require the NCVF resin fill process and are therefore automatically treated as filled in the CADCAM output regardless of this setting. The via filling option applies only to mechanically (CNC) drilled vias.

Run Valor ODB++ Viewer When Done?

When checked this option will automatically launch the Valor ODB++ Viewer and load in the CADCAM files after completing the CADCAM generation.

Note that since the takeover by Mentor the Valor viewer is not easily sourced on the net. The replacement Mentor Viewer is also free of charge but does not integrate directly with Proteus.