Phase 1: Step 1

Download the drawing package from the files section. Print them out - it will be easier to mark off dimensions as you enter them.

Phase 1: Step 2

Determine your router's constraints. Write the following information down:

1. Tool diameter you want to use
2. Cutting edge configuration (straight/spiral, 1/2/3/4 flute)
3. Max spindle speed
4. Working area

Phase 1: Step 3

Calculate parameters:

1. Max Depth of cut is 1x tool diameter for straight flute cutters, 0.5x tool diameter for spiral cutters. (Reduce this if you want to "ease in" on your first attempt.)
2. Feed Rate is .0254mm x spindle speed x number of flutes (DO NOT REDUCE THIS. If the feed rate scares you, reduce spindle speed and recalculate, or reduce depth of cut.)
3. Write down the max length and width of the area you can cut and reduce this by 4 x the diameter of your cutter in each direction. Make sure no parts are longer than this.

Phase 1: Step 4

Prepare drawings:

1. Download the drawings for the parts.
2. Print them out so you can look at them while you write the code. This will make it easy to mark off dimensions as you code them.
3. Feel free to redraw the parts in the cad system of your choice! (just be sure to use ONLY lines and circles)

Phase 1: Step 5

Write some Gcode!

1. Learn how to properly initialize your machine. There are plenty of tutorials and explanations of this, but expect to have something like the following string of code at the top of your program: G21 (Units in millimeters) G90 (Absolute programming) G64 (Default cutting) G17 (XY plane) G40 (Cancel radius comp.) G49 (Cancel length comp.)
2. For this process you will assume the edges of the part are at 0,0, and all of your code will be based on the drawing measurements.
3. Look up the G01, G02, and G03 commands. You will be using all of these to code. The first thing to do is code the profile of each part in a clockwise direction. To do this, look at each segment and decide if it is a straight line (use G01), Right hand Circle (G02) or Left hand Circle (G03). Follow the appropriate command with X# Y# [I# J#] where "#" is the appropriate dimension from the drawing. Cross each dimension out on the drawing as you code. Your profile will have the same number of lines of code as there are segments on the profile.
4. Now that you have a profile, you will be using that profile over and over for each layer. There are 2 ways to do this:
   1. Linear: Prior to your profile, plunge your cutter to the first depth by using a G01 Z(depth of cut). Paste your profile code. Plunge to the next depth, paste your profile code, repeat until you get to the bottom of your part. Retract at the end.
   2. Programmatic: move your profile shape to the end of your gcode file as a subroutine and bound it with a o111 and M99. Then use M98 P111 to call your sub program. Look up the use of M98 to learn how to do this, and it will greatly reduce the overall size of your program, plus make it easy to change your profile shape
5. Add cutter compensation. It is very advantageous to learn to use cutter compensation. The main reason is that your shape will be completely independent of the actual cutter you use. If your cutter is a different size, as long as the tool table on your machine is properly matched to your tool, it will create a good cut! Make sure to add in the proper lead-in moves (research G40, 41, 42).
6. Add safe Z height movements. Make sure that before any x,y move where you are positioning the cutter, there is a separate z move that raises the tool to the safe height.
7. End your file by including codes to shut off the spindle and mists (good practice to keep your code good if you add these features later), raising z to a safe height and placing M30 to signify program end.

Phase 1: Step 6

Simulate and run!

The thing to remember about this Phase 1 is that your machine is going to cut every shape starting at 0,0. This means you need to move the machine's axis well away from the hard stops, but you can generally just bolt a piece of wood down, move the tool to the spot you want to cut it, and hit go.

The best way to simulate is to Load your code on to your controller and view the toolpath that is generated. I use Mach3, which lets you step through every line of code and highlights the movement on the screen.

Next, you want to run your machine without cutting anything. Set your machine's z=0 height up enough that the tool won't hit anything and run the program in air. Another popular safe trial is to cut Styrofoam first.

If everything ran fine, clamp down some wood and go.