Shapeoko CNC Machine

We currently have 2 Shapeoko CNC machines in the smaller room within the Loud Noise room. The smaller Shapeoko is typically used for the Robot Portraits demos. The larger Shapeoko was recently fixed, and a SOP is currently in progress.

The steps to use the Shapeoko machines are similar to the CNC Machine Operation Steps, although that page documents the process to use the old CNC machine that is no longer at the space.

Using Shapeoko with Freecad

Shapeoko provides software for creating 2.5D toolpaths (gcode) called Carbide Create. It also has a gcode sender called Carbide Motion. Freecad, and open source cad package, also has CAM functionality to create toolpaths. It has both 2.5D and 3D capabilities. These instructions are tested with Freecad 1.0.

1. Create your part in freecad, import a step file, or follow along with the example file. Media:Example.FCStd
2. In the Model window, select the base object of your document. Change the unit system to Metric small parts & CNC.
3. Switch to the CAM workbench
4. In the CAM menu, open the Toolbit Library Editor. Select a location for your library and let Freecad create the required folders
5. In the Toolbit Library Editor, use the button on the left to create a new tool table
6. Create the tools you will use to do your work. AHA has a ball and square end mills in 1/4", 1/8", and 1/16" sizes, as well as a .25" V bit. You only need to create the tools you will actually use.
   1. Select a fcstd file to act as the prototype for your tool. Then create a file that will hold the details for your particular tool.
   2. Double click on your new tool to specify its details. The diameter is critical, but the others are less important. If you are using the example file, you will need a .25" V bit, and .25" and .125" end mills.
   3. Close the tool library
7. Click the Job button to create a job. Select the body that will be machined
8. Set the size of your stock. Then set the zero of your coordinate system. You may choose anywhere, but good choices are the corner of the stock or the corner of your part.
9. In the Output tab, select the GRBL postprocessor. Add the --translate_drill command line option if you will be using a drill in your part
10. Use the Tools tab to add some tools to your job. Detour to https://shapeokoenthusiasts.gitbook.io/shapeoko-cnc-a-to-z/feeds-and-speeds-basics for information about speeds and feeds. The router on the shapeoko is adjustable from about 11,000 to 30,000 RPM
11. Click OK to set up the job.
12. Select the Setup Sheet for your Job in the Model window. Under Tool Controller, set Horiz Rapid and Vert Rapid to at least 2000mm/min
13. Go through your tools in the Model window and select speeds and feeds for each.
14. If you are machining something like MDF or Plywood, there is a good chance that the thickness of your finished part is the same as the thickness of your stock. You will not need a facing operation.
15. If your stock is thicker (z height) than your finished part, you will need a facing operation.
    1. Select the top face of your part, then click the Face button.
    2. Select your largest square endmill as the tool to use. Using other tools will result in much worse surface finish.
    3. Select Stock as your Boundary Shape to bring your entire stock down to the correct z-height
    4. Click Apply to generate and display the proposed toolpath
    5. Adjust stepover and stepdown with information from the speeds and feeds webpage, or from a reference table that someone at AHA should create.
    6. Click OK when you are happy with the path
    7. Click the eye next to the Mill Face operation to reduce visual clutter
16. To create a helix operation for round holes that are a larger diameter than your router bit, click the Helix button. All appropriate geometry will automatically be selected. Adjust any settings you need to, and press Apply to inspect the tool path.
    1. For holes close to the radius of your tool, you will see a single helix with a circle on the bottom to mill the bottom of the hole flat.
    2. For wider holes, you will see several helixes that work to clear out all of the material of the hole. If this hole will cut all the way through your stock, you should switch the Start From setting to inside so that a piece of your stock isn't cut free in a way that could send it flying.
    3. If you have multiple holes with different depths, you must create a different helix operation for each depth. Unchecking the appropriate box under Base Geometry is insufficient. You must remove the geometry using the Remove button.
    4. For through holes, adjust Final Depth to OPFinalDepth - 1mm to make the tool cut all the way through the stock.
    5. Adjust the Cut Pattern as desired.
    6. Click OK to accept the operation
    7. You may select the operation and change the Label to be more descriptive
    8. If you need to change tools, the automatic feature selection will not work. You will have to select the correct feature manually
17. To create a pocket
    1. For blind pockets (that do not go through your stock completely), select the bottom of the pocket(s)
    2. For through pockets, hold down control and select the walls of the pocket(s)
    3. Select Pocket Shape from the toolbar
    4. Adjust the Cut Pattern as desired.
    5. Just like the Helix operation, you cannot combine pockets with different depths
    6. For through holes, adjust Final Depth to OPFinalDepth - 1mm to make the tool cut all the way through the stock.
    7. Click OK to accept the operation
18. To create a counter sink or other 3D operation
    1. Go to edit-->Preferences --> CAM --> Advanced
    2. Select Enable OCL dependent features and restart Freecad
    3. Use the dropdown menu attached to the 3D pocket button and select 3D surface
    4. Change settings as needed. In particular Cut Pattern should be circular or offset for a circular feature.
19. Cut your part out from the stock
    1. Select the outside edges of the your model and select Profile from the toolbar
    2. Make sure that Cut Side is outside
    3. Select OK, then select the profile in the Model window.
    4. Select the CAM --> Path Dressup --> Tags
    5. Adjust settings to get tags that will hold your piece to the stock while it is machined
20. Dressup any other paths that are required.
    1. In particular, Pocket Shape operations can be modified with the Ramp Entry Dressup. You can Change the Ramp Method to Helix to create an operation that moves continuously down
21. Double check all of the operations you have created to be sure you are happy with them. Then use the CAM Simulator or New CAM Simulator button to view what will happen.
22. Post Process your Jobs
    1. I haven't figured out to incorporate tool changes into the gcode.
    2. Adjust the order of your operations to use the same tool back to back to reduce the number of tool changes required.
    3. Decide which tool you will use first. Go to all of the other operations in the Model window. For each, in the Data window, switch Path --> Active to False
    4. Press the Post Process button and export the gcode for the first tool. Save the file with a .gcode extension instead of a .grbl extension
    5. Repeat steps 3 and 4 for every tool you will use.
23. Load your files into carbide motion and cut your piece!