Design007 Magazine

PCBD-May2016

Issue link: http://iconnect007.uberflip.com/i/679419

Contents of this Issue

Navigation

Page 67 of 73

68 The PCB Design Magazine • May 2016 PDF is a fine and widely supported format; however it is too complex for automatic data extraction. Remarkably enough, the best option for PCB fabrication data is a plain text format, as many fabricators have software that can automatically extract information from such files. Formal information is best expressed in structured text files: comma-separated values (CSV), XML, JSON or preferably YAML. YAML is well structured and human readable, and YAML files are the easiest and safest to automate. Please do not use Excel, Word or PowerPoint formats. Firstly, by doing so you introduce yet more formats for your manufacturing partners to deal with. More importantly, they are not open formats: They are proprietary application formats whose specifications are rightfully closely-guarded secrets. They are not, therefore, data exchange formats, and their use adds unnecessary complications as automated data extraction is well-nigh impossible. They require dedicated interactive applications and cannot be built into automated workflows; what's more, version problems abound (e.g., between open source and Microsoft software). If you must choose between such formats and PDF, choose PDF without hesitation, but plain text files are best. Often, general PCB data is delivered in drawings. This is an excellent and time-honored practice in all fabrication industries, but here too, data cannot realistically be extracted from drawings. Again, as automation protects against operator error, it is advisable to put all your general data in text files, even if it is already in a drawing. Always place all of your general data in human-readable text files, informally or structured as in CSV, XML and YAML. Do not use Excel, Word or Power Point formats for this purpose. Chapter 12: Number of Digits Used for Coordinates Use the same resolution and number of digits (resolution) for all data layers. If you use different resolutions for different layers, the position of the different elements will be rounded differently. The result is that, say, via pads and drill pads end up being out of alignment. You can only hope then that the CAM engineer notices this and "snaps" the via pads to the drill holes. This of course changes the copper image, which is something the CAM engineer is not supposed to do, but he is also supposed to deliver a perfectly aligned PCB. So he's damned if he does, and he's damned if he doesn't. Misalignment sometimes arises even when the same resolution is applied to all layers. This is usually because the output processors for Gerber and for Excellon round differently. As for other issues mentioned above, the simplest solution is to output the drill/rout layers in Gerber. (See Chapter 2 in this series.) Ideally, Gerber files use six decimal places in inches and five or six decimal places in mm. If your software cannot produce these resolutions then get as close as you can. Some recommend the use of lower resolutions, probably to save a few bytes. Who cares about saving a few bytes? Don't follow this recommendation: lower resolution increases rounding errors. This not only affects alignment, but, more importantly, it increases the risk of serious problems because these rounding errors can make contours self-intersect, which is invalid and result in invalid arcs. Low resolution is the root cause of most of the few image errors in Gerber files; it does not happen often but it makes no sense to take this risk to save a few bytes. Another reason given to use low resolution is that the drilling machine may not be able to handle big files. This may well be true but it is irrelevant: as we have already seen, the CAM system will output drill files exactly as the driller needs them. Remember: Use the maximum precision for co-ordinates, and output all layers with the same precision. PCBDESIGN This column has been excerpted from the Guide to PCB Fabrication Data: Design to Fabrication Data Transfer. Karel Tavernier is the managing director of Ucamco. THE GERBER GUIDE, CHAPTERS 11 & 12

Articles in this issue

Links on this page

Archives of this issue

view archives of Design007 Magazine - PCBD-May2016