Engrave on cast acrylic sheet using 90 degree, spring loaded drag bit
1. Start with a black and white design in svg format. The scale isn't that important, since we can change it later on.
2. Launch Carbide Create with a New File
3. Design tab -> Setup -> Job Setup
a. Enter dimensions of acrylic sheet in Stock Size. Model Resolution is Standard
b. Zero Height is Top
c. Enter desired Thickness(Z).
NOTE: This is NOT the thickness of the acrylic sheet. It should be greater than the Z height required to put the desired pressure on the bit's tip. For example, the bit manufacturer recommends that the bit should be compressed 0.25 inches to apply the optimum pressure on the tip. Since the top of the acrylic surface represents Z=0, we will fool the program into compressing the bit by telling it we want a 0.25 inch depth of cut. Therefore, the Stock Thickness should be greater than 0.25 inches. I selected 0.5 inches.
d. Toolpath Zero is Lower-Left
e. Material is Acrylic
f. Machine doesn't matter, but I selected Shapeoko XXL
g. Retract Height = 0.2 inches
h. Units are Inch, which is just my preference
4. Import the design into Carbide Create (Design -> Import)
a. Apply Transforms as necessary. I found that the Group Vectors transform was necessary in some cases to keep the program from messing up other transforms.
5. Unless you have a reason to believe that you'll need to operate on different parts of the desing, select the entire design before switching to the Toolpaths tab. This is easier to do under the Design tab.
6. NOTE: Carbide Create doesn't have a concept of a drag bit, so we'll have to fool it when we create a new definion.
a. Edit -> Show Tool Database to bring up the Select Tool dialog box
b. Machine is All and Material is Acrylic
c. Click New Library button to bring up the Create New Library dialog box
d. Material is Acrylic, Machine is Shapeoko, and Library Name is your choice
e. Back to the Select Tool window, right-click on the name of the library you just created and select New Tool -> Vee Mill -> Inch
f. In the Edit Tool window that just popped up, various parameters need to be filled in based on the drag bit you have.
1) Tool Information -> Name. I chose Drag Bit
2) Geometry -> Diameter. This will be the diameter of the tip. In my case, it was 0.005 inches
3) Geometry -> Included Angle. In my case, this would be 90.0
4) 2D Speeds and Feeds
a) Feedrate. The bit manufacturer recommended 20 in/mm
b) Plungerate. I chose to set it to the same as the Feedrate, but others have used lower values (with higher Feedrates).
c) RPM. Drag bits are not supposed to rotate at any speed, so this should be set to zero. Be sure that your CNC understands that zero means no rotation.
d) Depth (of cut). Since we want the bit to make just one pass, we set this to the desired depth of cut we chose in 3.c. (0.25 inches).
5) 3D Speeds and Feeds
a) Stepover. It should be the same as the tip Diameter (0.005, in my case). Set the percenter to achieve that figure.
g. Back to the Select Tool box, click OK to close it
h. Switch to the Toolpaths tab and click the Pocket button.
1) Change the Tool to the drag bit by clicking the Edit button.
a) You will probably need to change the Stepover to the desired one.
2) Cutting Depth -> Start Depth should be zero
3) Cutting Depth -> Max Depth should be 0.25 inches
i. Once you click OK on the Pocket Toolpath dialog, the program calculates the time the operation will take. The Show Simulation button will preview the toolpath, although it is a false picture, since the program thinks it is actually cutting to a depth of 0.25 inches when it is really just scratching the surface.
j. If the pocket toolpath was insufficent to cover the entire area of the path, you might need to lower the stepover or try adding a contour path.
1) Click the Contour button
2) Fill in the same values for Tool and Cutting Depth
3) Toolpath Settings -> Offset Direction is Inside Left
k. Once you click OK, the program will add that toolpath to the Group and perform similar calculations.