Creating the Gerber and NC Drill Files

pcbmilling.com

Now let's create the Gerber and NC drill files using the PCB layout program.

checkmrk.gif (3142 bytes) For Gerber files, create one file for each layer of your board.

For this example, files were created for the top layer, bottom layer, and the board outline. The files contain only track and pad data. In your project, do not include "extraneous" information such as silkscreen or soldermask data in the files. In this tutorial, the board files were created with the demo version of Ivex Winboard. Due to certain limitations in the program, comments and dimension information were placed on the solder (bottom) layer. Prior to board fabrication, this information would be deleted, anyway, since it resides outside of the actual board area. If your layout program supports additional layers (such as mid or mechanical layers), place all comments on layers other than the top, bottom, and board outline layers.

It should be pointed out that, although this tutorial mentions the use of photoplots and photoplotters when discussing Gerber files, photoplots are not used in the board fabrication process. The machine's software reads the Gerber and NC drill FILES directly and converts them to the appropriate milling and drilling data.

Specifying the Gerber setup information is not as confusing as you might assume. Let's look at the setup data used for the tutorial files:

ger_set.gif (11613 bytes)

First and foremost, the format selected is RS-274X. If your layout program supports RS-274X use this option when creating your files! In the old version of RS-274 (known as RS-274D), aperture files were created separately from the actual layer data. The aperture information had to be manually entered or separately processed before the photoplots could be produced.

The aperture information for this tutorial is shown in the list in the bottom portion of the screen capture. The D codes (known as draft codes in Gerber parlance) represent the various track and pad widths. For example, look at the first line of data for code D10. This is the draft code information that relates to the 1 mil track width for the board outline information. The shape "C" means that a circular aperture will be used. The size of the circle is 1 mil in the X dimension and 1 mil in the Y dimension. The orientation is 0 degrees (no rotation is specified). The mode "D" means that the aperture is "drawn" during the photoplot process. When the 1 mil track is drawn, the light source on the photoplotter is turned on and the 1 mil aperture is moved to the coordinates specified in the board outline file (more on this later). The track is thus "drawn" by this process. Now look at the entry for D16. This is the aperture information for the surface mount component pads. The shape "R" stands for rectangular. The size is 62 mils by 62 mils (or 62 mils square). The mode "F" means that the aperture is "flashed." The photoplotter moves the aperture to the specified coordinates and "flashes" the light source to produce the aperture. Since the surface mount component has two pads, two flashes occur.

checkmrk.gif (3142 bytes) The distinction between drawn and flashed apertures is extremely important for boards produced by some milling machines.

Some machine software packages allow different levels of milling around pads and tracks. For example, a flashed component pad may be milled with 30 mils isolation while a drawn track would be milled with only 11 mils isolation. Why is this important? The 30 mils isolation around pads makes it easier to solder the component leads without accidentally bridging across to nearby (residual) copper. Frequently, users try and "doctor up" pads at the last minute to increase their size or alter their shape by placing tracks on top of the pad. Don't do this! If you do, the software used to process your files will see that a track is present and only produce 11 mils isolation around the modified pad.

Let's now look at the other options in the setup screen. Units of inches are normally specified for files processed in the USA. Absolute and relative coordinates effect the actual content of the files. In the absolute mode, coordinates are specified for every pad and every track start and stop point. In the relative mode, coordinates are specified for the changes from one location to another. You can use either option when submitting your files although absolute coordinates are preferred. Probably the most important thing you can specify is the data format (referred to as the m.n format). For example, consider a setting of m.n = 2.4. The m=2 value means that the photoplot information can range up to a maximum of 99 inches. The n=4 value means that the information is computed to four decimal places (or 0.1 mils). For Gerber data, the decimal point is inferred based on the data format. The leading/trailing zero suppression option means that the data is "left" or "right" aligned within the maximum data field length of six digits (for 2.4 format). With RS-274X, the selection between leading and trailing zero suppression is not really relevant. Pick one; but know what data format and zero suppression you are using in case you need to make a "sanity check" of your file output. Errors in this selection will mean that the pads and tracks will be too large or too small by factors of ten. If you preview your files with a Gerber viewer program you'll see any errors that might be present. For example, if you specified a 50 mil pad and see a huge circle on the screen you'll know that the data format you selected is wrong.

Next, let's create the NC drill file information.

nc_drl.gif (5761 bytes)

The NC drill information is created in much the same manner as the Gerber data. Notice that the leading/trailing zero suppression options still exists with the same m.n format as the Gerber files. If your CAD program supports decimal formats you may want to use it. Looking for errors is easier with decimal format since the implied zeros and decimal point location don't have to be interpolated.

Home	Back to Tutorial