Run EasyPlot and select the “Setup” option. This can be done before or after you have loaded your PCB file.

Next Select the “Gerber” option and you will be taken to the “User” adjustable features.

Now select the “Aperture Table”. This item allows you to change the location of the aperture file - drive , directory etc. as well as the name of the table. It’s usually defaulted to the drive and directory where the program resides. In the event that the path name is too long to display you will see the drive letter and the aperture file name only. The “@” sign simply indicates that the path is too long to display.

In this example, after pressing “enter” on the aperture line and providing a path, the files “Extended.apt” and “Standard.apt” were located in the target folder. The “extended.apt” was selected for this session by using the key board arrows then pressing enter to select.

After selection of the aperture file our status line now reflects the change. You can repeat this similar selection procedure for each option you wish to change. The “output file” location will default to the same location you loaded your PCB file from. If you wish to change this, after loading the PCB file, return to this setup menu and redirect the output file location to one of your choosing. Remember that the path and folder must be valid as EasyPlot will not create new folders. This must be done beforehand.

The “OPTIONS” menu contains additional features worth investigating. Such as batch mode plotting and what should be contained in the Gerber output. Just as a point of interest the G54 option is not required on modern raster plotters. If your vendor uses an older style vector plotter you may have to turn this feature on. It’s a command for the vector plotter’s shape wheel to change. Modern laser plotters ignore the G54 as it’s not necessary. AP Circuits uses a GSI Raster Plotter and G54 can be left in the “off” position.

The options menu allows you to set batch mode plotting (all layers are done during the same generation session). Normally you want all items except for the title block to the ON position. Leaving any of these off will result in the absence of the off item in your Gerber files. For reference “Strings” are text items.

If you needed pilot holes for hand drilling, should you elect to make boards at home or in your office lab, setting the “Pad Hole Guide Size” will create a donut so you can find the pad center easier. This should ALWAYS be left at ZERO if you are sending your boards to APC.

The Drill Draw Symbol Size is used to create a drill location drawing if needed. The symbol size should be about 30 to 50 mils to make for an easier read. Normally this output is not needed for fab shops that can use NC drill files but if you are making them yourself it can be used for an overlay so you can identify hole sizes at each pad location.

'Solder Mask Enlargement' is used to create over sizes of your pads on the solder mask layer. Leaving this set to 0 creates pads of the same size on your solder mask layer. Most board shops, including ours, would prefer this left to actual size so that we can adjust the swell to best accommodate in-house processes.

After selecting the Flip Layer Setup option please make sure that all items are set to “Normal” , The alternate setting will mirror the layer, you may need to do this for home or lab projects, but don’t mirror the outputs for fab ships. Also if you are making printed check plots, you may find that a mirror of the bottom layer will make inspection easier. Don’t forget to set it back to normal before outputting to Gerber.

This next section describes how to setup “Batch Mode” plotting which creates all of the Gerber outputs during the same session (recommended). From the main setup menu select “Batch Mode” and press enter. The next menu provides toggles for each of the layers you want to be included in the batch. Pretty straignt forward, what’s on is included and what’s off is not.

For the AP Circuits P1 or proto type service you only need the top and bottom layers on. The AP Circuits P2 or production service allows for masking options, if you need them then you need to turn on the mask options for the required files.

Overlay is the Component Legend which shows your part numbers and part outlines. Note: if for what ever reason you laid your signal layers out on layers other than the top or bottom, you will need to turn on those layers (the mid layers for example). The Plane layers are power and ground planes and are solid copper except where you have placed a trae or pad, any item you can see on a plane layer is clear and the rest is solid (it’s a negative image) and plane layers are usually used for multi layer production which AP Circuits does not provide as yet.

Just in case you have not loaded in your PCB file yet this group of pictures shows you the process. Leaving the Setup menu (pressing the <esc> key) takes you back to the main menu where you load your File. Select File then Load followed with the drive and folder/path for the file location. You will then be at the file selection screen (below) where you can select the desired PCB file.

After the proceeding sections you are now ready to begin the generation process. From the Main Menu select Gerber Plot (you must have your file loaded before accessing this menu). You will then be prompted to proceed (screen shot below), examine the parameters (in red) to ensure that the desired aperture file is loaded and the output path is ok (this is where your files will be written) as well as the Plotting Mode - Batch was selected for this run. To continue select YES.

Instruct the generation process to match shapes automatically and No to paint match confirmation and set Fills to automatic

Should you come across a shape that is not in the aperture file the process will pause and ask you to pick an alternate shape, paint matching will draw the item as best as possible provided the shape and size are with in reason. In this case a relief pad is not matching and they are not used anywhere on the layout so I’ve selected a paint match to pacify the program. You may also encounter the match progam sending the error message “Abort Process” while it’s running in a DOS Window. This can usually be resolved by going to a full screen view (usually ALT+Enter)

Finally we get to the NC drill routine. There is not much in the way of setup here. Protel has this hard coded to 2.4 TZ so all you can do is play with the output destination, offsets (usually never needed) and the tool table. The Extended.etl file was used for this example.