Artwork Files

Traditional Artwork files, or Gerber data, are text files containing data to control a photoplotter. The photoplotter plots a master image for exposure onto the light sensitive coating applied to a blank laminate before etching. Whilst there are, more modern, “intelligent” Artwork formats, like ODB++ and IPC-2581, many users prefer to supply Gerber data because the output files are devoid of any details of the source design. The “intelligent” Artwork formats have other benefits related to processing the design but they may also contain details of the source design which some users prefer not to share, unless steps are taken to remove the design data from the output. The Gerber data has one file per film that is required. Films are created for, at least, the Etch, conductor, layers but there may be a number of other films related to the board like Silkscreen, Soldermask (resist) and Solderpaste, and related to processing and documentation, like Assembly, Drill drawing and so on.

Defining Films

The most productive way to define films is to set the display visibility to the required Classes and Subclasses and then Add the Film and the contents will match the display. If the Film contents are incorrect, the display visibility can be changed, the Film selected and Match Display used to set the Film contents to match the current display. The Film contents can also be defined by manually selecting the Film Contents from the available Classes and Subclasses. Classes and Subclasses can also be added to existing Films by manual selection. It is also possible to select a Film and set the display to it’s contents. If the mask layers (silkscreen, soldermask etc) are added to the cross section of the board, these are added automatically using the Create Missing Films button. Films can also be stored into a text file called film_setup.txt (select the required films and right click>Save All Checked)  and then reused using either a parameter file, template file or imported using the Add button.

Generating Artwork

Once the Films have been defined, the artwork can be generated. Films may be output selectively but, more typically, all of the configured Films are generated. Shapes will need to be set to Smooth and be up to date before the Films can be generated. There will be a button shown on the Film Control form if Dynamic Shapes need updating.

Artwork parameters need to be configured to accept the resolution of the board. For RS-274X the number of decimal places output needs to be one greater than the board database. For example, a board with an accuracy of 3 decimal places of mm, will need a artwork accuracy of 4 decimal places – that’s a tenth of a micron and it’s unlikely than any etching process could manage that. The default integer places is 2, that will mean a maximum dimension of 99mm, and this will often need to be increased. There will be a warning in the log file if the number of integer places is insufficient to handle the design.

One output file will be created for each Film defined with the Film name and a default file extension of “.art”. There is the option to add a Prefix and Suffix to the Film Name and the file extension is stored as a user preference if an alternative to “.art” is required.

A photoplot.log file will be written to report on the artwork generation. If the design does not have a Photoplot Outline defined, the photoplot.log file will contain a warning about this but nothing in the output will be affected by this. If there is a Photoplot Outline defined, no Gerber data will be generated outside of the outline, this can cause a lot of confusion if the board is ever changed and the updated board needs artwork details that are now outside of the Photoplot Outline.

Line and text items that do have a thickness defined (zero width) are not processed by Gerber creation. It is recommended that all items have a thickness defined. For text this can be done by Setup>Design Parameters, Text tab then left click on Setup Text Sizes and ensure that a Photo Width value is defined. For line items you can specify a width (0.2mm for example) when the items are added. There is a safe guard setting in the Artwork control form called undefined line width that can be set on a film name by film name basis to catch any undefined items, There is also a user preference (Setup>User Preferences>Manufacture>Artwork) called artwork_undef_line_width which will set this for any new films created.

Viewing Artwork

PCB Editor can open artwork files that it has generated but cannot open artwork data form other sources. There are Gerber viewer utilities available if an “independent” view of the exported data is required.

Drill and Router files

The fabricator will need to get Drill, and possibly Router, files to machine any holes or slots in the board. The outline will usually be determined from the artwork data. There will be multiple drill files created to fabricate any blind and buried Vias as the board is built. There will be a message in the ncdill.log file if the board contains any slots that require Router file generation.

All content Copyright 2022 Parallel Systems Ltd.