Part Two: Generating Gcode
At this point, your drawing probably looks something like this:
Now it’s time to tell the computer that we want to cut this part out. We are first going to tell the computer to cut out the inside piece, and then to cut around the outside.
Click on the inner rectangle to with the cursor tool. It will turn red when it is selected. With the inner circle selected, click on the “CAM” tab, and then click on the “Profile Operation” option.
This will open a new window with a LOT of options.
This can be a little bit intimidating, but you will pick it up quickly.
The first setting is “tool diameter.” I will be using a 1/8th inch end mill so I’m going to put .125 (⅛ = .125) in here.
Next is “target depth”. This sets how deep the cut will go. I am using ¼ inch plywood but when I measured it’s thickness using calipers I found that it was really only .2 inches thick so I’m going to set the “target depth” to .21 inches.
Next is “inside/outside”. This asks if you want to cut along the inside of the line, or along the outside. We want to cut along the inside.
“safety height” sets how high the tool will lift out of the material when moving between cuts. ½ inch is a lot, so I’m going to set the safety height to .25 inches.
“stock surface” is confusing. We don’t need to worry about it right now. You can just leave it at zero.
“step down” sets how deep the machine cuts with each pass. The lower the step down is, the cleaner and more accurate the cut will be, but the longer it will take. I’m going to set the step down to .03 inches.
The feed rates set how fast the machine will cut. We can leave both of those on the defaults.
When you are done, the window will look something like this:
Click “OK” to close the window.
Now we need to tell the computer to take all that information and generate tool paths from it. To do this click “CAM” -> “Calculate All”.
You should now see the tool’s path appear inside of the inner rectangle like this:
Now click on the outer rectangle and repeat the process. All of the settings will be the same, except that this time we are going to cut on the outside.
Click “OK” and then generate the tool paths again. You should now see two sets of tool paths.
At this point, you could save your gcode and cut the part out, but there is one more thing that we are going to do. When the cut finishes, the part has a tendency to break free. We are now going to add “tabs” which will hold the piece in place.
I usually don’t use tabs because when you cut them off you can usually still see where they were. Instead I usually use a pencil to hold the piece in place as the cut finishes, but I want to show you how to add tabs so you have the option.
To add tabs, select the tool path around the outer rectangle and then click “CAM” -> “add tabs to selected”. The only way I was able to reliably select the tool path was to draw a very small rectangle around a section of it.
Next, this window will open:
We really only need two tabs to hold the piece in place so I will set the tabs spacing to 3 inches (because 5 inches only gave me one tab). The tab height sets how thick the tabs holding the piece in place will be. Set the tab height to .1 inches because we don’t need the tabs to go all the way to the top of the wood.
Clicking “OK” will add two blue rectangles to the outside of the larger rectangle. These represent the locations of the tabs.
Drag the tabs to a more logical places by clicking on them and dragging.
Now we are ready to save the file. First click “CAM” -> “calculate all” to regenerate the gcode to make sure it is up to date. Then click “CAM” -> “export gcode”
You will see this window open:
This will only save the selected toolpaths, so make sure you select all of them. You can use the “all” button. Then click “Export Selected Toolpaths” and save the file somewhere you can find it again.
Congratulations you just designed your first thing, and generated the code to cut it out. Good work!
Click here for the next step.