BoardSurfers: Units, Accuracy, and Artwork - How to Do It Right!

It might seem simple, but database units and accuracy directly relate to the artwork generated, and it is possible to misunderstand the artwork format as it relates to the board setup. Thirty years ago, databases were set up as Mils (0.0) or Millimeter (0.1), and it was easy to output artwork for either without fabrication problems.  There were no fabrication problems to build an 8 mil line, 8 mil space, and a ½ mil tolerance. Fast forward to 2020 where PCB boards are more complex, smaller or larger, and most often denser with tighter rules. Fabrication vendors today routinely hold tolerances in tenths of Mils (that’s 0.0001 Inch, and this refers to boards, not packages). While package designs bring you into sub-microns, fiberglass is manufacturable at 0.000x Inches.

For the designer, the idea that “more accuracy must be better” is OK until "more" is beyond the ability to fabricate. It could be that those working on both packages and boards may not realize the fabrication processes are vastly different or that boards cannot be built to the same standards. Databases set to levels beyond 2 Micron should use the GDSII or IPC2581 standards, and not Gerber artwork for manufacturing media.

Allegro PCB Editor defaults to a 2.5 format (regardless of the unit) which works for most data and has been the Gerber standard for years. This is where the integer and decimal places are set in the artwork parameters:

Recently, Gerber increased support to 0.6 accuracy and PCB Editor now allows the decimal place field to accept 6 as a legal value. Remember, the Gerber standard is output as Inch or Metric only (not in the database unit). Supporting 0.6 in the artwork file will not allow you to build a board with a line width at #.000005 and measure it on the physical board, but it does allow better precision for arc data.  Arcs are written as two X Y endpoints with a center point and a radius.  Higher artwork accuracy means more precise ‘arc’ information for the photoplotter. I say this because arc center points are stored in the database as a floating-point value rather than rounding down to the database accuracy.

Example of a Single Arc in a 1 Mil Database

Show Element in PCB Editor displays the arc with endpoints, a radius, and center:

arc seg:xy (199.2 363.2) xy (131.9 308.1) width (0.1)

center-xy: (350.5 109.7) radius (295.2)   CCW

This is what it looks like in the Gerber files when written at 2.4, 2.5, and 2.6:

Reading an Arc in the Gerber File

G03 tells you to draw counter-clockwise circular interpolation. I and J define the center point from the first point of the arc. I’ve always found Gerber’s description for arcs to be a little bit of a mystery compared to what PCB Editor displays in Show Element, so I drew the arc with the I and J dimensioned as a visual aid:

Looking back at the chart listing this arc at different accuracies, you can see how a more granular I, J center point will give you the most accurate arc geometry when photoplotted. Basically, “more” is better in the output.

Why am I Emphasizing Arcs?

Even if you do not use curved trace routing, almost all boards today contain shapes, and shape voids are composed of arcs. Now that we understand arcs, let’s look at database units. I’ve put together a chart to show the various design units and accuracies that can be set in PCB Editor, along with what you should use for the artwork decimal place in the Format section of the Artwork Control Form at each accuracy.

From my experience, outputting artwork at less than the database accuracy is a terrible idea. Your vendor will see spacing problems everywhere because data will round down. Outputting the board accuracy has not had reported problems, but the arcs photoplotted will have the most precise geometry and spacing to other objects when using the above-recommended Artwork Formats (consider my single arc illustration to understand the reasoning).

How do Problems Happen?

PC boards are usually set up in Mils or Millimeters and PCB Editor defaults the design accuracy to a limit that is manufacturable using artwork as the media for either. It is possible to increase accuracy beyond those listed above. For board design, the variable drawing_4mils allows greater accuracy, but it comes with this caution:

The “rounding issue” is referring to arcs, and if you set a database to 0.4 Mils, for example, you would need to output artwork at a decimal accuracy of 0.8 Inch, which is not supported in the industry.  If you chose to move beyond 2 Micron, then you will have the same problem. Artwork will not be guaranteed.

Attempting to output artwork from a Micron database with accuracy 3, the database will issue the following message suggesting alternative output media:

Understanding Data Storing in the PCB Editor to Prevent Problems

While some CAD systems have an underlying unit and only display information about the data at the unit set, PCB Editor stores all data at the actual unit and accuracy, except for the arc center. The arc center is not a physical part of the object, which allows it to be stored as a floating-point number. And that explains why outputting at the database accuracy +1 is advised. This also means that if you decide to change the unit, all data will convert to the new unit. Increasing accuracy after parts are placed will not move the pins to a finer grid if they were already placed at a lesser accuracy. Reducing accuracy or changing the unit itself will cause all data to round to the changed unit/accuracy. If you do any unit and/or accuracy change, I strongly recommend refreshing all symbols and then updating all shapes so that your data is where you want it and not rounded down.

Tired of reading this? I am almost finished.

The point of this blog is to help you understand the relationship of the database to the output data. “Set up your units and accuracy based on what you are building” and set the appropriate format for the artwork output. This will prevent problems when you are ready to fabricate that design. My last thought, if you do output at 0.6, you should check with your vendor to make sure they are now able to process Gerber artwork at this accuracy. Three years ago, this was not part of the standard.