New Page 1

Protel Bits to AP Circuits Atoms

Now that you've created your PCB it's time to take the leap from bits to atoms. Here's a step by step guide to preparing the board for AP Circuits. If this is your first time, give yourself up to 1 - 2 hours for this process. As you become more experienced, it'll take about ten minutes.

A few Protel notes:

If you shift-select a group of objects, unselect by pressing 'x' then 'a'. Or from the "Edit" menu, "Deselect : all".
Undo is Alt-Backspace, NOT control-Z as us Windows users have come to expect.
Many menu items are context sensitive -- they only show when, for example, the PCB is the active document. If you're looking for a menu item you just knew was there a minute ago, try changing the active document type.

Add Corner Marks

In addition to having you specify the board size, AP Circuits requests corner marks be placed in the corners of the board. Place corner marks as you would any top layer trace. If you have a keepout layer, simply place the corner marks over the keepout layer. The keeput layer simply defines the boundaries of the circuit board. If you use autoroute, all traces are constrained to be inside the keepout layer.

Run Hole Size Editor

Install the Hole Size Editor (holesizeeditorforprotel99se.exe in \\milliserver\resenv\software\Protel99SE). You'll have to quit Protel to do this. Run the hole size editor by selecting "Hole Size Editor" from the "Edit" menu while PCB document is active. You want to be sure you're only using "free" holes from AP Circuits. If you use non-free hole sizes, they charge you $$$. AP Circuits gives enough free hole sizes there's no reason to stray, especially for a prototyping board. Free hole sizes, as well as other info about holes can be found at: http://www.apcircuits.com/resources/technologies/drills.html

Note the hole size is not the size of the hole you will get. You're actually specifying the drill size. Plating the hole reduces it's size. AP Circuits recommends adding .01" to the dimensions of all components to make sure they'll fit in the hole. They should have used the words "drill size" instead of "hole size". I agree with AP Circuits that .042" is a very versatile hole size for things like resistors, LEDs and DIP sockets.

The hole size editor simply reports the number of each sized hole. Unfortunately it doesn't tell you which holes are which size. It's up to you to figure that out.

Create NC Drill File

While your PCB document is active, run the "CAM Manager" by selecting "CAM Manager" from the "File" menu.
NOTE: If you've previously run the CAM Manager, this option will take you to the already completed CAM Output page. Instead you will select "CAM Wizard..." from the "Tools" menu while in the "CAM Outputs" page. They both take you to the "CAM Wizard", which is what you want.
Select "NC Drill" for the kind of file you want to make
Use 2:4 format when asked. If you choose a different format, make sure it matches the Gerber files below.
Select "finish" and you're all done.

Create Gerber Files

Select "CAM Wizard..." from the "Tools" menu. Make sure your "CAM Outputs" page is active.
Select "Gerber" for the kind of file you want to make
Use 2:4 format when asked. More importantly, make sure this matches the NC Drill file above.
Use the default values for the remaining screens. We'll make changes in the next step.

Check Your Work

Make sure your output files look like the tabs pictured here. Some of the default values above may not have been correct, so you may have to change some settings here.
DO NOT SKIP THIS STEP!!!!

Create Output Files

Select "Preferences" under the "Tools" menu and choose a directory to output your CAM files. Don't let the grayed out text make you think this is disabled.
Press F9 to create output files.
It should take a few seconds to create the output files.

Send to AP Circuits

Now it's time to run AP Client. Download and install APCLIENT.ZIP from AP Circuits. If it's your first time, you'll be asked about billing and shipping info, and whether you want to use a Fedex account number, or just have the Fedex cost added to the bill.

Click "Add a Job".

There are lots of screens and options, but only four files and the size of your board are necessary to fully specify a board for AP Circuits. I've only included screen shots for the two screen where you actually have to enter a file. The other screens you either leave blank, or should be equipped to answer without my gentle supervision.
Screen 1: Intro. Nothing you need to do. You don't even need to read the text if you're in a hurry.
Screen 2: Enter a job name.
Screen 3: Order more boards than you think you need. Figure you're going to loose two, give away three, and mangle four. Once you have a board working, you're going to think of five new cool projects for that board. In other words, don't order fewer than 12 or so.
Screen 4: The most reliable means of measuring your board is to go into your PCB screen on Protel, and actually measure the board with the "Measure Distance" command under "Reports". The "Film Size" under the "Advanced" tab of the Gerber output is NOT the board size (I don't know what it is)
Screen 5: Choose P1 service for speedy overnight service.
Screen 6: For your positive top layer, choose the file with the .GTL extension (Gerber Top Layer). For the positive bottom layer, choose the file with the .GBL extension (Gerber Bottom Layer). Use the handy navigator on the right for ease of file selection.
Screen 7: Do not include any negative layers. We avoid negativity here.
Screen 8: Do not include any solder masks. Solder masks are the greenish plastic-like coating on commercial circuit boards.
Screen 9: Do not include any silkscreens. Silkscreens are the text lettering over a board so you know what to place where.
Screen 10: Your Excellon drill file is the .TXT file that's not the "Status Report.txt". Don't confuse the two. Your NC Drill Tool Size File is the .DRR file (Drill Routing Report)

You're all set. Use the built-in FTP functionality to send you completed file directly to AP Circuts.